AERO-S 1.1

Short Contents

AERO-S
1 INTRODUCTION
2 INSTALLATION
3 ACOUSTIC TIME-DOMAIN ARTIFICIAL BOUNDARY *S*
4 ACOUSTIC TIME-DOMAIN DIRICHLET BOUNDARY CONDITIONS *S*
5 ACOUSTIC TIME-DOMAIN DISTRIBUTED NEUMANN BOUNDARY CONDITION *S*
6 ACOUSTIC TIME-DOMAIN NEUMANN BOUNDARY CONDITIONS *S*
7 ACOUSTIC TIME-DOMAIN ROBIN DISTRIBUTED BOUNDARY CONDITION *S*
8 ACTUATORS *S*
9 AEROELASTICITY
10 AEROHEAT
11 ATTRIBUTES *S*
12 BEAM OFFSET
13 BEAM REFERENCE FRAMES
14 BINARY INPUT / OUTPUT
15 BOUNDARY CONVECTION *S*
16 BOUNDARY DISPLACEMENTS *S*
17 BOUNDARY FLUXES
18 BOUNDARY FORCES *S*
19 BOUNDARY TEMPERATURES *S*
20 BUCKLING
21 CLUSTERING SNAPSHOTS OR CONSTRUCTING A REDUCED BASIS
22 COMMENTS
23 COMPOSITE (OR ORTHOTROPIC SHELL OR ANISOTROPIC SOLID)
24 COMPOSITE (ORTHOTROPIC SHELL OR ANISOTROPIC SOLID) ELEMENT FRAMES
25 CONDITION NUMBER
26 CONSTRAINTS
27 CONSTRUCTING A REDUCED MESH
28 CONTACT SURFACES
29 CONTROL STATEMENT
30 CONWEP
31 DENSITY-TEMPERATURE TABLE
32 DISCRETE NODAL MASS AND INERTIA
33 DYNAMIC ANALYSIS
34 EIGENVALUE PROBLEMS
35 ELEMENT TOPOLOGY *S*
36 ENABLING REDUCTION AND HYPER REDUCTION USING LOCAL REDUCED-ORDER BASES
37 END
38 EQUATION SOLVER CONFIGURATION
39 FIELD WEIGHTS FOR MESH DECOMPOSITION
40 FLUID/STRUCTURE INTERFACE
41 FORCE TIME TABLE-MECHANICS AND ACOUSTICS
42 GEOMETRIC RIGID BODY MODES
43 GEOMETRIC STIFFENING DUE TO PRESTRESS
44 GLOBAL SIMULATION PARAMETERS
45 GRAVITATIONAL ACCELERATION
46 GROUPS
47 HEAT CONDUCTION COEFFICIENT-TEMPERATURE TABLE
48 HEAT ZERO ENERGY MODE
49 HEAT ZERO ENERGY MODES FILTER
50 HELMHOLTZ
51 HELMHOLTZ ANALYSIS (AXISYMMETRIC/PARTIALLY AXISYMMETRIC)
52 HELMHOLTZ ARTIFICIAL ABSORBING BOUNDARY CONDITIONS *S*
53 HELMHOLTZ ARTIFICIAL ABSORBING BOUNDARY CONDITIONS (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) *S*
54 HELMHOLTZ AUXILIARY SURFACE FAR-FIELD PATTERN (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) *S*
55 HELMHOLTZ CONSTRAINED FICTITIOUS NODES (PARTIALLY AXISYMMETRIC) *S*
56 HELMHOLTZ DIRICHLET BOUNDARY CONDITIONS *S*
57 HELMHOLTZ DIRICHLET BOUNDARY CONDITIONS (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) *S*
58 HELMHOLTZ DISTRIBUTED NEUMANN BOUNDARY CONDITION *S*
59 HELMHOLTZ FAR-FIELD PATTERN (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) *S*
60 HELMHOLTZ LINEAR MULTIPOINT CONSTRAINTS
61 HELMHOLTZ LINEAR MULTIPOINT CONSTRAINTS (PARTIALLY AXISYMMETRIC) *S*
62 HELMHOLTZ LOCATIONS WHERE TO COMPUTE THE KIRCHHOFF INTEGRAL
63 HELMHOLTZ NEUMANN BOUNDARY CONDITIONS *S*
64 HELMHOLTZ NEUMANN BOUNDARY CONDITIONS – FICTITIOUS DOMAIN (PARTIALLY AXISYMMETRIC) *S*
65 HELMHOLTZ NEUMANN BOUNDARY CONDITIONS – REAL DOMAIN (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) *S*
66 HELMHOLTZ NODES BELOW AUXILIARY SURFACE (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) *S*
67 HELMHOLTZ SCATTERER BOUNDARY *S*
68 HELMHOLTZ WAVE NUMBER (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) *S*
69 HELMHOLTZ WET INTERFACE BOUNDARY *S*
70 HYDROELASTIC FLUID/STRUCTURE BOUNDARY
71 HYDROELASTIC FREE SURFACE BOUNDARY
72 HYPER REDUCTION OF THE INERTIA FORCES ASSOCIATED WITH A CONSTANT MASS MATRIX
73 IMPEDANCE ANALYSIS
74 INITIAL ACCELERATIONS (Not Supported Yet)
75 INITIAL DISPLACEMENTS *S*
76 INITIAL DISPLACEMENT 6 COLUMNS (IDISP6 completely spelled out) *S*
77 INITIAL OR SEED DISPLACEMENT FOR PITA (IDISP6PITA completely spelled out)
78 INITIAL OR SEED VELOCITY FOR PITA (IVEL6PITA completely spelled out)
79 INITIAL TEMPERATURES *S*
80 INITIAL VELOCITIES *S*
81 INTRUSIVE POLYNOMIAL CHAOS
82 LINEAR MATERIAL PROPERTIES *S*
83 LINEAR MULTIPOINT CONSTRAINTS FOR MECHANICAL ANALYSIS
84 LOAD
85 LOADCASE DEFINITION
86 LUMPED
87 MASS EVALUATION
88 MATERIAL LAW
89 MATERIAL LAW USAGE
90 MESH DECOMPOSITION
91 NODAL CONTACT
92 NODAL FRAMES
93 NODES *S*
94 NON INTRUSIVE POLYNOMIAL CHAOS
95 NONLINEAR ANALYSIS
96 NONLINEAR SUPERPOSITION OF RIGID AND DEFORMATION MODES
97 OUTPUT OF RESULTS (OUTPUT completely spelled out)
98 OUTPUT OF RESULTS 6 COLUMNS (OUTPUT6 completely spelled out)
99 PARALLEL-IN-TIME ALGORITHM (PITA)
100 PRELOAD
101 PRESSURE
102 PRINTMAT
103 QUASISTATICS ANALYSIS
104 RANDOM
105 READING REDUCED BASES
106 RECONSTRUCTING THE SOLUTION FROM THE REDUCED COORDINATES
107 RENUMBERING
108 RESTART
109 RIGID BODY (AND OTHER ZERO ENERGY) MODES
110 RIGID BODY MODES FILTER
111 RUBBER DAMPING PROPERTIES TABLE
112 SAVING EIGENMODES OR PROJECTING ONTO A BASIS
113 SENSITIVITY ANALYSIS (SENSITIVITY completely spelled out)
114 SENSORS *S*
115 SLOSHING PROBLEMS
116 SLOSHING ZERO ENERGY MODE
117 SOURCE TIME TABLE-HEAT CONDUCTION
118 SPECIFIC HEAT COEFFICIENT-TEMPERATURE TABLE
119 STATICS
120 STRESS-STRAIN ONE-DIMENSIONAL TABLE
121 STRESS-STRAIN TWO-DIMENSIONAL TABLE
122 STRUCTURAL DAMPING LOSS FACTOR TABLE
123 SURFACE TOPOLOGY
124 THERMAL EXPANSION TEMPERATURE TABLE
125 THERMOELASTICITY
126 TIED SURFACES
127 USER DEFINED FORCES *S*
128 USER DEFINED PRESCRIBED DISPLACEMENTS *S*
129 WEIGHTS
130 YOUNG MODULUS-STRAIN TABLE
131 YOUNGS MODULUS-TEMPERATURE TABLE
132 YIELD STRESS-EFFECTIVE PLASTIC STRAIN TABLE
133 YIELD STRESS SCALING FACTOR-EFFECTIVE PLASTIC STRAIN RATE TABLE

AERO-S

1 INTRODUCTION

This section compiles basic information on how to prepare an input data for a finite element analysis using the AERO-S code, and how to run this code.

The input data consists of command macros, clustered numerical data, and comment lines. Each data cluster is preceded by a command statement. The following rules of thumb are suggested:

1	The users are allowed to have as many comment lines as they wish, as long as the first column of each line starts with * (see COMMENTS).
2	The subsequent data clusters may appear in any order. The command statement preceding each cluster may be in lower, upper, or mixed characters.
3	The data in each cluster are free format.
4	Only the first four letters of a command need to be specified unless otherwise noted.

INCLUDE filename (or "filename")

where filename is the name of the file containing the information. "filename" can contain a path or can be replaced by <filename> in which case the path is that of the environment variable \$FEM\_INCLUDE. Furthermore, the included file filename can be compressed by gzip, bzip2, or zip.

	[`-d <decomposition_pathandfilename>`]	(Specifies a decomposition file).
	[`-v <verbose_frequency>`]	(Turns on verbose and specifies frequency of printing on screen the FETI iteration count and subspace iteration count).
	[`-c`]	(Outputs contact status on screen (FETI solver)).
	[`-t`]	(Converts input file to XPost format).
	[`-T`]	(Converts input file to XPost format after removing all numbering gaps).
	[`-m`]	(Converts input file to XPost format after gathering each material in a separate element set).
	[`-M`]	(Converts input file to XPost format after removing all numbering gaps and gathering each material in a separate element set).
	[`-P`]	(Generates automatically XPost patterns for the various XPost element sets. This option is useful only in conjunction with the -m and -M options which can generate multiple XPost element sets. Also, automatically generates a global element set).
	`<filename.aeros.aicdf>`	(AERO-S ASCII Input Command Data file containing the finite element structural model and analysis commands).

The command line for executing AERO-S in parallel mode on a shared memory system using OpenMP and number_of_threads threads is

	[`-d <decomposition_pathandfilename>`]	(Specifies a decomposition file).
	[`-v <verbose_frequency>`]	(Turns on verbose and specifies frequency of printing on screen the FETI iteration count and subspace iteration count).
	[`-c`]	(Outputs contact status on screen (FETI solver)).
	[`-t`]	(Converts input file to XPost format).
	[`-T`]	(Converts input file to XPost after removing all numbering gaps).
	[`-m`]	(Converts input file to XPost format after gathering each material in a separate element set).
	[`-M`]	(Converts input file to XPost format after removing all numbering gaps and gathering each material in a separate element set).
	[`-P`]	(Generates automatically XPost patterns for the various XPost element sets. This option is useful only in conjunction with the -m and -M options which can generate multiple XPost element sets. Also, automatically generates a global element set).
	`<filename.aeros.aicdf>`	(AERO-S ASCII Input Command Data file containing the finite element structural model and analysis commands).

The command line for executing AERO-S in parallel mode on a distributed system using MPI with number_of_MPI_processes MPI processes [and number_of_threads_within_an_MPI_process threads within an MPI process] is

mpirun -np number_of_MPI_processes aeros -n number_of_threads_within_an_MPI_process

	[`-d <decomposition_pathandfilename>`]	(Specifies a decomposition file).
	[`-v <verbose_frequency>`]	(Turns on verbose and specifies frequency of printing on screen the FETI iteration count and subspace iteration count).
	[`-c`]	(Outputs contact status on screen (FETI solver)).
	[`-t`]	(Converts input file to XPost format).
	[`-T`]	(Converts input file to XPost after removing all numbering gaps).
	[`-m`]	(Converts input file to XPost format after gathering each material in a separate element set).
	[`-M`]	(Converts input file to XPost format after removing all numbering gaps and gathering each material in a separate element set).
	[`-P`]	(Generates automatically XPost patterns for the various XPost element sets. This option is useful only in conjunction with the -m and -M options which can generate multiple XPost element sets. Also, automatically generates a global element set).
	`<filename.aeros.aicdf>`	(AERO-S ASCII Input Command Data file containing the finite element structural model and analysis commands).

2 INSTALLATION

The installation of AERO-S on a given computing system requires the availability on that system of the following tools:

`C++` compiler `g++`	Version 4.1.2 or higher.
`Fortran` compiler `gfortran`	Version 4.1.2 or higher.
`Flex` utility	Version 2.5 or higher. `Flex` is a lexical analyser required for building the parser of AERO-S's input command data file.
`Bison` utility	Version 2.3 or higher. `Bison` is a parser generator required for building the parser of AERO-S's input command data file.
`CMake` utility	Version 2.6 or higher. `CMake` is a cross-platform open-source build system. It is comparable to the Unix `Make` program in that the build process is ultimately controlled by configuration files (`CMakeLists.txt`). However unlike `Make`, it does not directly build the final software but instead generates standard build files such as makefiles for Unix and projects/workspaces for Windows Visual C++. The `CMake` version 2.6 utility can be obtained from http://www.cmake.org. (Note: a “README.cmake” file discussing details on `cmake` options for code configuration and installation is available in the directory containing the source code of AERO-S).

`BLAS` library	`BLAS` is a set of Basic Linear Algebra Subprograms required by various operations performed in AERO-S.
`LAPACK` library	`LAPACK` is a high-performance Linear Algebra PACKage with advanced solvers.
`MPI` library `openmpi`	Version 1.2.6 or higher. `Open MPI` is a high-performance implementation of the Message Passing Interface (MPI) required for performing interprocessor communication, among others. More specifically, AERO-S requires an MPI-2 implementation such as the one provided by the Open MPI project.
`OpenMP` API	Open Multi-Processing is an Application Programming Interface (API) that supports multi-platform shared memory multiprocessing programming in C, C++ and Fortran on many architectures, including Unix. As an option, AERO-F can be compiled with `OpenMP` to enable multi-threaded execution.

In addition, the following optional libraries extend the capabilities of AERO-S:

`SPOOLES` library	`SPOOLES` is a library for solving sparse real and complex linear systems of equations with a sparse direct solver, written in the C language using object oriented design.
`MUMPS` library	`MUMPS` is a library for solving sparse real and complex linear systems of equations with a multifrontal massively parallel sparse direct solver.
`SUPERLU` library	`SUPERLU` is a general purpose library for the direct solution of large sparse nonsymmetric systems on high performance machines.
`ARPACK` library	`ARPACK` is the Arnoldi PACKage for the solution of large-scale symmetric, nonsymmetric, and generalized eigenproblems.
`ScaLAPACK` library	`ScaLAPACK` is also known as the Scalable LAPACK. This library includes a subset of LAPACK routines redesigned for distributed memory MIMD parallel computers.
`BLACS` library	`BLACS` (Basic Linear Algebra Communication Subprograms) is a linear algebra oriented message passing interface designed for linear algebra.
`PARPACK` library	`PARPACK` is the parallel version of `ARPACK` used by AERO-S's parallel eigensolver.
`METIS` library	`METIS` is a library of graph manipulation routines that can be used by AERO-S for reordering of a sparse matrix to reduce the number of fill-in entries created during factorization.
`Zoltan` library	The `Zoltan` library includes among other things a suite of dynamic load-balancing and parallel partitioning tools that are used by AERO-S for parallel proximity searches.
`Eigen3` library	`Eigen3` is a versatile C++ template library for linear algebra (vectors, matrices, and related algorithms (see http://eigen.tuxfamily.org)).

The successful completion of the procedure described above leads to the creation in the bin/ directory of AERO-S's executable aeros.

3 ACOUSTIC TIME-DOMAIN ARTIFICIAL BOUNDARY *S*

The ATDARB command statement is used to specify the artificial boundary

\text{[math]}

on which an Antoine absorbing condition is to be applied in the time domain, and the order of this absorbing boundary condition. The input format is given below.

`ORDER`	Order of Antoine's absorbing boundary condition in the time domain (real). Currently supported values are 0 and 1.
`FACE`	Face (or edge in two dimensions) identification number whose type and connectivity are to be specified (integer). In practice, this identification number is ignored by AERO-S.
`FACE_TYPE`
1	2-node line segment. To be used with two-dimensional linear elements.
2	3-node line segment. To be used with two-dimensional quadratic elements.
3	3-node triangular face. To be used with three-dimensional linear tetrahedral element.
4	4-node quad face. To be used with three-dimensional linear hexahedral element.
6	6-node triangular face. To be used with three-dimensional quadratic tetrahedral element.
10	$\text{[math]}$ -node arbitrarily higher-order quad face where $\text{[math]}$ is the number of nodes on an edge of this face. To be used with element type 95.
11	arbitrarily higher-order triangular face.
12	arbitrarily higher-order line segment.
13	edge of a full isoparametric triangular element where the nodes are numbered linearly along it.
14	$\text{[math]}$ -node arbitrarily higher-order (spectral) quad face where $\text{[math]}$ is the number of nodes on an edge of this face. To be used with spectral element type 105.
`CONNECTIVITY_NODES`	These should be listed in a stacked fashion on a single line, and numbered clockwise (when looking from infinity in three dimensions).

4 ACOUSTIC TIME-DOMAIN DIRICHLET BOUNDARY CONDITIONS *S*

The ATDDIR command statement is used to specify nodal Dirichlet boundary conditions for a time-domain acoustic scattering problem. The input format is given below.

`NODE#`	Node number where the Dirichlet boundary condition is specified (integer).
`VALUE`	Value of the specified boundary condition (real).

5 ACOUSTIC TIME-DOMAIN DISTRIBUTED NEUMANN BOUNDARY CONDITION *S*

The ATDDNB command statement is used to specify the surface of a scatterer on which a distributed Neumann boundary condition of the form

\text{[math]}

is applied in a time-domain acoustic computation, and the value of the constant c.

`CONSTANT`	Value of the constant `c` (real).
`FACE`	Face (or edge in two dimensions) identification number whose type and connectivity are to be specified (integer). In practice, this identification number is ignored by AERO-S.
`FACE_TYPE`
1	2-node line segment. To be used with two-dimensional linear elements.
2	3-node line segment. To be used with two-dimensional quadratic elements.
3	3-node triangular face. To be used with three-dimensional linear tetrahedral element.
4	4-node quad face. To be used with three-dimensional linear hexahedral element.
6	6-node triangular face. To be used with three-dimensional quadratic tetrahedral element.
10	$\text{[math]}$ -node arbitrarily higher-order quad face where $\text{[math]}$ is the number of nodes on an edge of this face. To be used with element type 95.^M
11	arbitrarily higher-order triangular face.
12	arbitrarily higher-order line segment.
13	edge of a full isoparametric triangular element where the nodes are numbered linearly along it.
14	$\text{[math]}$ -node arbitrarily higher-order (spectral) quad face where $\text{[math]}$ is the number of nodes on an edge of this face. To be used with spectral element type 105.
`CONNECTIVITY_NODES`	These should be listed in a stacked fashion on a single line, and numbered clockwise (when looking from infinity in three dimensions).

6 ACOUSTIC TIME-DOMAIN NEUMANN BOUNDARY CONDITIONS *S*

The ATDNEU command statement is used to specify the nodal Neumann boundary conditions for a time-domain acoustic scattering problem. The input format is given below.

`NODE#`	Node number where the Neumann boundary condition is specified (integer).
`VALUE`	Value of the specified boundary condition (real).

7 ACOUSTIC TIME-DOMAIN ROBIN DISTRIBUTED BOUNDARY CONDITION *S*

The ATDROB command statement can be used to specify the surface of a scatterer on which a distributed Robin boundary condition of the form

\text{[math]}

is applied in a time-domain acoustic computation, and the three constants

\text{[math]}

\text{[math]}

, and

\text{[math]}

$\text{[math]}$	Non-zero constant premultiplying the normal derivative of the Robin boundary condition (real).
$\text{[math]}$	Constant premultiplying the unknown of the Robin boundary condition (float).
$\text{[math]}$	Constant right hand-side of the Robin boundary condition (float).
`FACE`	Face (or edge in two dimensions) identification number whose type and connectivity are to be specified (integer). In practice, this identification number is ignored by AERO-S.
`FACE_TYPE`
1	2-node line segment. To be used with two-dimensional linear elements.
2	3-node line segment. To be used with two-dimensional quadratic elements.
3	3-node triangular face. To be used with three-dimensional linear tetrahedral element.
4	4-node quad face. To be used with three-dimensional linear hexahedral element.
6	6-node triangular face. To be used with three-dimensional quadratic tetrahedral element.
10	$\text{[math]}$ -node arbitrarily higher-order quad face where $\text{[math]}$ is the number of nodes on an edge of this face. To be used with element type 95.^M
11	arbitrarily higher-order triangular face.
12	arbitrarily higher-order line segment.
13	edge of a full isoparametric triangular element where the nodes are numbered linearly along it.
14	$\text{[math]}$ -node arbitrarily higher-order (spectral) quad face where $\text{[math]}$ is the number of nodes on an edge of this face. To be used with spectral element type 105.
`CONNECTIVITY_NODES`	These should be listed in a stacked fashion on a single line, and numbered clockwise (when looking from infinity in three dimensions).

8 ACTUATORS *S*

The ACTUATORS command is used to prescribe at specified nodes and local degrees of freedom a time-variant source term (for example, a force field for a structural model) using a user-defined subroutine, and request the solution state at that node (for example, the displacement, velocity, and acceleration fields for a structural model). In this case, the user has to write his/her own algorithm for specifying the prescribed source term within a subroutine named "control.C". The SENSORS command must be used to pass to "control.C" the solution state at the nodes of interest (see SENSORS). The user should grab the special makefile for this command which is located within the AERO-S.d/Control.d directory, and use the LOAD command to activate this command.

For structural models, all prescribed forces and moments are interpreted by default as being of the axial type — that is, as being defined in the fixed nodal degree of freedom reference frames (see NODES and NFRAMES). However, if a node has rotational degrees of freedom, the user can specify that the forces and/or moments prescribed at this node are of the follower type — that is, they act in a direction that remains constant in the local frame attached to the node where they are applied. This local frame coincides with the nodal degree of freedom reference frame (see NODES and NFRAMES) in the undeformed configuration. In the deformed configuration, the orientation of this local frame is defined by the rotation of the node to which it is attached. In other words, the specified nodal force or moment "follows" in this case the rotation of the node to which it is applied.

`NODE#`	Node number where an actuating force/moment is specified (integer).
`DOF#`	Degree of freedom local number where an actuating force/moment is specified (integer).
`TYPE`	For structural models, all specified nodal source terms are by default of the axial type. However, if this parameter is set to `FOLLOWER` and the node `NODE#` has rotational degrees of freedom, the source term specified at this node and degree of freedom `DOF#` is considered to be of the follower type (characters).

9 AEROELASTICITY

Command Statement: AERO

The AERO command statement can be used to perform any of the following instructions:

- Choose a staggered time-integration algorithm (ALGORITHM subcommand) and, if needed, a displacement predictor (ALGORITHM subcommand) defined by two coefficients

\text{[math]}

and

\text{[math]}

and the formula

when the structural time-integrator is explicit, to perform a static or dynamic aeroelastic simulation.

Here,

\text{[math]}

(

\text{[math]}

) is the predicted displacement field at time-step

\text{[math]}

(

\text{[math]}

) and

\text{[math]}

is the structural time-step size (or simply, time-step) resulting from some settings of the DYNAMICS command. It is relevant however only for dynamic simulations.

Before setting the values of

\text{[math]}

and

\text{[math]}

that complete the definition of the displacement predictor and choosing the force corrector, the user should note that:

ALGORITHM $\text{[math]}$ $\text{[math]}$
SUBCYCLING n_subcycles
PRESSURE
MATCHER pathandfilename
EMBEDDED embeddedsurfaceid

`ALGORITHM`
`PP` [ALE]	This “Ping-Pong” algorithm sends the initial displacement of the structure, specified under either the IDISP6 command or the IDISPLACEMENTS (possibly equipped with the sub-command `MODAL`), to the fluid code which receives it and deforms the CFD mesh accordingly (characters). For this purpose, the `DYNAMICS` command must also be present in the AERO-S input file. After the send occurs, the structure code exits gracefully, the fluid code computes the fluid mesh deformation associated with the specified structural displacement and outputs (if requested) the corresponding position and/or displacement of the fluid mesh (characters).
`MPP`	This “Multi-Ping-Pong” algorithm sends several initial displacements of the structure at a time — for example, modal displacements — to the fluid code, which uses them to compute compatible fluid mesh deformations. The READMODE command must be used to input the initial displacements of interest — for example, a set of eigenmodes. If the second format of that command is used to specify the Reduced-Order Basis (ROB) to be used to generate the initial displacements, the coefficient $\text{[math]}$ of this command must be used to identify that ROB (see the field `rob_idi` in READMODE). If a coefficient $\text{[math]}$ is specified after `MPP`, the initial displacements are amplified by $\text{[math]}$ before they are sent to the fluid code. However, the fluid code scales back by $\text{[math]}$ the corresponding fluid mesh displacements it computes before saving them in an output file, in order to preserve the effect of the mass normalization of the modal structural displacements. The deformed fluid mesh configurations can then be used to generate sources of excitations for the construction of fluid POD bases and ROMs, or for linearized (perturbation) flow simulations whose initial conditions involve a (modal) position or velocity of the fluid surface mesh. As for the “Ping-Pong” case, the `DYNAMICS` command must also be present in the AERO-S input file, AERO-S exits gracefully after the send occurs, the fluid code computes the fluid mesh deformation associated with the specified structural displacements and outputs (if requested) the corresponding positions and/or displacements of the fluid mesh. In addition, for each inputted deformed fluid mesh position, the fluid code outputs an identification tag — for example, the frequency of the corresponding input structural mode in the case of modal displacements (characters).
`A0`	This is the basic sequential staggered solution algorithm (characters). When fluid subcycling is effected, the same algorithm has been referred to in the AIAA Paper 96-1388 by Farhat and co-workers as the `A1` algorithm (characters). It should not be used without a displacement predictor as it would reduce the overall order of time-accuracy compared to that intrinsic to the structural time-integrator. For the same reason, it is also not recommended — and as a matter of fact not available — when the structural time-integrator is explicit.
`A4`	This is the basic staggered solution algorithm with fluid-structure inter-parallelism (characters). It has been referred to as `A2` in the AIAA Paper 96-1388 by Farhat and co-workers. When this algorithm is specified, AERO-F sends to AERO-S $\text{[math]}$ or $\text{[math]}$ rather than the corresponding pressure fields at $\text{[math]}$ . Currently, this algorithm is not available when an explicit structural time-integrator is chosen.
`A5`	This staggered solution algorithm also features inter-parallelism but offers a better accuracy than `A4` when both methods are used without a displacement predictor (characters). Currently, this algorithm is not available when an explicit structural time-integrator is chosen.
`A6`	This staggered solution algorithm has superior stability and accuracy properties. It is recommended when the fluid is time-advanced by an implicit time-integrator. It has been referred to in most papers by Farhat and co-workers as the ISS (Improved Serial Staggered algorithm) method (characters). It delivers good accuracy without any displacement predictor. However, it is provably second-order time-accurate when equipped with the the displacement predictor defined by $\text{[math]}$ and $\text{[math]}$ , the midpoint implementation of the Newmark time-integrator with $\text{[math]}$ and $\text{[math]}$ (see DYNAMICS), and a second-order time-integrator for the discrete fluid problem. Also, this partitioned solution procedure prefers a non time-averaged pressure field. Most importantly, it was designed to be used exclusively with the `NONCOLLOCATED` scheme of aerodynamic force evaluation (see below) (characters). Currently, it does not support an explicit structural time-integrator.
`B0`	This one-way coupled steady-state aeroelastic algorithm sends the initial displacement of the structure (if any) to the flow solver. After receiving it and updating its mesh, AERO-F performs any requested flow simulation and sends to AERO-S upon completion the flow-induced load. Then, AERO-S receives this load, performs a static analysis if requested, and finally outputs any requested data (such as the computed flow-induced load, and/or resulting displacement, stress, and strain fields).
`C0`	This staggered solution algorithm is designed for the case where the structural subsystem is time-integrated by the explicit central difference method (see DYNAMICS), and the fluid subsystem is time-integrated by either an explicit or an implicit scheme. As shown in C. Farhat, A. Rallu, K. Wang and T. Belytschko, “Robust and Provably Second-Order Explicit-Explicit and Implicit-Explicit Staggered Time-Integrators for Highly Nonlinear Fluid-Structure Interaction Problems,” International Journal for Numerical Methods in Engineering, (2010), it is genuinely second-order time-accurate when equipped with the second-order displacement predictor obtained by setting $\text{[math]}$ and $\text{[math]}$ (see below), and a second (or higher)-order accurate explicit or implicit ALE fluid time-integrator. Currently, this algorithm supports only explicit structural time-integrators, and is the only algorithm which supports element deletion in fluid-structure simulations.
$\text{[math]}$	When used with the `MPP` command, this coefficient can be specified to amplify the initial displacements to be sent to the fluid code (however, as noted above, the fluid mesh displacements computed by the fluid code are scaled back by $\text{[math]}$ before they are saved in an output file). In this case, the default value is 1. Otherwise, this coefficient is part of the construction of a predictor for the position of the structure. For $\text{[math]}$ (and $\text{[math]}$ ), no prediction is effected. Setting $\text{[math]}$ (and $\text{[math]}$ ) generates a first-order prediction, and setting $\text{[math]}$ (and $\text{[math]}$ generates a second-order prediction. The optimal values of $\text{[math]}$ and $\text{[math]}$ depend on the specifics of the fluid and structure field time-integrators (see the aforementioned paper on interface energy conservation by Piperno and Farhat) (real). In this case, the default value is 0.5 for algorithm `C0`, and 0 for all other algorithms.
$\text{[math]}$	When used with the `MPP` command, this coefficient is interepreted as an integer that identifies among the reduced-order bases read using the READMODE command (see there the field `rob_idi`) that to be used with the algorithm `MPP` (integer). Otherwise, this coefficient is interpreted as a real coefficient that is part of the construction of a predictor for the position of the structure (real) and therefore should be used only as such (see above). In this case, its default value is $\text{[math]}$ for algorithm `C0`, and 0 for all other algorithms.
`SUBCYCLING` `n_subcycles`	This pair of sub-command keyword (characters) and corresponding numerical value (integer) specifies the structural subcycling factor, which defines the coupling fluid-structure time-step size (or simply, time-step) $\text{[math]}$ – that is, the time-interval during which structural and fluid computations are performed without any coupling, or equivalently, the time-interval between two couplings of the fluid and structural sub-systems – as follows $\text{[math]}$ where $\text{[math]}$ is the structural time-step resulting from some settings of the DYNAMICS command. Hence, `n_subcycles` can also be described as the number of time-steps that the structural analyzer performs per coupling fluid-structure time-step. The default value is 1.
`PRESSURE`	This option, which can take either value `COLLOCATED` or `NONCOLLOCAED`, specifies how to compute the corrected pressure field. It is relevant only when `ALGORITHM` is set to `A0`, `A4`, `A5`, or `A6`.
`COLLOCATED`	In this case, $\text{[math]}$ is set to the received pressure field $\text{[math]}$ (or $\text{[math]}$ ), then converted to $\text{[math]}$ before the aerodynamic forces are constructed and fed into the structural equations of dynamic equilibrium (see the introduction to this command). Therefore, this option covers the cases $\text{[math]}$ and $\text{[math]}$ , which explains the origin of the word “collocated” (characters).
`NONCOLLOCATED`	In this case, which is also the default value of `PRESSURE`, the pressure field $\text{[math]}$ is set to $\text{[math]}$ (or $\text{[math]}$ ), then converted to $\text{[math]}$ (here, $\text{[math]}$ is the $\text{[math]}$ parameter of the Generalized $\text{[math]}$ method). This specific choice for $\text{[math]}$ is consistent with the quadrature rule of the Generalized $\text{[math]}$ method for evaluating the work done by an external force in the time-interval $\text{[math]}$ . In other words, the pressure forces fed into the structural equations of equilibrium are based on $\text{[math]}$ . For $\text{[math]}$ , $\text{[math]}$ , which explains the origin of the word “non collocated” (characters).
`MATCHER`
`pathandfilename`	Name (including path, if needed) of the structural matcher file (characters). This file should be specified because the fluid-structure computation is to be performed without element deletion, using either the ALE or EBM framework. In the first case, the structural mesh should be matched with the fluid mesh. In the second case, it should be matched with the embedded discrete surface and this surface should be inputted to AERO-F.
`EMBEDDED` [EMB]
`embeddedsurfaceid`	Integer identification number of a surface defined in SURFACETOPO using 3-noded triangles, 4-noded quadrilaterals, or a combination of such elements (integer). This parameter should be specified when the discrete surface to be embedded in the fluid mesh for the purpose of a fluid-structure computation (with or without element deletion) is identical to the wet surface of the finite element structural model and defined using the same nodes of this model. In this case, it is not necessary to specify above a structure matcher file.

10 AEROHEAT

The AEROH command statement is used to indicate that AERO-S is to interact with AERO-F to perform an aerothermal (thermostructure-thermofluid) coupled simulation, to select a staggered time-integration algorithm (ALGORITHM subcommand), and specify the

\text{[math]}

and

\text{[math]}

parameters of the following prediction of the temperature of the structure at time-step

\text{[math]}

(ALGORITHM subcommand)

`ALGORITHM`
`A0`	This is the basic sequential aerothermal partitioned solution algorithm. It is similar to the `A0` algorithm of the `AERO` command.
$\text{[math]}$	For $\text{[math]}$ (and $\text{[math]}$ ), no prediction is effected. Setting $\text{[math]}$ (and $\text{[math]}$ ) generates a first-order prediction,and setting $\text{[math]}$ (and $\text{[math]}$ generates a second-order prediction. However, the optimal values of $\text{[math]}$ and $\text{[math]}$ depend on the specifics of the fluid and structure field time-integrators (see S. Piperno and C. Farhat, “Partitioned Procedures for the Transient Solution of Coupled Aeroelastic Problems - Part II: Energy Transfer Analysis and Three-Dimensional Applications,” Computer Methods in Applied Mechanics and Engineering, Vol. 190, pp. 3147-3170 (2001)) (real).
$\text{[math]}$	See above (real).

11 ATTRIBUTES *S*

The ATTRIBUTES command statement is used to label an element with an attribute identification number for linear elastic material and/or geometric properties, a composite or orthotropic shell, or anisotropic solid element attribute identification number, a frame or fiber-angle attribute identification number if this element has been defined as a composite or orthotropic shell or anisotropic solid element, and a hyper reduction coefficient when the mesh containing this element is sampled for the purpose of hyper reduction.

The attribute identification number for linear elastic material properties and/or geometric properties is required for all elements of the computational model. It is used in the MATERIAL command when specifying the linear elastic material properties and/or geometric properties of a group of elements (see MATERIAL).

An “empty” (or “phantom”) element — that is, an element with zero generalized stiffness and mass matrices — can be useful in aeroelastic and aerothermal computations to facilitate the exchange of elastodynamic, thermal, and aerodynamic data between the fluid, thermal, and structural analyzers. Such an element can be specified by assigning it a negative attribute number. In this case, it is not necessary to specify a material for such an element as its properties will be ignored.

It is also not necessary to assign an attribute number to a massless rigid element or simple joint element (types 118–125 and 127) for which the default constraint method (see CONSTRAINTS) is to be used for enforcing the associated constraints. On the other hand, an attribute number should always be assigned to a rigid element which has a mass (see MATERIAL), and a revolute-joint-with-joint-driver element (type 126) or a joint spring combination element (types 220–227), regardless of whether the default constraint method is to be used or not for this element.

The hyper reduction coefficients are computed by the RMSHC command and outputted in the result file SAMPLMSH (see OUTPUT) which includes the header ATTRIBUTES. Hence, this file can be simply included in the AERO-S input file using the INCLUDE command (see INTRODUCTION) for the purpose of hyper reduction. An alternative approach for this purpose that leads to faster CPU performance is to use the reduced mesh generated by the command RMSHC and outputted in the file SAMPLMSH.elementmesh.inc (see OUTPUT).

AERO-S supports three input formats for this command that are described below. In the case of the first format, there should be as many lines as the number of finite elements. All formats can be mixed.

ELEMENT# MAT_ATT# CMP_ATT# THETA

\text{[math]}

HRC HRCOEFF [EXTFOL]

STARTING_ELEMENT# ENDING_ELEMENT# MAT_ATT# CMP_ATT# THETA

\text{[math]}

`ELEMENT#`	Element number whose attribute numbers are to be specified (integer).
`MAT_ATT#`	Group identification number (integer); AERO-S supports gaps in numbering. Identifies material properties.
`CMP_ATT#`	Composite (orthotropic or anisotropic) identification number (integer); AERO-S supports gaps in numbering. Identifies composite (orthotropic or anisotropic) properties. May be left blank if element is not a composite (orthotropic or anisotropic) element and must be set to -1 if the orthotropic and/or anisotropic material properties of element are specified using the command MATLAW instead of the command COMPOSITE.
`CMP_FRM#`	Composite frame identification number (integer); AERO-S supports gaps in numbering. May be left blank if element is not a composite (orthotropic or anisotropic) element.
`THETA`	Keyword that must be spelled as `THETA` (characters). This keyword announces that the next item on the same input line is the value $\text{[math]}$ of `THETA`. This unusual AERO-S input is necessary to avoid parsing conflicts.
$\text{[math]}$	Reference angle in degrees between the axis defined by local nodes 1 and 2 of the element, and the material local x-axis defining the direction of the $\text{[math]}$ and $\text{[math]}$ of the constitutive law (real). When also using the `LAYN` and `LAYC` commands, the material x-axis corresponds to the direction of $\text{[math]}$ when $\text{[math]}$ is zero. If this angle rather than `CMP_FRM#` is specified, the composite frame is internally generated by AERO-S.
`STARTING_ELEMENT#`	First element of a sequence of elements that have the same MAT_ATT#, CMP_ATT#, and CMP_FRM# (integer).
`ENDING_ELEMENT#`	Last element of a sequence of elements that have the same MAT_ATT#, CMP_ATT#, and CMP_FRM# (integer).
`MAT_ATT#`	Group identification number. Identifies material properties (integer).
`CMP_ATT#`	Composite identification number (integer). Identifies composite (orthotropic or anisotropic) properties. May be left blank if element is not a composite (orthotropic or anisotropic) element.
`CMP_FRM#`	Composite frame identification number (integer). May be left blank if element is not a composite (orthotropic or anisotropic) element.
`IDENTITY`	This keyword signals to the AERO-S code that each element in the range delimited by `STARTING_ELEMENT#` and `ENDING_ELEMENT#` has a material attribute identification number equal to its element identification number. For example, the sequence 1 3 IDENTITY means that element#1 has the material attribute identification 1, element#2 has the material attribute identification 2, and element#3 has the material attribute identification 3.
`HRC`	Sub-command keyword to request the application of a specified hyper reduction coefficient to the element-level reduced internal forces and moments and acquiring this coefficient (characters).
`HRCOEFF`	Hyper reduction coefficient computed by the RMSHC command and stored in the result file `SAMPLMSH` under OUTPUT (float).
[`EXTFOL`]	Optional sub-command keyword to request the application of the specified hyper reduction coefficient to all of the element-level reduced internal forces and moments and the element-level reduced follower external forces and moments (see FORCES) (characters).

12 BEAM OFFSET

The BOFFSET command statement is used to specify a beam's neutral axis offset from the line passing through its two end nodes. This command may be used for both Euler-Bernoulli and Timoshenko beam elements. For beam elements not listed under BOFFSET, a zero offset is used. If the BOFFSET command is absent altogether, then an offset of zero is used for all beam elements. If a listed element is neither an Euler-Bernoulli nor a Timoshenko beam element, then the offset is ignored for that element. The input format is as follows.

`STARTING_ELEMENT#`	First element of a sequence of elements that have the same offset specified by {`x`, `y`, `z`} (integer).
`ENDING_ELEMENT#`	Last element of a sequence of elements that have the same offset specified by {`x`, `y`, `z`} (integer). If `ENDING_ELEMENT#` is the same as `STARTING_ELEMENT#`, then the specified offset is applied to that element only (integer).
`x`	x component of the offset vector expressed in the global frame (float).
`y`	y component of the offset vector expressed in the global frame (float).
`z`	z component of the offset vector expressed in the global frame (float).

13 BEAM REFERENCE FRAMES

The EFRAMES command statement is used to specify a beam's orientation which defines the position of the beam with respect to the global frame. The requirements for each beam frame are that one of the axis, the local x-axis, concurs with the longitudinal axis of the beam, and the remaining two axes complete an orthogonal triad. If this requirement is violated, AERO-S regenerates the local x-axis as well as the local z-axis.

For flexible beams, AERO-S also supports a run-time generation of frames that is activated either when the target flexible beam element is identified under this command and a third node is specified to generate the frame, or when a third node is found in the definition of a flexible beam element within the TOPOLOGY command. The only requirement for the third node is that it does not be colinear with the other two beam nodes that define the local x-axis (X). Under this command, the third node defines the X,Y plane. Under the TOPOLOGY command, it defines the X,Z plane. Using the third node option under the TOPOLOGY command also relieves the user from specifying the EFRAMES command. An example illustrating the third node option in the TOPOLOGY command can be found in FEM.d/fem_examples/Third_Node.d

Otherwise, the input format for this command is given below with the number of lines equal to the number of beams in the problem.

`ELEMENT#`	Element number where the beam frame is specified (integer).
$\text{[math]}$	The first axis, the local x-axis, of the beam frame expressed in the global frame. This axis must concur with the longitudinal axis of the beam (floats).
$\text{[math]}$	The second axis of the beam frame expressed in the global frame (floats).
$\text{[math]}$	The third axis of the beam frame expressed in the global frame (floats).
`THIRDNODE`	Keyword that must be spelled as `THIRDNODE`. This keyword announces that the next item on the same input line is the value `third_node#` of `THIRDNODE`. This unusual AERO-S input is necessary to avoid parsing conflicts (characters).
`THIRD_NODE#`	Id number of an existing node to be considered as a third node of the flexible beam element identified by `ELEMENT#`, and which must be in the local x-y plane of the beam. The only requirement for the third node is that it does not be colinear with the other two beam nodes. The normalized vector node1 to node2 defines the local x axis. The normalized vector node1 to node3 defines the local y-axis. The local z-axis is automatically generated as cross product of the other two normalized axes.

Note 1: The above axes have to be normalized. By default, the beam frames concur with the global frame.

14 BINARY INPUT / OUTPUT

When the finite element model of interest is very large, it may become necessary (for example, because of memory limitations), to organize the input data of an AERO-S computation in a set of binary distributed files, and more efficient to output its results in another set of binary distributed files. This requires:

To decompose the input data contained in an initial instance of the ASCII Input Command Data file according to a generated mesh partition and reorganize it in a set of binary distributed input files, the user should use the specialized version of the software SOWER that is embedded in AERO-S. The generated binary distributed input files can then be inputted via this command in the final instance of the ASCII Input Command Data file. This command can also be used to request outputting the results marked for output in OUTPUT and/or OUTPUT6 in the binary distributed format compatible with the generated mesh partition. In that case, the original SOWER (see SOWER's User's Reference Manual) should be used to convert these output files into the ASCII format suitable for postprocessing by XPost.

If memory is not an issue, AERO-S can also operate directly on the global set of input data — that is, on the standard content of the ASCII Input Command Data file.

Note 2: Any command present in the initial instance of the ASCII Input Command Data file and whose description in this User's Reference Manual is marked by "*S*" can be assumed to be contained in one of the aforementioned binary distributed input files. However, if that command contains both an algorithmic parameter as well as data, only the data will be contained in the appropriate distributed binary input file. Therefore, the command itself should be kept in the updated ASCII Input Command Data file together with the algorithmic parameter, but without the data. For example, the command IDISPLACEMENTS specifies both an amplification factor and an initial displacement data. The initial displacement data will be included in the aforementioned binary distributed input file, but the amplification factor will not. This is to allow the user to change simple things such as this amplification factor without having to regenerate the binary distribtued input files.

Note 3: This data organization option does not support the sparse direct solver MUMPS (see STATICS).

BINARYINPUT flagBIN [<pathandfileprefix>]
BINARYOUTPUT flagBOUT
CPUMAP <pathandfilename>

`BINARYINPUT` `flagBIN`	This pair of sub-command keyword (characters) and corresponding value (characters) can be used to choose between reading the binary distributed input files designated by `<pathandfileprefix>`, or the standard ASCII global input data contained in the initial instance of the ASCII Input Command Data file. `flagBIN` should be inputted on the same line as `BINARYINPUT`; it can take one of the following values:
`On`	This setting chooses the specified binary distributed input files as input. In this case, the user should check first that all binary distributed input files have been generated and that the associated filenames and path are those referred to in `<pathandfileprefix>`.
`Off`	This setting, which is also the default setting, chooses the standard ASCII global data. In this case, the user should check first that all needed input data is included in the ASCII Input Command Data file.
`<pathandfileprefix>`	This entry is relevant only when `flagBIN` is set to `On`. By default, AERO-S expects the binary input data command to be contained in four binary distributed files named `INPUT.dec`, `INPUT.con`, `INPUT.sub`, and `INPUT.msh`. Alternatively, this data can be contained in four equivalent files that are named differently, as long as they share the same path and filename prefix — that is, these four binary distributed files must have the same path and can be named `fileprefix.dec` (substitute for `INPUT.dec`), `fileprefix.con` (substitute for `INPUT.con`), `fileprefix.sub` (substitute for `INPUT.sub`), and `prefixfile.msh` (substitute for `INPUT.msh`). In the latter case, `<pathandfileprefix>` specifies the common filename prefix (and file path if needed) (characters).
`BINARYOUTPUT` `flagBOUT`	This pair of sub-command keyword (characters) and corresponding value (characters) can be used to choose between outputting the results specified in OUTPUT and/or OUTPUT6 in the binary distributed format, or the standard ASCII global format. `flagBOUT` should be inputted on the same line as `BINARYOUTPUT`; it can take one of the following values:
`On`	This setting chooses the binary distributed format for all output files that support it.
`Off`	This setting, which is also the default setting, chooses the standard ASCII global format for all output files.
`CPUMAP` `<pathandfilename>`	This pair of sub-command keyword (characters) and corresponding value (characters) can be used to input a CPU map file – that is, a file that specifies to which CPU each subdomain is to be assigned. The format of this file is the same as that of the decomposition file, with the number of subdomains replaced by the number of CPUs, the number of elements in a given subdomain replaced by the number of subdomains in a given CPU, and the element ID number in each subdomain replaced by the subdomain ID number in each CPU. The default for `<pathandfilename>` is CPUMAP, in which case this file must be located in the directory where the simulation is launched. If `<pathandfilename>` is not specified and a file named CPUMAP is not found in the aforementioned directory, a default subdomain-to-CPU map is internally generated by AERO-S.

15 BOUNDARY CONVECTION *S*

The CONVECTION command statement is used to specify nodal convection type boundary conditions. Each node can have only one degree of freedom. This command statement can be used to solve a prescribed boundary convection problem for both statics and dynamics. The input format is given below.

`LOADSET_ID`	Optional non-negative integer which identifies explicitly the "load" set to which the source term generated by this command belongs to (integer). The default value is 0. Hence, the `CONVECTION` command can be repeated as many times as desired within the same input file using each time a different value for `LOADSET_ID` and different data. The LOADCASE command can refer to `LOADSET_ID` to define one or multiple "load" cases for static analysis (see the STATICS command and the explanation of its sub-command keyword `CASES`), and/or the "load" case for dynamic analysis.
`NODE#`	Node number where the convection is specified (integer).
`H_COEFF`	Convection coefficient at the prescribed node (float).
`AREA`	Value of the node cross-sectional area (float).
`TA`	Ambient temperature around the node (float).

16 BOUNDARY DISPLACEMENTS *S*

The DISPLACEMENTS command is used to prescribe nodal displacements and/or rotations, either directly, or via the definition of a surface using the command SURFACETOPO. In the latter case, the specified displacement or rotation is applied to each specified local degree of freedom of each node of that surface. The user can specify up to three displacements per node if a node can have up to three degrees of freedom, and up to three displacements and three rotations if it can have up to six degrees of freedom.

`NODE#`	Node number where the displacement or rotation is specified (integer).
`DOF#`	Degree of freedom local number where the displacement or rotation is specified (integer).
`VALUE`	Value of the specified displacement or rotation (real).
`SURFACE`	Keyword indicating that a surface defined in SURFACETOPO is to be identified next by its integer identification number (characters).
`SURFACE#`	Integer identification of the surface defined in SURFACETOPO where the force `VALUE` is specified (integer).

17 BOUNDARY FLUXES

The FLUX command statement is used to specify nodal heat sources (for example, products of nodal areas and nodal values of finite element fluxes) either directly, or via the definition of a surface using the command SURFACETOPO. In the latter case, a specified heat source is applied to each node of the identified surface. This command statement can be used to define both statics and dynamics heat problems with prescribed temperature flux boundary conditions. Its input format is given below.

`LOADSET_ID`	Optional non-negative integer which identifies explicitly the "load" set to which the source term generated by this command belongs to (integer). The default value is 0. Hence, the `FLUXES` command can be repeated as many times as desired within the same input file using each time a different value for `LOADSET_ID` and different data. The LOADCASE command can refer to `LOADSET_ID` to define one or multiple "load" cases for static analysis (see the STATICS command and the explanation of its sub-command keyword `CASES`), and/or the "load" case for dynamic analysis.
`NODE#`	Node number where the flux is specified (integer).
`VALUE`	Value of the prescribed boundary flux (float).
`SURFACE`	Keyword indicating that a surface defined in SURFACETOPO is to be identified next by its integer identification number (characters).
`SURFACE#`	Integer identification of the surface defined in SURFACETOPO where the nodal heat source `VALUE` is specified (integer).

18 BOUNDARY FORCES *S*

The FORCES command is used to prescribe external nodal forces and/or moments, either directly, or via the definition of a surface using the SURFACETOPO command. In the latter case, the specified force or moment is applied to each specified local degree of freedom of each node of that surface. The user can specify up to three forces per node if a node has three degrees of freedom attached to it, and up to three forces and three moments if it has six degrees of freedom attached to it.

By default, all prescribed forces and moments are interpreted as being of the axial type — that is, as being defined in the fixed nodal degree of freedom reference frames (see NODES and NFRAMES).

However, if a node has rotational degrees of freedom, the user can specify that the forces and/or moments prescribed at this node are of the follower type — that is, they act in a direction that remains constant in the local frame attached to the node where they are applied. This local frame coincides with the nodal degree of freedom reference frame (see NODES and NFRAMES) in the undeformed configuration. In the deformed configuration, the orientation of this local frame is defined by the rotation of the node to which it is attached. In other words, the specified nodal force or moment "follows" in this case the rotation of the node to which it is applied.

Finally, the user can also time-vary the specified forces and moments using the MFTT command.

`LOADSET_ID`	Optional non-negative integer which identifies explicitly the "load" set to which the source term generated by this command belongs to (integer). The default value is 0. Hence, the `FORCES` command can be repeated as many times as desired within the same input file using each time a different value for `LOADSET_ID` and different data. The LOADCASE command can refer to `LOADSET_ID` to define one or multiple "load" cases for static analysis (see the STATICS command and the explanation of its sub-command keyword `CASES`), and/or the "load" case for dynamic analysis.
`NODE#`	Node number where the force or moment is specified (integer).
`DOF#`	Degree of freedom local number where the force or rotation is specified (integer).
`VALUE`	Value of the specified force or moment (real).
`TYPE`	By default, all specified nodal forces and moments are considered to be of the axial type. However, if this parameter is set to `FOLLOWER` and the node where a force or moment is specified has rotational degrees of freedom, this specified nodal force or moment is considered to be of the follower type (characters).
`SURFACE`	Keyword indicating that a surface defined in SURFACETOPO is to be identified next by its integer identification number (characters).
`SURFACE#`	Integer identification of the surface defined in SURFACETOPO where the force or moment `VALUE` is specified (integer).

19 BOUNDARY TEMPERATURES *S*

The TEMPERATURES command statement is used to specify prescribed nodal temperature type boundary conditions either directly, or via the definition of a surface using the command SURFACETOPO. In the latter case, a specified temperature is applied to each node of the identified surface. For structural analysis using AERO-S, this command statement causes AERO-S to construct a thermal load based on the prescribed nodal temperatures and the reference temperatures (see MATLAW, see TOPOLOGY, and use this load as usual in a structural analysis).

`NODE#`	Node number where the temperature is specified (integer).
`VALUE`	Value of the prescribed temperature (float).
`SURFACE`	Keyword indicating that a surface defined in SURFACETOPO is to be identified next by its integer identification number (characters).
`SURFACE#`	Integer identification of the surface defined in SURFACETOPO where the temperature `VALUE` is specified (integer).

20 BUCKLING

The BUCKLE command statement is to be used together with the GEPS, IDISP6 (with

\text{[math]}

), and EIGEN command statements to request the buckling analysis of a given structure.

When the EIGEN, GEPS, and IDISP6 (with

\text{[math]}

) command statements are specified in the input file, the BUCKLE command statement signals to FEM that the eigenvalue problem to be solved is

\text{[math]}

, where

\text{[math]}

is the geometric stiffness matrix associated with a displacement field specified under the IDISP6 command statement, and whose computation is triggered by the presence of the GEPS command statement in the input file. For each eigenvalue

\text{[math]}

, the corresponding buckling load is

\text{[math]}

where f is the load that created the displacement field specified under the IDISP6 command.

An example input file that illustrates a buckling analysis can be found in FEM.d/fem_examples/Buckle.d The syntax for invoking this option is given below.

21 CLUSTERING SNAPSHOTS OR CONSTRUCTING A REDUCED BASIS

Each computed cluster of displacement (and other associated quantities) is outputted by this same command as described in the explanation of the DO_CLUSTERING sub-command keyword. On the other hand, any computed ROB can be outputted using the result keyword ROBDATAF under OUTPUT.

SNAPFI <pathandfilenameS1> <pathandfilenameS2> ... ... <pathandfilenameSN>
VELSNAPFI <pathandfilenameV1> <pathandfilenameV2> ... ... <pathandfilenameVN>
ACCSNAPFI <pathandfilenameA1> <pathandfilenameA2> ... ... <pathandfilenameAN>
ROBFI <pathandfilenameR1> <pathandfilenameR2> ... ... <pathandfilenameRN>
SSCALI flagss flagrs
SNORMA flagsn flagrn
COMPRESS flagco
DIMENS dim
ROMENR $\text{[math]}$
MNORMA flagmn
SKIP freq [offset]
USE_NMF maxnoi cvtolr
USE_NMF numrob incsiz numini maxnoi cvtolr
USE_GREEDY
USE_PQN maxnoi cvtolr maxini stepln
NSUBS nblcks
DO_CLUSTERING nclusters

`SNAPFI`	Sub-command keyword for specifying one or multiple ASCII or binary files containing solution snapshots and associated weights (characters). These snapshots can be: Primal (displacement, velocity, and/or acceleartion) or dual (Lagrange multiplier) solution snapshots, if this command is used to construct a primal or dual, global or local ROB. Displacement solution snapshots, if this command is used for the purpose of clustering. If the solution snapshots were generated in the time domain, the weight of a solution snapshot is the square root of the average of the time-steps separating this snapshot from the previous and next ones, except for the first and last outputted solution snapshots which are computed as follows: the weight of the first solution snapshot is the square root of the time-step separating this snapshot and the next one, and that of the last solution snapshot is computed as the square root of the time-step separating this snapshot and the previous one.
`<pathandfilenameS>`	Path and name of each ASCII or binary file containing solution snapshots and associated weights (characters). If more than one file is specified, all files are read. The union of all inputted solution snapshot vectors (and consistent ROB vectors inputted after the `ROBFI` sub-command keyword) is either: Compressed to construct the desired ROB: in this case, all inputted solution snapshots can be scaled by their associated weights or normalized using the infinity norm before they are compressed using the SVD, if requested using `SSCALI` or `SNORMA`, respectively. Or clustered (see `DO_CLUSTERING`).
`VELSNAPFI`	Optional sub-command keyword for specifying one or multiple ASCII or binary files containing velocity solution snapshots (characters). It should be used only when this command is used for clustering solution snapshots. In this case, the velocity solution snapshots are regrouped in the same clusters as the associated displacement solution snapshots and saved in the binary files `<pathandfilenameV1>.cluster`j, where j is the cluster index.
`<pathandfilenameV>`	Path and name of each ASCII or binary file containing velocity solution snapshots (characters). If more than one file is specified, all files are read. The union of all inputted velocity s olution snapshots is clustered when the `DO_CLUSTERING` sub-command keyword is used (see below).
`ACCSNAPFI`	Optional sub-command keyword for specifying one or multiple ASCII or binary files containing acceleration solution snapshots (characters). It should be used only when this command is used for clustering solution snapshots. In this case, the acceleration solution snapshots are regrouped in the same clusters as the associated displacement solution snapshots and saved in the binary files `<pathandfilenameA1>.cluster`j, where j is the cluster index.
`<pathandfilenameA>`	Path and name of each ASCII or binary file containing acceleration solution snapshots (characters). If more than one file is specified, all files are read. The union of all inputted acceleration solution snapshots is clustered when the `DO_CLUSTERING` sub-command keyword is used (see below).
`ROBFI`	Sub-command keyword (characters) for specifying one or multiple ASCII or binary files containing: ROB vectors. Associated weights (singular values, if these vectors were generated using SVD.)
`ROBFI`	Sub-command keyword (characters) for specifying one or multiple ASCII or binary files containing: ROB vectors. Associated weights (singular values, if these vectors were generated using SVD).
`<pathandfilenameR>`	Path and name of each ASCII or binary file containing ROB vectors (and when applicable, associated weights) to be considered for constructing the desired ROB (characters). If more than one file is specified, all files are read. The union of these ROB vectors (and potentially solution snapshots inputted after the `SNAPFI`) sub-command keyword) is compressed by SVD or NMF, as specified, to construct the desired ROB. When requested using `SSCALI` or `SNORMA`, all inputted ROB vectors are scaled by their associated weights or normalized using the infinity norm, respectively, if SVD is chosen as the data compression algorithm.
`SSCALI`	Sub-command keyword for specifying whether to scale or not the snapshots inputted using `SNAPFI`, or the ROB vectors inputted using `ROBFI` by their associated weights, when this command is used for the purpose of constructing a desired ROB and SVD is chosen as the data compression algorithm (characters).
`flagss`	If this flag is set to `YES`, the snapshots inputted using `SNAPFI` are scaled by their associated weights before they are used to construct a ROB. If it is set to `NO`, which is the default setting, they are left as is.
`flagrs`	If this flag is set to `YES`, the ROB vectors inputted using `ROBFI` are scaled by their associated weights before they are used to construct a ROB. If it is set to `NO`, which is the default setting, they are left as is.
`SNORMA`	Sub-command keyword for specifying whether to normalize or not – using the infinity norm – the snapshots inputted via `SNAPFI`, or the ROB vectors inputted using `ROBFI`, when this command is used for the purpose of constructing a desired ROB and SVD is chosen as the data compression algorithm (characters).
`flagsn`	If this flag is set to `YES`, the snapshots inputted using `SNAPFI` are normalized using the infinity norm before they are used to construct a ROB. If it is set to `NO`, which is the default setting, they are left as is.
`flagrn`	If this flag is set to `YES`, the ROB vectors inputted using `ROBFI` are normalized using the infinity norm before they are used to construct a ROB. If it is set to `NO`, which is the default setting, they are left as is.
`COMPRESS`	Sub-command keyword relevant only when the `ROBC` command is used specifically for orthonormalizing a previously computed global or local primal ROB with respect to the mass matrix arising from the current ASCII Input Command Data file. Its purpose is to specify whether or not to compress the solution snapshots inputted under `SNAPFI` and/or `ROBFI` (characters).
`flagco`	This flag can have one of the following two settings: `NO`: In this case, the information inputted under `SNAPFI` or `ROBFI` should be the column vectors of a previously computed global or local primal ROB, and the objective of the `ROBC` command should be to orthonormalize this primal ROB with respect to the mass matrix arising from the current ASCII Input Command Data file. `YES`: This is the default setting. In this case, the information inputted under `SNAPFI` and/or `ROBFI` is compressed using SVD or NMF, as specified.
`DIMENS`	Sub-command keyword for specifying the desired dimension of the ROB to be constructed (characters). Note that if both `ROMENR` and this sub-command keyword are specified in the same ASCII Input Command Data file, this sub-command keyword takes priority. If none of them is specified and the ROB is constructed using SVD, the dimension of this ROB is set to the rank of the snapshot matrix.
`dim`	Dimension of the ROB to be constructed (integer). The default value is the minimum between the total number of degrees of freedom of the underlying finite element model, and the total number of vectors to be compressed.
`ROMENR`	Sub-command keyword that is relevant only when SVD is chosen as the data compression algorithm for constructing a global or local, primal or dual ROB. It requests using the criterion based on the relative energy of the solution snapshots captured by the first SVD vectors to truncate the SVD basis and therefore determine the appropriate dimension $\text{[math]}$ of the ROB to be constructed (characters). Specifically, $\text{[math]}$ is determined in this case so that the square of the relative error gives an indication of the magnitude of the "missing" information — that is $\text{[math]}$ where $\text{[math]}$ is the matrix of $\text{[math]}$ solution snapshots, $\text{[math]}$ is its rank, $\text{[math]}$ is the size of the high-dimensional model, $\text{[math]}$ is the $\text{[math]}$ -th singular value of $\text{[math]}$ , $\text{[math]}$ , and $\text{[math]}$ is the desired ratio of the energy of the solution snapshots captured by the constructed ROB and total energy of the computed solution snapshots and is specified below. Note that if both `DIMENS` and this sub-command keyword are specified in the same ASCII Input Command Data file, `DIMENS` takes priority. If none of them is specified and the ROB is constructed using SVD, the dimension of this ROB is set to the rank of the snapshot matrix.
$\text{[math]}$	Desired value of the ratio $\text{[math]}$ of the energy of the solution snapshots to be captured by the constructed ROB, and total energy of the computed solution snapshots (real).
`MNORMA`	Sub-command keyword for specifying the SVD-based computation of the desired global or local, primal ROB (characters).
`flagmn`	This flag can have one of the following three settings: `IM`: This is the defaut setting. In this case, two equivalent but different ROBs are computed as follows and in this order: First, one ROB that is orthonormalized with respect to the identity matrix. Second, a counterpart ROB whose columns span the same subspace, but which is orthonormalized with respect to the mass matrix. In this case, the construction of the second ROB does not incur the factorization of the high-dimensional mass matrix, but that of the reduced mass matrix. Note that if the high-dimensional mass matrix is singular, the reduced mass matrix may or may not be singular, depending on the content of the ROB. `MI`: In this case, two equivalent but different ROBs are computed as follows and in this order: First, one ROB that is orthonormalized with respect to the mass matrix and computed using an algorithm that factorizes this mass matrix. Hence, in this case, the user must ensure that the mass matrix of the finite element model is non singular. A counterpart ROB whose columns span the same subspace, but which is orthonormalized with respect to the identity matrix. `ID`: In this case, a single ROB that is orthonormalized with respect to the identity matrix is computed.
`SKIP`	Sub-command keyword for specifying whether or not to skip some of the solution snapshots inputted using the `SNAPFI` sub-command keyword for the purpose of their clustering or the construction of the desired ROB (characters).
`freq`	Frequency (every so many) at which to skip a solution snapshot in any specified solution snapshot file (integer). The default value is 1.
`offset`	Offset in terms of the solution snapshot number to apply before starting the skipping process (integer). The default value is 0.
`USE_NMF`	Sub-command keyword that is relevant only for the solution of the class of constrained problems identified above, using the methods and algorithms also identified above. It activates the computation of a dual ROB using the non-negative matrix factorization approach based on the alternating Non-Negative Least-Squares (NNLS) method (characters).
`maxnoi`	Maximum number of outer-iterations for the non-negative matrix factorization algorithm (integer).
`cvtolr`	Relative convergence tolerance of the Frobenius norm of the dual basis increment computed at each iteration of the non-negative matrix factorization method (real). This parameter is relevant only for the solution of the class of constrained problems identified above, using the methods and algorithms also identified above.
`numrob`	Number of ROBs to be computed (integer). The default value is 1.
`incsiz`	Size increment to apply when computing multiple ROBs (integer).
`numini`	Number of random initializations to perform when computing each ROB (integer). The default value is 1.
`USE_GREEDY`	Sub-command keyword for activating the computation of a dual ROB using a Greedy method (characters). This parameter is relevant only for the solution of the class of constrained problems identified above, using the methods and algorithms also identified above.
`USE_PQN`	Sub-command keyword for activating the computation of a dual ROB using the non-negative matrix factorization approach based on a projected quasi-Newton method (characters). It is relevant only for the solution of the class of constrained problems identified above, using the methods and algorithms also identified above.
`maxini`	Maximum number of inner-iterations that can be performed by the projected quasi-Newton method for computing the non-negative matrix factorization (integer).
`stepln`	Step length parameter for the projected quasi-Newton method for computing the non-negative matrix factorization (real).
`nblcks`	Number of column-wise blocks defining the parallelization strategy for the alternating NNLS method (integer). The default value is 1.
`DO_CLUSTERING`	Sub-command keyword for clustering a set of displacement solution snapshots using the k-means algorithm. In this case, the generated solution snapshot clusters and their centroids are saved in the binary files `<pathandfilenameS1>.cluster`j and `<pathandfilenameS1>.cluster`j`.centroid`, respectively, where j designates the $\text{[math]}$ -th cluster and `<pathandfilenameS1>` is the `<pathandfilenameS1>` specified after the `SNAPFI` sub-command keyword. If the optional `VELSNAPFI` sub-command keyword is also specified (see above), the inputted velocity solution snapshots are regrouped in the same clusters as the associated displacement solution snapshots and saved in the binary files `<pathandfilenameV1>.cluster`j, where j is the cluster index. Similarly, if the optional `ACCSNAPFI` sub-command keyword is also specified (see above), the inputted acceleration solution snapshots are regrouped in the same clusters as the associated displacement solution snapshots and saved in the binary files `<pathandfilenameA1>.cluster`j, where j is the cluster index.
`nclusters`	Desired number of clusters (integer).

22 COMMENTS

The '*' at the beginning of a line indicates that the subsequent input on the same line is a comment. For FEM, it can be placed anywhere.

23 COMPOSITE (OR ORTHOTROPIC SHELL OR ANISOTROPIC SOLID)

The COMPOSITE command is used to specify the properties of a composite, anisotropic, or orthotropic solid, shell, or membrane element made of a linear material. It currently supports only the solid elements type 17, 23, 24, 25, 72, 91 92, and 97, the (Kirchhoff) shell elements type 15, 1515, 20, and 2020, and the membrane elements type 128 and 129. All information concerning constitutive coefficients or the layering of a composite is inputted using this command.

For the above solid elements, the constitutive matrix, the coefficients of thermal expansion, and the hygroelastic coupling coefficients are inputted using the COEF sub-command. The constitutive matrix is defined in the local frame of the element specified in the CFRAMES command. Entries in the matrix that are not specified are determined from symmetry if appropriate, or are set to zero.

For the shell elements, the composite (anisotropic, or orthotropic) constitutive law can be prescribed either by entering the

\text{[math]}

coefficients of the 6 by 6 constitutive matrix, or by defining the material properties and geometrical characteristics for each layer of the composite. In the first case, the COEF sub-command should be used. In the second case, either of the LAYC and LAYN sub-commands can be used, depending on whether the coupling between bending and membrane effects is to be enforced or not, respectively. When many layers of the composite are made of the same anisotropic material, the LAYD and LAYMAT sub-commands can be used instead of the LAYC sub-command to simplify the data entry process. Likewise, in similar circumstances, the LAYO and LAYMAT sub-commands can be used instead of the LAYN sub-command.

Note 1: If a laminate layup is unsymmetric (with respect to the mid-plane), the plies must be numbered from the top side to the bottom side, with the top side defined by the direction of its element normals that must point from bottom to top.

Note 2: In a nonlinear analysis, the COEF sub-command can currently be used only to define an anisotropic hyperelastic or hyperviscoelastic material. Hence, it can be specified together with the following material laws: Linear, LinearPlaneStress, HyperElasticPlaneStress, HenckyElastic, StVenantKirchhoff, ViscoLinearElastic, ViscoStVenantKirchhoff, ViscoLinearPlaneStress, and ViscoHyperElasticPlaneStress (see MATLAW). In the case of StVenantKirchhoff and HyperElastic, the material laws relate the Green-Lagrange (engineering) strain and its conjugate stress, the second Piola-Kirchhoff stress. In the case of HenckyElastic, the material law relates the Lagrangian Hencky (engineering) strain and its conjugate stress, the rotated Kirchhoff stress.

Note 3: The case of a linear hyperelastic material includes the special case of a linear hygrothermoelastic material represented by the constitutive equation

where

\text{[math]}

and

\text{[math]}

denote the vectorized stress and strain tensors, respectively;

\text{[math]}

denotes the temperature field;

\text{[math]}

denotes the moisture concentration (mole number);

\text{[math]}

denotes the standard constitutive matrix for elasticity;

\text{[math]}

and

\text{[math]}

denote the vectorized tensors of thermal expansion and hygroelastic coupling coefficients, respectively; and

\text{[math]}

and

\text{[math]}

denote the temperature and moisture concentration of the reference (stress-free) state of the material, respectively. For example,

\text{[math]}

can be chosen to be the ambient temperature

\text{[math]}

specified in MATERIAL.

COEF attribute# $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
ROW# ( $\text{[math]}$ ) COLUMN# ( $\text{[math]}$ ) VALUE ( $\text{[math]}$ )
.
.
.
ROW# ( $\text{[math]}$ ) COLUMN# ( $\text{[math]}$ ) VALUE ( $\text{[math]}$ )

`COEF`	Sub-command keyword used to directly input the coefficients of the constitutive law. Since the 6 by 6 constitutive matrix is symmetric, up to 21 independent coefficients may follow.
`attribute#`	Integer value that corresponds to the composite (or orthotropic or anisotropic) attribute of the element.
$\text{[math]}$	Thermal expansion coefficient associated with the strain $\text{[math]}$ . It can be omitted, in which case its default value is 0.
$\text{[math]}$	Thermal expansion coefficient associated with the strain $\text{[math]}$ . It can be omitted, in which case its default value is 0.
$\text{[math]}$	Thermal expansion coefficient associated with the strain $\text{[math]}$ . It can be omitted, in which case its default value is 0.
$\text{[math]}$	Thermal expansion coefficient associated with the strain $\text{[math]}$ . It can be omitted, in which case its default value is 0.
$\text{[math]}$	Thermal expansion coefficient associated with the strain $\text{[math]}$ . It can be omitted, in which case its default value is 0.
$\text{[math]}$	Thermal expansion coefficient associated with the strain $\text{[math]}$ . It can be omitted, in which case its default value is 0.
`ROW#`	Integer value that corresponds to the row $\text{[math]}$ of the coefficient $\text{[math]}$ . A row can be skipped if all its entries are zero.
`COLUMN#`	Integer value that corresponds to the column $\text{[math]}$ of the coefficient $\text{[math]}$ .
`VALUE`	Real value of the coefficient $\text{[math]}$ .

For a solid or anisotropic shell or membrane element equipped with a numerically-enforced plane stress counterpart of a 3D material law (seeMATLAW), the constitutive matrix C relates the stresses to the engineering strains in the element's local frame system {x ; y ; z} as follows:

For a (Kirchhoff) shell element that is not equipped with a numerically-enforced plane stress counterpart of a 3D material law (see MATLAW), the constitutive matrix C relates the forces and moments to the mid-surface strains and curvatures in the shell element's local frame system {x ; y ; z} as follows:

The element's local axes are defined with respect to the global reference frame by the three vectors defined in the CFRAMES command for the corresponding composite (orthotropic, or anisotropic) frame number that is specified in the ATTRIBUTES section. For shell elements, the constitutive matrix, C, can be decomposed into sub-matrices containing the bending and membrane properties of the shell element:

Note the absence of the transverse shear behavior, as can be expected from a Kirchhoff type shell element. In the case of an isotropic material, or a single layer orthotropic or orthotropic material, there is no coupling between the bending and membrane behavior:

For an isotropic material, the membrane constitutive matrix can be defined in terms of the Young's modulus, E, Poisson's ratio,

\text{[math]}

, and shell thickness, h as:

Using the COEF sub-command, different values of E,

\text{[math]}

, and h can be utilized for building the membrane and bending components of the constitutive law, for example, if one wishes to adjust in some specific manner the bending and membrane behaviors of the shell element.

When the COEF sub-command keyword is used for a shell element that is not equipped with a numerically-enforced plane stress counterpart of a 3D material law (see MATLAW), the MATERIAL command must be used as follows: both structural and non-structural mass densities per unit area (see the section Notes in MATERIAL for the definition of a non-structural mass) must be inputted at the fourth position after the attribute number, and for shells, the total thickness must also be defined at the seventh position after the attribute number if a stress analysis is requested.

For shell elements, if the pre-integrated constitutive matrix C is not available, the LAYC or LAYN sub-command keywords (or their counterparts LAYD, LAYO and LAYMAT) should be used to input the material properties and geometrical characteristics of each composite layer. If either LAYN or LAYO is used, no coupling between bending and membrane effects is enforced explicitly during integration through the thickness — that is:

\text{[math]}

\text{[math]}

and

\text{[math]}

The input format given below is the same for both LAYC and LAYN sub-commands.

The input format given below is the same for both LAYD and LAYO sub-commands.

LAYD (or LAYO) attribute#

$\text{[math]}$ LAYER_MATERIAL_ID $\text{[math]}$
LAYMAT
LAYER_MATERIAL_ID $\text{[math]}$
or
LAYER_MATERIAL_ID $\text{[math]}$

.
.
.

LAYER_MATERIAL_ID $\text{[math]}$
or
LAYER_MATERIAL_ID $\text{[math]}$

`LAYC, LAYD, LAYN, or LAYO`	Sub-command keyword used for inputting geometrical and material properties for each layer of a composite shell element (characters).
`attribute#`	Integer value that corresponds to the composite (orthotropic) attribute of the element.
$\text{[math]}$	Integer value that corresponds to the layer number.
$\text{[math]}$	Young's modulus in the local direction $\text{[math]}$ (that is, in the direction of the fibers for the $\text{[math]}$ layer).
$\text{[math]}$	Young's modulus in the local direction $\text{[math]}$ (that is, in the direction orthogonal to the fibers for the $\text{[math]}$ layer).
$\text{[math]}$	Poisson's ratio for transverse strain in the local direction $\text{[math]}$ when stressed in the local direction $\text{[math]}$ for $\text{[math]}$ = constant and all other stresses zero.
$\text{[math]}$	Transverse shear modulus in the plane $\text{[math]}$ of the layer.
$\text{[math]}$	Coefficient of mutual influence of the first kind which characterizes stretching in the local direction $\text{[math]}$ caused by shear in the plane $\text{[math]}$ of the layer for $\text{[math]}$ = constant and all other stresses zero.
$\text{[math]}$	Coefficient of mutual influence of the first kind which characterizes stretching in the local direction $\text{[math]}$ caused by shear in the plane $\text{[math]}$ of the layer for $\text{[math]}$ = constant and all other stresses zero.
$\text{[math]}$	Density (mass per unit volume) of the structural mass type of the material of the $\text{[math]}$ layer (real).
$\text{[math]}$	Thickness of the $\text{[math]}$ layer.
$\text{[math]}$	Angle between a reference vector and the fibers in the layer that defines the orientation of these fibers. If `CMP_FRM#` is specified as an attribute for an element containing this layer under the ATTRIBUTES command, the reference vector is the projection onto the plane of that element of the first of the three vectors defining a local frame for this element and specified in the CFRAMES command. On the other hand, if a reference angle $\text{[math]}$ is specified as an attribute for an element containing this layer under the ATTRIBUTES command, the reference vector is the vector obtained by rotating the directional edge connecting local nodes 1 and 2 of this element around its normal by an angle equal to $\text{[math]}$ . In both cases, this angle must be inputed in degrees.
$\text{[math]}$	Coefficient of thermal expansion in the direction $\text{[math]}$ . It can be omitted, in which case its default value is 0.
$\text{[math]}$	Coefficient of thermal expansion in the direction $\text{[math]}$ . It can be omitted, in which case its default value is 0.
$\text{[math]}$	Coefficient of thermal expansion associated with the in-plane shear strain. It can be omitted, in which case its default value is 0.
`LAYER_MATERIAL_ID`	Identifier of a set of material properties (integer).
`LAYMAT`	Sub-command keyword that can be used for inputting the properties of a layer when it is made of a two-dimensional orthotropic material (characters).

The report number CU-CAS-94-16, “The 3-node Composite Shell and Isotropic Timoshenko Beam Elements” by Fran\c cois M. Hemez, provides a detailed description of the theory and implementation for the type-20 composite (orthotropic) shell element.

24 COMPOSITE (ORTHOTROPIC SHELL OR ANISOTROPIC SOLID) ELEMENT FRAMES

The CFRAMES command statement is used to specify the orientation of composite laminates and orthotropic or anisotropic elements with respect to the global reference frame. The input format of this command is given below with the number of lines equal to the number of different composite (or orthotropic or anisotropic) element frames referenced in the ATTRIBUTES command.

`CMP_FRM#`	Identification of a composite frame (integer).
$\text{[math]}$	The first axis, the local x-axis, expressed in the global frame. For `LAYC` and `LAYN` type composites, the orientation of the fibers of the layers should be defined with respect to the projection of this axis onto the plane of the element.
$\text{[math]}$	The second axis of the frame expressed in the global frame (floats).
$\text{[math]}$	The third axis of the frame expressed in the global frame (floats).

25 CONDITION NUMBER

The CONDITION command statement is used to request the evaluation of the condition number of the system being solved by FEM. The input format is given below.

`TOLERANCE`	Error tolerance for computing the lowest and highest eigenvalues of the finite element model using the inverse power and power methods, respectively (float). The default value is $\text{[math]}$ .
`MAXITR`	Maximum number of iterations for computing the lowest and highest eigenvalues of the finite element model using the inverse power and power methods, respectively (integer). The default value is $\text{[math]}$ .

26 CONSTRAINTS

The CONSTRAINTS command statement is used to specify a default method for enforcing the constraints defined or associated with a problem. Its input format is given below.

Note 2: The augmented Lagrangian method for enforcing constraints is currently available only for NONLINEAR static and NONLINEAR implicit dynamic analyses.

Note 3: The elimination method is supported only by the following equation solvers (see STATICS): skyline, sparse, mumps in the context of a single domain, and spooles. Furthermore, this method is currently supported only when applied to all constraints: in other words, it cannot be combined with another method for enforcing constraints.

`METHOD`	Specified default method for enforcing constraints (characters). This specified method can be overruled in the CONTACTSURFACES, MATERIAL, LMPC, NODALCONTACT, and TIEDSURFACES commands.
`multipliers`	In this case, which is also the default case, AERO-S uses the Lagrange multiplier method for enforcing all constraints associated with the LMPC, NODALCONTACT, CONTACTSURFACES, and TIEDSURFACES commands, and with joint and rigid elements (see TOPOLOGY). Warning: before relying on this default value of `METHOD`, the user should read above the notes describing the scope of the Lagrange multiplier method.
`elimination [factol [lhstol [rhstol]]]`	In this case, AERO-S uses an elimination method for enforcing all constraints associated with the commands LMPC and TIEDSURFACES, and with joint and rigid elements (see TOPOLOGY). This method can be configured with the following three parameters: `factol`. This parameter is a tolerance used in the factorization of the constraint Jacobian matrix to define a zero pivot as a pivot whose absolute value is less or equal to `factol` $\text{[math]}$ \|maxdiagcoeff\|, where $\text{[math]}$ is the machine precision and maxdiagcoeff is the largest diagonal coefficient of the matrix. Note that the factorization is performed only to compute the Reduced Row Echelon Form (RREF) of the linearized constraint equations if these equations cannot be arranged in such a form by simply permuting the rows and/or columns of the constraint Jacobian matrix. The factorization method is QR if AERO-S is configured with the C++ template library for linear algebra Eigen 3, or the Gauss-Jordan elimination method otherwise. The default value of this parameter is $\text{[math]}$ . `lhstol`. This parameter is another tolerance used to set to zero any coefficient of the left hand side of the RREF of the linearized constraint equations that is smaller than `lhstol` $\text{[math]}$ , where $\text{[math]}$ is the machine precision. The sparsity of this matrix is important for computational efficiency. The default value of this parameter is $\text{[math]}$ . `rhstol`. This parameter is yet another tolerance used to set to zero any coefficient of the right hand side of the RREF of the linearized constraint equations that is smaller than `rhstol` $\text{[math]}$ , where $\text{[math]}$ is the machine precision. The default value of this parameter is $\text{[math]}$ . This method is particularly efficient when `MORTAR_TYPE` in TIEDSURFACES is set to $\text{[math]}$ (AERO-S's dual mortar method) because in this case the constraint equations are constructed in RREF.
`penalty` `beta`	In this case, AERO-S uses the penalty method for enforcing all constraints associated with the LMPC, NODALCONTACT, CONTACTSURFACES, and TIEDSURFACES commands, and with joint and rigid elements (see TOPOLOGY). The parameter `beta` should be a large positive number, typically of the order of $\text{[math]}$ (no default value is provided).
`augmented` `beta`	In this case, AERO-S uses the augmented Lagrangian method for enforcing all constraints associated with the LMPC, NODALCONTACT, CONTACTSURFACES, and TIEDSURFACES commands, and with joint and rigid elements (see TOPOLOGY). The parameter `beta` should be a large positive number, typically of the order of $\text{[math]}$ (no default value is provided).

27 CONSTRUCTING A REDUCED MESH

The computed or updated reduced meshes, the traces of the training ROBs on these meshes, the constant reduced-order information mentioned above, and the offline hyper reduced initial conditions can be outputted using SAMPLMSH in OUTPUT.

Note 5: Repeating within this command the pair of sub-command keywords (PODROB, TRNSOL)

\text{[math]}

times, while using the same single instance of each other sub-command keyword, enables the construction of

\text{[math]}

hyper reduced meshes, one for each ROB specified in PODROB — for example, for equipping a suite of

\text{[math]}

local ROBs with

\text{[math]}

associated reduced meshes.

PODROB <pathandfilename1> dimlrb
DUALBASIS <pathandfilename2> dimldb
TRNSOL <pathandfilename3>
TRNSOL <pathandfilename3> <pathandfilename4>
TRNSOL <pathandfilename3> <pathandfilename4> <pathandfilename5>
DIMENS dimens
SAMFRQ samfrq
EXTFOL flag_ext
SOLVER solver_type
TOLERA tolera
USE_MNB flag_mnb
USE_CMF flag_cmf
USE_ICO flag_ico
USE_STR flag_str
POSCFG
x_scale_factor1 y_scale_factor1 z_scale_factor1
[<pathandfilename1_1> <pathandfilename1_2> ... <pathandfilename1_M>]
x_scale_factor2 y_scale_factor2 z_scale_factor2
[<pathandfilename2_1> <pathandfilename2_2> ... <pathandfilename2_M>]
.
.
.
x_scale_factorN y_scale_factorN z_scale_factorN
[<pathandfilenameN_1> <pathandfilenameN_2> ... <pathandfilenameN_M>]
NDSCFG
nodalcoordinates1
[<pathandfilename1_1> <pathandfilename1_2> ... <pathandfilename1_M>]
nodalcoordinates2
[<pathandfilename2_1> <pathandfilename2_2> ... <pathandfilename2_M>]
.
.
.
nodalcoordinatesN
[<pathandfilenameN_1> <pathandfilenameN_2> ... <pathandfilenameN_M>]

`PODROB`	Sub-command keyword to specify a path and filename for the binary file containing a local or global basis (see ROBC) $\text{[math]}$ (characters).
`<pathandfilename1>`	Path and filename of the binary file containing the (primal) basis $\text{[math]}$ (characters).
`dimlrb`	Specifies the first `dimlrb` columns of the basis stored in `<pathandfilename1>` as the ROB for training (integer). If the basis is not a local one (see ROBC), this parameter should be ignored and the dimension of the training ROB should be specified instead in `dimens` (see below).
`DUALBASIS`	Sub-command keyword for activating reading and using a precomputed dual basis $\text{[math]}$ , in order to precompute the reduced constraint matrix $\text{[math]}$ for a class of constrained problems identified above, using the methods and algorithms also identified above, and outputting this reduced matrix in the reduced mesh file outputted itself in `SAMPLMSH` (see OUTPUT) (characters).
`<pathandfilename2>`	Name of the binary file (including path, if needed) containing the dual ROB $\text{[math]}$ to be read (characters). This file is relevant only for the solution of the class of constrained problems identified above, using the methods and algorithms also identified above. It is generated by the command ROBC and is readable by this command. Note that currently, this ROB cannot be a local dual ROB, but only a global dual ROB.
`dimldb`	Specifies the first `dimldb` columns of the dual basis stored in `<pathandfilename2>` as the ROB for training (integer).
`TRNSOL`	Sub-command keyword to specify a path and filename for the binary file containing the training solutions needed for building the training force vectors (characters).
`<pathandfilename3>`	Path and filename of the binary file containing solution snapshots needed for building training force vectors (characters).
`<pathandfilename4>`	Path and filename of the binary file containing velocity solution snapshots for building training force vectors (characters). The corresponding option is recommended when the finite element model has rotational degrees of freedom, regardless of whether the time-integrator is explict or implicit.
`<pathandfilename5>`	Path and filename of the binary file containing acceleration solution snapshots for building training force vectors (characters). The corresponding option is recommended when the finite element model has rotational degrees of freedom, and the time-integrator is implicit.
`DIMENS`	Sub-command keyword to specify the dimension of the basis stored in `<pathandfilename1>`, when this basis is not a local one (see ROBC) (characters).
`dimens`	Specifies the first `dimens` columns of the non-local basis stored in `<pathandfilename1>` as the ROB for training (integer).
`SAMFRQ`	Sub-command keyword to specify a sampling frequency for the inputted solution snapshots (characters).
`samfrq`	Specifies using every `samfrq`-th solution snapshot for building the training force vectors (integer).
`EXTFOL`	By default, the training force vectors are the internal force vectors. However, this sub-command keyword can be used to define the training force vectors as the union of the internal and external follower (see PRESSURE) force vectors.
`flag_ext`
`On`	In this case, the training force vectors are defined as the union of the internal and external follower (see PRESSURE) force vectors.
`Off`	In this case, the training force vectors are defined as the internal force vectors only.
`SOLVER`	Sub-command keyword to specify the method for computing the reduced mesh and its elements weights (characters).
`solver_type`	Specifies the method for computing the reduced mesh and its elements weights (characters). Five choices are available:
`nnlsqr`	Specifies the Lawson and Hanson Non-Negative Least-Squares (NNLS) method based on the QR factorization algorithm. If a mesh partition is also specified (see DECOMPOSE), this method is executed in parallel using this mesh partition and the `ScaLAPACK` and `MPI` libraries. This is the default method for computing the reduced mesh and its elements weights.
`nnlscg`	Specifies the Lawson and Hanson Non-Negative Least-Squares (NNLS) method based on the CG algorithm. If a mesh partition is also specified (see DECOMPOSE), this method is executed in parallel using this mesh partition and the `MPI` library. This method is also known in the literature as the Non-Negative Conjugate Gradient Pursuit method.
`pfpqr`	Specifies the polytope faces pursuit method based on the QR factorization algorithm. If a mesh partition is also specified (see DECOMPOSE), this method is executed in parallel using this mesh partition and the `ScaLAPACK` and `MPI` libraries.
`pfpcg`	Specifies the polytope faces pursuit method based on the CG algorithm. If a mesh partition is also specified (see DECOMPOSE), this method is executed in parallel using this mesh partition and the `MPI` library.
`lassocg`	Specifies the Least Absolute Shrinkage and Selection Operator (LASSO) method based on the CG algorithm. If a mesh partition is also specified (see DECOMPOSE), this method is executed in parallel using this mesh partition and the `MPI` library.
`TOLERA`	Sub-command keyword to specify a tolerance for controlling the error in energy conservation due to mesh sampling (characters).
`tolera`	Tolerance for controlling the error in energy conservation due to mesh sampling. For example, `tolera` = 0.01 means that 99 % of the energy associated with the training force vectors and the ROB is conserved on the reduced mesh (real).
`USE_MNB`	Sub-command keyword to specify that the inputted ROB is mass-orthonormalized (characters).
`flag_mnb`	Flag for specifying which available ROB instance to select for the assigned task (characters).
`On`	In this case, this command selects the mass-orthonormalized ROB instance for the assigned task (characters).
`Off`	In this case, this command selects the orthonormalized ROB instance for the assigned task (characters).
`USE_CMF`	Sub-command keyword to specify whether to include or not the reduced inertia forces associated with a constant mass matrix in the training of ECSW (characters).
`flag_cmf`	Flag for specifying whether to include or not the reduced inertia forces associated with a constant mass matrix in the training of ECSW (characters).
`On`	In this case, the reduced inertia forces associated with a constant mass matrix are included in the ECSW training procedure, which implies the intent to hyperreduce the reduced-order mass matrix. Consequently, in this case, the reduced-order mass matrix is neither computed within the scope of this command nor stored in the file `<PATHANDFILENAME>.elementmesh.inc` if `SAMPLMSH` is specified as an output result under OUTPUT.
`Off`	In this case, the reduced inertia forces associated with a constant mass matrix are excluded from the ECSW training procedure, which implies the intent to pre-compute rather than hyperreduce the reduced-order mass matrix. Consequently and unless the ROB is mass-orthonormal, the reduced-order mass matrix is pre-computed in this case within the scope of this command and stored in the file `<PATHANDFILENAME>.elementmesh.inc` if `SAMPLMSH` is specified as an output result under OUTPUT. Warning: currently, AERO-S does not support a mechanism for suppressing the output of the reduced-order mass matrix when `flag_cmf` is set to `Off` and the ROB is not mass-orthonormal.
`USE_ICO`	Sub-command keyword to specify whether to hyper reduce or not any high-dimensional initial displacement and/or velocity condition(s) specified in the same ASCII Input Command Data file as this command – and therefore whether to include or not this/these initial condition(s) in the training of ECSW (characters).
`flag_ico`	Flag for specifying whether to include or not the aforementioned initial condition(s) in the training of ECSW (characters).
`On`	In this case, the aforementioned initial condition(s) are included in the ECSW training procedure.
`Off`	In this case, the aforementioned initial condition(s) are not included in the ECSW training procedure.
`USE_STR`	This sub-command keyword is relevant only if `flag_cmf` and/or `flag_ico` are/is set to `On`. It should be used to specify how to train ECSW for the reduced inertia forces associated with a constant mass matrix and/or any specified high-dimensional initial conditions (characters).
`flag_str`	Flag for setting how to train ECSW for the reduced inertia forces associated with a constant mass matrix and/or any specified high-dimensional initial conditions (characters).
`On`	In this case, the contributions to the ECSW training procedure of the reduced inertia forces associated with a constant mass matrix and/or any specified high-dimensional initial conditions are stacked with those of all other reduced forces to be hyper reduced, in order to achieve accuracy for each individual hyper reduction. This setting is strongly recommended for EIGEN and DYNAMICS analyses in the context of the nonparametric probabilistic method for uncertainty quantification, because: in the first case, the reduced mass and stiffness matrices must be accurately hyper reduced; and in the second case, any specified non zero high-dimensional initial condition(s) must by accurately hyper reduced.
`Off`	In this case, the contributions to the ECSW training procedure of the reduced inertia forces associated with a constant mass matrix and/or any specified high-dimensional initial conditions are added to the contributions of all other reduced forces to be hyper reduced, in order to achieve accuracy for the hyper reduction of the balance of all aforementioned terms. This setting is recommended for transient DYNAMICS analysis, when no high-dimensional initial condition requires hyper reduction.
`POSCFG`	Sub-command keyword to specify that the collected training snapshots were computed on different meshes that share however the same connectivity — that is, on meshes that have different position configurations — and whose nodal coordinates differ only by scaling factors in the $\text{[math]}$ , $\text{[math]}$ , and $\text{[math]}$ directions. These scaling factors are defined with respect to the nodal coordinates specified under the NODES command of this ASCII Input Command Data file. Note that even if a single common ROB is assigned to all specified different meshes, using the `POSCFG` sub-command keyword requires that this ROB go first through a clustering process using the ROBC command configured with the `DO_CLUSTERING` sub-command keyword and `nclusters` = 1, in order for AERO-S to build the association between a snapshot and the mesh on which it was computed.
`x_scale_factori`	$\text{[math]}$ -coordinate scale factor for the `i`-th mesh and the case where the collected training snapshots were computed on different meshes (real).
`y_scale_factorj`	$\text{[math]}$ -coordinate scale factor for the `j`-th mesh and the case where the collected training snapshots were computed on different meshes (real).
`z_scale_factork`	$\text{[math]}$ -coordinate scale factor for the `k`-th mesh and the case where the collected training snapshots were computed on different meshes (real).
`<pathandfilenamei_j>`	Name of the optional binary file (including path, if needed) containing (characters): The `j`-th mass-orthonormalized local ROB computed on the `i`-th mesh, when model reduction is to be based on local ROBs. The global mass-orthonormalized ROB computed on the `i`-th mesh, otherwise. Note that this optional entry should be omitted (for the sake of computational efficiency) when the training on different meshes is to be performed using orthonormal ROBs. Note also that the aforementioned ROBs can be efficiently constructed using the `COMPRESS` sub-command of the ROBC command (instead of performing SVD multiple times using different mass metrics).
`NDSCFG`	Sub-command keyword to specify that the collected training snapshots were computed on different meshes that share however the same connectivity — that is, on meshes that have different position configurations — and whose nodal coordinates differ by an arbitrary manner. Note that even if a single common ROB is assigned to all specified different meshes, using the `NDSCFG` sub-command keyword requires that this ROB go first through a clustering process using the ROBC command configured with the `DO_CLUSTERING` sub-command keyword and `nclusters` = 1, in order for AERO-S to build the association between a snapshot and the mesh on which it was computed.
`nodalcoordinatesi`	Name of the binary file (including path, if needed) containing the nodal coordinates of the `i`-th mesh.

28 CONTACT SURFACES

The CONTACTSURFACES command can be used to enforce contact laws between pairs of surfaces defined using the command SURFACETOPO, for static and dynamic analyses only. Surface interactions are detected using the search module of the library ACME. For explicit computations, the discrete kinematic constraint equations are defined and enforced as specified in the sub-command keyword TDENFORCE and its associated flag flagTDENFORCE of the DYNAMICS object. For implicit computations, the discrete kinematic constraint equations are formulated using AERO-S's mortar method and enforced using the method specified in CONSTRAINTS or in CONSTRAINT_METHOD below with the following limitation: in this case, the enforcement method can be only one of the following three methods: the penalty method, the Lagrange multiplier method, or the augmented Lagrange multiplier method.

Note 2: For explicit dynamic computations performed with the flag TDENFORCE set to On (see DYNAMICS), the contact forces can be computed using one of the following four enforcement models: frictionless (default), constant friction, velocity-dependent friction, and pressure-dependent friction. For all other computations (for example, for explicit dynamic computations performed with the flag TDENFORCE set to Off, implicit dynamic or static computations) only the frictionless model is supported.

Note 3: The enforcement of contact surface constraints by the Lagrange multiplier method in static and implicit dynamic analyses is supported only by the FETI-DP family of solvers.

Note 4: The enforcement of contact surface constraints by the elimination method is not supported.

Note 5: For contact detection and enforcement, a surface is treated as 2-sided (or “shell” surface) when both of the following conditions are met: (a) the simulation is explicit dynamics with flagTDENFORCE set to On in DYNAMICS (or omitted since this is the default setting), and (b) a surface thickness attribute is specified under SURFACETOPO. In all other cases, the contact detection and enforcement is 1-sided. For a 1-sided surface, the directions of the normals to the faces of the surface are important. Contact interactions between two 1-sided surfaces, or self-contact involving one 1-sided surface, can only be detected between two faces with normals in opposite directions. Furthermore, if an interaction is detected, the directions of the normals establish whether the configuration involves penetration or separation. For a 2-sided surface, the directions of the normals of the faces of the surface are not important. Contact interactions between two 2-sided surfaces, or self-contact involving one 2-sided surface, can be detected between two faces regardless of the directions of the normals. For contact between one 2-sided surface and one 1-sided surface, only the normal direction of the 1-sided surface is important. If an interaction is detected, the direction of the normal of the 1-sided surface establishes whether the configuration involves penetration or separation.

SURF_PAIR_ID# MASTER SLAVE MORTAR_TYPE NORMAL_TOL TANGENTIAL_TOL CONSTRAINT_METHOD

For an explicit dynamic computation with the flag flagTDENFORCE set to On (see DYNAMICS) and a frictionless model

SURF_PAIR_ID# MASTER SLAVE KPART_TYPE NORMAL_TOL TANGENTIAL_TOL NUM_ITER CONVERG_TOL CONSTRAINT_METHOD

For an explicit dynamic computation with the flag flagTDENFORCE set to On (see DYNAMICS) and a constant friction model

SURF_PAIR_ID# MASTER SLAVE KPART_TYPE NORMAL_TOL TANGENTIAL_TOL NUM_ITER CONVERG_TOL FRIC_COEF CONSTRAINT_METHOD

For an explicit dynamic computation with the flag flagTDENFORCE set to On (see DYNAMICS) and a velocity dependent friction contact model

SURF_PAIR_ID# MASTER SLAVE KPART_TYPE NORMAL_TOL TANGENTIAL_TOL NUM_ITER CONVERG_TOL STATIC_COEF DYNAMIC_COEF VELOCITY_DECAY CONSTRAINT_METHOD

For and explicit dynamic computation with the flag flagTDENFORCE set to On (see DYNAMICS) and a pressure-dependent friction contact model

SURF_PAIR_ID# MASTER SLAVE KPART_TYPE NORMAL_TOL TANGENTIAL_TOL NUM_ITER CONVERG_TOL FRIC_COEF REF_PRES OFFSET_PRES PRES_EXP CONSTRAINT_METHOD

`SURF_PAIR_ID#`	Id number of the surface pair to be described (integer).
`MASTER`	Identification of the master (mortar method) surface (see SURFACETOPO) (integer).
`SLAVE`	Identification of the slave (mortar method) surface (see SURFACETOPO) (integer).
`CONSTRAINT_METHOD`	Method for enforcing the associated constraints (characters). The default method is set in CONSTRAINTS and used whenever this entry is omitted.
`multipliers`	The Lagrange multiplier method.
`penalty` `beta`	The penalty method. The parameter `beta` should be a large positive number, typically of the order of $\text{[math]}$ (no default value is provided).
`augmented` `beta`	The augmented Lagrangian method. The parameter `beta` should be a large positive number, typically of the order of $\text{[math]}$ (no default value is provided). If penetration occurs, the value of `beta` should be increased and the value of the computational time-step specified in DYNAMICS decreased.
`MORTAR_TYPE`	Mortar type: 0 = standard, 1 = dual, default value is 0 (integer).
`NORMAL_TOL`	Normal search tolerance used by `ACME` to identify interactions. The default value is 0.1 (float) (see Figs. 1.2 and 1.3 in Section 1.3 of ACME's User Reference Manual). This tolerance should be larger than the maximum relative displacement occurred during one load step of a static simulation or one time-step of a dynamic one. If penetration occurs, the value of this parameter should be increased. For a surface with a surface thickness value, the normal tolerance is defined w.r.t. the position/s of the “lofted” surface/s. For a 1-sided surface, this is the position of the surface + 0.5surface thickness in the direction of the normal. For a 2-sided surface, these are the positions of the surface +/- 0.5surface thickness. The normal tolerance must be greater than the distance that a point on the contact surface can move in one time/load step. Therefore, a larger computational time/load step calls for a larger normal tolerance. For contact between two 2-sided surfaces, the normal tolerance must be less than the sum of the two surface thickness values. Also, for self-contact of a 2-sided surface, the normal tolerance must be less than twice the surface thickness value. Even for contact involving one or more 1-sided surfaces, there may be certain cases where it would be appropriate to limit the normal tolerance in order to prevent particular configurations from being treated as penetration. Increasing the normal tolerance will make the contact detection more robust, provided the aforementioned upper limits are respected. However, it also makes the simulation more expensive.
`TANGENTIAL_TOL`	Tangential search tolerance used by `ACME` to identify interactions. The default value is 0.001 (float) (see Figs. 1.2 and 1.3 in Section 1.3 of ACME's User Reference Manual). If penetration occurs, this tolerance should be increased, in which case the simulation should be expected to become slower. The value of this parameter should be neither too small nor too large. A value corresponding to a small percentage (between 0.5% and 50%) of the minimum edge length of the face elements is suggested.
`KPART_TYPE`	In `ACME`, kinematic partitioning pertains to determining the fraction $\text{[math]}$ of the total momentum to be absorbed by each surface of a pair of surfaces in contact. If surface 1 is in contact with surface 2 and the kinematic partitioning fraction for surface 1 is $\text{[math]}$ , it is $\text{[math]}$ for surface 2. One specific value of the kinematic partitioning factor $\text{[math]}$ can be inputted to `ACME` (see below), or this factor can be automatically computed by `ACME` for each contact interaction as follows $\text{[math]}$ where $\text{[math]}$ , $\text{[math]}$ , is the kinematic partitioning fraction for surface $\text{[math]}$ , $\text{[math]}$ is the density at a given node of this surface, and $\text{[math]}$ is the speed of sound in the material of which this surface is made. Setting `KPART_TYPE` to 0 specifies $\text{[math]}$ for the slave surface (see `SLAVE`) and $\text{[math]}$ for the master surface (see `MASTER`). Setting `KPART_TYPE` to 1 specifies that $\text{[math]}$ and $\text{[math]}$ are to be automatically computed by `ACME` as outlined above. The default value of `KPART_TYPE` is 0 (integer).
`NUM_ITER`	Maximum number of predictor-corrector iterations to be performed at each time step. The default value is 5 (integer).
`CONVERG_TOL`	Convergence tolerance of the predictor-corrector iteration loop. The default value is 1.0e-10 (float).
`FRIC_COEF`	Friction coefficient (float).
`STATIC_COEF`	Static friction coefficient (float).
`DYANAMIC_COEF`	Dynamic friction coefficient (float).
`VELOCITY_DECAY`	Velocity decay parameter (float).
`REF_PRES`	Reference pressure (float).
`OFFSET_PRES`	Offset pressure (float).
`PRES_EXP`	Pressure exponent (float).

29 CONTROL STATEMENT

AERO-S always generates a performance file named FNAME.timing which reports on the complexity, memory, and CPU resources associated with the performed computation. By default, the prefix FNAME is set to the name of the AERO-S input file (AERO-S also outputs some of these performance results on the screen). This optional command statement can be used to reset the value of the prefix FNAME. This prefix is also used by AERO-S, when executed with the “-t” (or “-T”) option, to name the ASCII output file (FNAME.top) containing the geometry of the performed computation in the XPost format. It is also used by AERO-S for outputting, when requested, a number of domain decomposition (or mesh partitioning) files (see DECOMPOSE).

Currently, this command is also needed for specifying the type of analysis to be performed by AERO-S. For this reason, it features the entry ANATYPE described below. For parsing reasons, ANATYPE must be specified whenever the CONTROL command is included in the input file, even this entry is not needed.

`FNAME`	Prefix of the names of the files reporting on the performance, geometry, and mesh decomposition of the performed computation, when applicable. The default value, which is applicable when this optional command is entirely skipped, is the name of the AERO-S input file.
`ANATYPE`	Analysis type identifier (integer). It is needed for any thermal (heat conduction) analysis involving radiation, in which case it must be set to 2. Otherwise, this parameter should be set to 1.
`NODESET`	Name of the node set describing the grid points of the geometry of the computation in the file `FNAME.top` outputted in the XPost format, when AERO-S is executed with the “-t” (or “-T”) option. The default name is “nodes”.
`ELEMSET`	Name of the element set describing the connectivity of the geometry of the computation in the file `FNAME.top` outputted in the XPost format, when AERO-S is executed with the “-t” (or “-T”) option. The default name is “elems”.

30 CONWEP

The CONWEP command statement is used to define, in conjunction with the PRESSURE command, a pressure load due to air blast in the free field using the software module CONWEP. More specifically, the CONWEP command is used to specify the position of the charge, its mass, and the detonation time. The PRESSURE command is used to specify those elements of the finite element model on which to apply the generated pressure load.

`XCHARGE`	x-ordinate of the charge (real).
`YCHARGE`	y-ordinate of the charge (real).
`ZCHARGE`	z-ordinate of the charge (real).
`MCHARGE`	Mass of the explosive charge (real).
`DTIME`	Time at which the charge is detonated (real).

31 DENSITY-TEMPERATURE TABLE

The DCTT command can be used to describe, for a given material, the evolution of the mass density with temperature. This evolution can be specified here in a curve (or one-dimensional table) defined by pairs of density and temperature values. Linear interpolation is used for "in between" points, and the extrema values are adopted for "outside" points. Several curves can be specified, one after the other. Each curve is identified by an ID number as described below.

Note 1: Currently, this command is supported only by the 4-noded tetrahedral termal element (type 50).

`CURVE`	Sub-command keyword (characters) that signals the definition of a density-temperature curve (or one-dimensional table).
`curve_id`	ID number for the following curve (or one-dimensional table) (integer).
`T_i`	A specified temperature value (real).
$\text{[math]}$	A specified mass density value at temperature `T_i` (real).

32 DISCRETE NODAL MASS AND INERTIA

The command DIMASS is used to lump a discrete mass or inertia on a specified degree of freedom attached to a specified node, either for a diagonal contribution to the mass matrix or an off-diagonal one. If a node number appears more than once under this command with the same degree of freedom (or pair of degrees of freedom), AERO-S sums all the lumped masses at the implied entries of the mass matrix. If a gravity field is also specified in the input file using the command GRAVITY, AERO-S generates at each specified translational degree of freedom at each specified node under this command a weight-force component equal to the product of the specified discrete mass and specified gravity acceleration in the corresponding direction.

`NODE#`	Node number where the mass or inertia will be added (integer).
`DOF#`	Degree of freedom for which the mass or inertia will contribute a diagonal entry to the mass matrix (integer).
`VALUE`	Value of the prescribed discrete mass or inertia (float).
`DOF1#`	Degree of freedom for which the specified mass or inertia will contribute an off-diagonal entry (and its symmetric counterpart) to the mass matrix at the location implied by this degree of freedom and that specified in `DOF2#` (integer). Note that only the contribution to the lower triangular part of the mass matrix should be specified, and therefore `DOF1#` should be greater than `DOF2#`. Note also that for an explicit time-integration scheme or when the mass is requested to be LUMPED, this contribution will be part of the lumping process.
`DOF2#`	Degree of freedom for which the mass or inertia will contribute an off-diagonal entry (and its symmetric counterpart) to the mass matrix at the location implied by this degree of freedom and that specified in `DOF1#` (integer). Note that only the contribution to the lower triangular part of the mass matrix should be specified, and therefore `DOF2#` should be smaller than `DOF1#`. Note also that for an explicit time-integration scheme or when the mass is requested to be LUMPED, this contribution will be part of the lumping process.

If more than one line addressing the same degree of freedom of the same node are encountered under this command, the effect is the accumulation of the lumped masses or inertias at this degree of freedom.

33 DYNAMIC ANALYSIS

Note that for the purpose of structural dynamic analysis, structural damping can be represented in AERO-S using two different approaches:

Note 2: Whenever an implicit time-integration algorithm is selected, an equation solver must be specified under the STATICS command.

Note 3: For nonlinear thermal analysis (see NONLINEAR), the appropriate midpoint rule algorithm is automatically selected by this command.

Note 4: Currently, the reduction of inequality constraints such as those associated with contact problems is supported only for nonlinear implicit structural dynamic computations, and only for those cases where the constraints are linear and enforced using the Lagrange multipliers method.

STABLE
MODAL
SROM
TROM
MECH
MECH
MECH
ACOU
ACOU
ACOU
ACOU
HEAT
TIME
RAYDAMP
MODDAMP
MODE#
.
.
MODE#
TDENFORCE
IAEROF
de>IACC

flagIACC

option

coeff

tol

maxitr

freq

smsc

dedt

rob_id_1

[rob_id_2

...

rob_id_L]

[CONTACT rob_id_L+1]

$\text{[math]}$

(midpoint implementation of Newmark — that is, $\text{[math]}$ )

$\text{[math]}$

(generalized $\text{[math]}$ )

$\text{[math]}$

(generalized $\text{[math]}$ )

$\text{[math]}$

(midpoint implementation of Newmark — that is, $\text{[math]}$ )

$\text{[math]}$

(generalized $\text{[math]}$ )

$\text{[math]}$

(generalized $\text{[math]}$ )

$\text{[math]}$

(modified wave equation method)

$\text{[math]}$

th

tm

tt

$\text{[math]}$

MDV

flagTDENFORCE

[maxItrTDENFORCE

tolTDENFORCE

tiTDE

tfTDE]

flagIAEROF

`IACC`	For both linear and nonlinear explicit and implicit dynamic computations, the initial acceleration can be either set to zero, or computed by AERO-S to satisfy equilibrium at $\text{[math]}$ . The sub-command keyword `IACC` enables the user to make this choice (characters).
`flagIACC`	`On`/`Off` flag (characters). The default value is `On`.
`On`	In this case, the acceleration is automatically initialized by AERO-S to satisfy equilibrium at $\text{[math]}$ . This initialization requires the solution of a linear system of equations where the left-hand side operator is the mass matrix. For implicit dynamic computations, the solver specified under STATICS command is used for this purpose.
`Off`	In this case, the acceleration is automatically initialized by AERO-S to zero.
`STABLE`	Sub-command keyword for managing the time-step of a linear or nonlinear, structural dynamic or acoustic time-integration using the explicit central difference method (characters).
`option`	This integer parameter specifies how to manage the computational time-step for an explicit simulation.
`0`	In this case, the time-step is not managed and the computations are performed using the specified computational time-step `tm` (see below).
`1`	In this case, which is also the default case, AERO-S estimates automatically the critical time-step — that is, the maximum stability time-step — and multiplies it by the specified coefficient `coeff` (see below). In the case of the linear explicit central difference method, AERO-S estimates the critical time-step by computing the largest eigenvalue of the finite element model using the power method. In the case of the nonlinear explicit central difference method, AERO-S estimates the critical time-step by an element-dependent method and updates this estimate every `freq` time-steps. If the specified computational time-step `tm` (see below) is larger than the product of the critical time-step and `coeff`, this product is used instead for the computation.
`2`	In this case, AERO-S computes automatically the critical time-step as described above for `option` = 1. However in this case, the explicit computations are performed using a computational time-step equal to the product of the estimated critical time-step and `coeff` (see below), regardless of the value of the specified computational time-step `tm` (see below).
`coeff`	Real-valued coefficient for managing the computational time-step (see above). The default value is $\text{[math]}$ .
`tol`	Error tolerance for computing the highest eigenvalue of the finite element model using the power method (real). The default value is $\text{[math]}$ .
`maxitr`	Maximum number of iterations for computing the highest eigenvalue of the finite element model using the power method (integer). The default value is $\text{[math]}$ .
`freq`	Integer parameter specifying the frequency (every so many time-steps) at which the critical time-step is re-estimated during nonlinear explicit computations (see above). The default value is $\text{[math]}$ .
`smsc`	Integer-valued parameter that can be used to activate selective mass scaling. The default value is $\text{[math]}$ .
`0`	In this case, no selective mass scaling is performed.
`1`	In this case, selective mass scaling is activated for nonlinear, explicit dynamic computations. Specifically, if at the start of the simulation the stability time-step of an element is less than `tm` (see below), the element mass matrix of that element is scaled so that its stability time-step is equal to `tm`.
`dedt`	Real-valued parameter that can be used to activate element deletion using a minimum stability time-step criterion. The default value is $\text{[math]}$ . If at any time the stability time-step of an element is less than the specified value of this parameter, the element is deleted. This option is enabled only for nonlinear, explicit dynamic computations.
`MODAL`	Sub-command keyword (characters) for: Requesting the construction of a linear structural dynamic ROM based on a Reduced-Order Basis (ROB) of the type `eigen` — and therefore consisting of mass-orthonormalized eigen vectors — which must be inputted using the first format of the READMODE command. Performing the requested linear structural dynamic analysis using this structural dynamic ROM — which amounts to performing a linear modal superposition analysis. As in the case of a dynamic analysis using direct time-integration, the initial displacement and velocity conditions can be inputted in a generalized coordinates system, the finite element coordinates system, or both (see IDISPLACEMENTS and IVELOCITIES). If `tt` (see below) is set to zero, AERO-S will exit after constructing the requested structural dynamic ROM.
`SROM`	Sub-command keyword (characters) for: Requesting the construction offline of a structural dynamic ROM based on: A primal ROB which must be inputted using the second format of the READMODE command and identified by `rob_id_1` (see below). And when applicable, a dual ROB which must be inputted using the second format of the READMODE command and identified using `rob_id_L+1` (see below). Requesting the construction offline of a structural dynamic ROM for an unrestrained structural system, in a floating reference frame, based on (see FLOATINGFRAME): The rigid body modes of the system, which are automatically computed by AERO-S. A (partial) primal ROB associated with the flexible modes of the system, which must be inputted using the second format of the READMODE command and identified using `rob_id_1` (see below). The modal superposition of all aforementioned modes, which is characterized in general by a nonlinear coupling between the rigid and flexible structural modes. Performing the requested structural dynamic analysis online using the constructed structural dynamic ROM. In the case of a standard ROM, the initial displacement and velocity conditions can be inputted in a generalized coordinates system, the finite element coordinates system, or both (see IDISPLACEMENTS and IVELOCITIES) — that is, as in the case of a dynamic analysis using direct time-integration. In the case of a structural dynamic ROM formulated in a floating reference frame, the initial values of the generalized velocity degrees of freedom (dofs) associated with the rigid body modes should be specified in FLOATINGFRAME using the `RMIV` sub-command keyword and those of the dofs associated with the structural deformation modes should be specified in IVELOCITIES using the `MODAL` sub-command keyword. Reconstructing the high-dimensional solution offline using RODC, the ROB — or local ROBs — specified in this command via `rob_id_1` — or `rob_id_1`, `rob_id_2` ... `rob_id_L` — and inputted in READMODE. If `tt` (see below) is set to zero, AERO-S will exit after constructing the requested structural dynamic ROM.
`rob_id_1`	Integer number identifying the primal structural ROB inputted using READMODE (integer). Its default value is 0. Note that whereas a mass-orthonormalized primal structural ROB can be used for both explicit and implicit dynamic computations using the corresponding SROM, an identity-orthonormalized primal structural ROB can be used only for implicit dynamic computations using the corresponding SROM.
`rob_id_2` ... `rob_id_L`	Optional suite of integer numbers identifying a suite of primal local ROBs, in which case model reduction based on the method of local ROBs is activated (integers). Note that whereas a mass-orthonormalized primal structural ROB can be used for both explicit and implicit dynamic computations using the corresponding SROM, an identity-orthonormalized primal structural ROB can be used only for implicit dynamic computations using the corresponding SROM.
`CONTACT`	Optional sub-command keyword specifying that the following entry pertains to a dual ROB needed for the reduction of a contact problem (characters).
`rob_id_L+1`	Optional integer number identifying the dual structural ROB inputted using READMODE (integer). It is needed only for the reduced-order solution of contact problems.
`TROM`	Sub-command keyword (characters) for: Requesting the construction of a linear dynamic thermal (heat transfer) ROM based on an identity-orthogonal POD ROB inputted using READMODE. Performing the requested linear dynamic thermal analysis using this linear thermal ROM. If `tt` (see below) is set to zero, AERO-S will exit after constructing the requested linear dynamic thermal ROM.
`MECH` or `ACOU` or `HEAT`	The sub-command keyword `MECH` can be used to request a structural dynamic analysis (characters). The sub-command keyword `ACOU` can be used to request a time-domain acoustic analysis (characters). The sub-command keyword `HEAT` can be used to request a thermal (heat transfer) analysis (characters).
$\text{[math]}$	Newmark coefficient $\text{[math]}$ for a second-order system (real). Set $\text{[math]}$ $\text{[math]}$ and $\text{[math]}$ to specify the explicit central difference method.
$\text{[math]}$	Newmark coefficient $\text{[math]}$ for a second-order system (real).
$\text{[math]}$	Generalized $\text{[math]}$ coefficient $\text{[math]}$ for a second-order system (real). To obtain the standard Newmark algorithm, set $\text{[math]}$ . The default is $\text{[math]}$ .
$\text{[math]}$	Generalized $\text{[math]}$ coefficient $\text{[math]}$ for a second-order system (real). To obtain the standard Newmark algorithm, set $\text{[math]}$ . The default is $\text{[math]}$ .
$\text{[math]}$	Generalized $\text{[math]}$ infinite frequency spectral radius for a second-order system (real). When this option is used and this coefficient is specified in the range $\text{[math]}$ , $\text{[math]}$ , $\text{[math]}$ , $\text{[math]}$ and $\text{[math]}$ are automatically set to $\text{[math]}$ which results in a second-order unconditionally stable scheme that minimizes low frequency dissipation. The parameter $\text{[math]}$ can be set to dissipate higher frequencies — which are usually spurious, numerical frequencies — while minimizing the dissipative side effect of the lower frequencies. For $\text{[math]}$ , the midpoint rule is recovered. Otherwise, the smaller is the value attributed to $\text{[math]}$ within the range $\text{[math]}$ , the larger is the set of higher frequencies that are dissipated and the larger is the amount of dissipation that is introduced for these frequencies. This option is particularly useful for stabilizing dynamic fluid-structure computations in the presence of constraints or rigid elements, as these introduce infinite frequencies in the numerical model. In this case, $\text{[math]}$ is a recommended value, but the optimal value is problem dependent.
$\text{[math]}$	For $\text{[math]}$ , the explicit modified wave equation method is fourth-order time-accurate. Furthermore, for many applications, experience shows that for $\text{[math]}$ , this method behaves almost like a sixth-order time-accurate scheme.
`HEAT`	Sub-command keyword which preceds the parameter of the Newmark algorithm for a first-order time-dependent system (characters).
$\text{[math]}$	Main parameter of the generalized trapezoidal family of methods for first-order systems (real). This parameter must be chosen within $\text{[math]}$ .
`TIME`	Sub-command keyword for specifying time-interval parameters (characters).
`th`	Integration time-step for thermal analysis (real). This time-step should be put to zero if a structural dynamic or time-domain acoustic analysis is to be performed.
`tm`	Integration time-step for a structural dynamic or time-domain acoustic analysis (real).
`tt`	End of time-interval for time-integration (real); beginning of time-interval for time-integration is zero for all types of time-dependent analyses.
`RAYDAMP`	This sub-command keyword is active only in the context of the option `MECH`. It is used for specifying global Rayleigh proportional damping coefficients — that is, Rayleigh proportional damping coefficients to be applied to the entire structure (characters). However, these coefficients are treated as default values as they can be overwritten by specifying counterpart material- or element-level coefficients in MATERIAL.
$\text{[math]}$	Rayleigh damping stiffness coefficient (real). In the nonlinear case, this coefficient is assigned at each iteration to the initial linearized stiffness matrix and the product of these two quantities, which remains constant through the nonlinear iterations, constitutes the contribution to the damping term.
$\text{[math]}$	Rayleigh damping mass coefficient (real).
`MODDAMP`	Sub-command keywords for signaling that the following lines specify modal damping ratios (characters). This option is active only when the sub-commands `MECH` and `MODAL` are also specified — that is, for a dynamic analysis of a mechanical system using modal superposition. If a mode is repeated, the modal damping ratio values are added for that mode. If both `RAYDAMP` and `MODDAMP` commands are specified, and the keyword `MODAL` is also specified, then modal damping takes precedence over Rayleigh damping.
`MODE#`	Mode ID number (integer).
`MDV`	Modal damping ratio (also known as modal damping factor and modal $\text{[math]}$ of critical damping and usually denoted by $\text{[math]}$ ) for mode `MODE#` (real).
`TDENFORCE`	For implicit dynamic computations with TIEDSURFACES and/or CONTACTSURFACES constraints, the discrete kinematic constraint equations are automatically formulated by AERO-S using its mortar method. In this case, the user can specify in CONSTRAINTS, TIEDSURFACES, or CONTACTSURFACES the penalty, Lagrange multiplier, or augmented Lagrange multiplier method for enforcing these constraints. For explicit dynamic computations with TIEDSURFACES and/or CONTACTSURFACES constraints however, the discrete kinematic constraint equations can be either defined using a node-to-segment approach and enforced using `ACME`'s enforcement module, or defined using AERO-S's mortar method and enforced using its penalty method. `TDENFORCE` is the sub-command keyword which can be used to choose between either of these two options (characters).
`flagTDENFORCE`	`On`/`Off` flag (characters). The default value is `On`.
`On`	In this case, the discrete kinematic constraint equations are defined using a node-to-segment approach and the constraint forces are computed using `ACME`'s enforcement module.
`Off`	In this case, the discrete kinematic constraint equations are defined using AERO-S's mortar method and the constraint forces are computed using its penalty method.
`maxItrTDENFORCE`	Optional parameter that can be used to specify the maximum number of outer iterations for contact enforcement when performed using the library `ACME` (integer). The default value is 1.
`tolTDENFORCE`	Optional parameter that can be used to specify the absolute tolerance for monitoring the convergence of the outer iterations of the contact enforcement performed by the library `ACME` (real). The default value is 0.
`tiTDE`	Optional parameter that can be used to specify the time at which contact detection and enforcement is activated (real). The default value is 0. This parameter can be used to speed up execution time when it can be determined a priori that no contact will occur during the first part of a simulation.
`tfTDE`	Optional parameter that can be used to specify the time at which contact detection and enforcement is deactivated (real). The default value is infinity. This parameter can be used to speed up execution time when it can be determined a priori that no contact will occur during the final part of a simulation.
`IAEROF`	For linear and nonlinear implicit dynamic computations, when `flagIACC` is set to `On` and the AERO command is specified in the AERO-S ASCII Input Command Data file to perform a fluid-structure computation using the tandem AERO-F-AERO-S, the user can request to either ignore or account for the contribution of the initial aeroelastic forces in the computation of the initial acceleration of the structural subsystem. The sub-command keyword `IAEROF` enables the user to make this choice (characters).
`flagIAEROF`	`On`/`Off` flag (characters). The default value is `Off`.
`On`	In this case, `SendInitialForce` must be set to `True` in the ASCII Input Command Data File of AERO-F, in which case the aeroelastic forces are accounted for in the computation of the initial acceleration of the structural subsystem.
`Off`	In this case, `SendInitialForce` must be set to `False` (or omitted) in the ASCII Input Command Data File of AERO-F and the contribution of the initial aeroelastic forces is neglected in the computation of the initial acceleration of the structural subsystem.

34 EIGENVALUE PROBLEMS

The EIGEN command statement is used to request the construction and solution of a generalized eigenvalue problem of the form

where

\text{[math]}

and

\text{[math]}

are two finite element square matrices,

\text{[math]}

is the rectangular matrix of generalized eigenvectors, and

\text{[math]}

is the diagonal matrix of corresponding eigenvalues. Currently, only the subspace iteration method (the default choice) and the ARPACK package are available in AERO-S for this purpose.

The input format of this command is given below. An example input file can be found in FEM.d/fem_examples/Eigen.d.

VERSION
SHIFT

\text{[math]}

NSBSPV nsbspv
NEIGPA neigpa
TOLEIG toleig
TOLJAC toljac
ARPACK which mode
ARPACK lbound nshifts
ARPACK lbound ubound neigps
MAXITR maxitr

`VERSION`
`explicit`	In this case, the $\text{[math]}$ matrix is used explicitly when constructing the reduced generalized eigen problem in the subspace iteration method. Otherwise (default), the reduced generalized eigen problem is constructed by exploiting some mathematical identities to avoid using explicitly the $\text{[math]}$ matrix which has been factored by then. Note that specifying the `explicit` version of the subspace iteration algorithm incurs additional memory storage.
`SHIFT`
$\text{[math]}$	Value of a specified shift for the $\text{[math]}$ matrix (real).
`NSBSPV`
`nsbspv`	In the case of the subspace iteration method (default eigensolver), `nsbspv` denotes the number of subspace iteration vectors and should be set to the minimum between twice the number of requested eigen pairs, $\text{[math]}$ `neigpa`, and `neigpa + 8`. If rigid body modes are expected, the previous formula should be increased by the total number of rigid body modes. In the case of ARPACK, `nsbspv` denotes the number of Krylov vectors (per shift, if a shifting strategy is used).
`NEIGPA`
`neigpa`	Number of requested eigen pairs. If rigid body modes are found, their number is included in the specified value of `neigpa`.
`TOLEIG`
`toleig`	Tolerance for the convergence of the subspace iteration method.
`TOLJAC`
`toljac`	Tolerance for the Jacobi Determinant algorithm used in the subspace iteration method.
`ARPACK`	The presence of this keyword under the `EIGEN` command specifies the usage of the ARPACK eigensolver in the specified mode (see `mode` below). Otherwise, the default choice is the subspace iteration method. The ARPACK choice is required whenever one of the two matrices $\text{[math]}$ or $\text{[math]}$ is indefinite, or one or both of them are singular. Indefinite systems arise: (1) if the analysis involves the HELMHOLTZ, IMPEDANCE, or EIGEN command with a positive shift (see `SHIFT` in EIGEN) or for buckling analysis (see `ARPACK` in EIGEN), or (2) the structural model includes rigid and/or joint elements (see TOPOLOGY), linear multi-point constraints (see LMPC), or tied surfaces (see TIEDSURFACES), and the Lagrange multiplier method is chosen for enforcing the associated constraints (see CONSTRAINTS). In either case, the equation solver must be properly chosen in STATICS.
`which`	Keyword (characters) to specify which eigenpairs to be computed by ARPACK. This keyword can take one of the following values.
`LA`	In this case, the `neigpa` eigenpairs whose eigenvalues are just to the right of the shift $\text{[math]}$ are computed. This is the default value of `which` when the shift is zero ( $\text{[math]}$ ).
`SA`	In this case, the `neigpa` eigenpairs whose eigenvalues are just to the left of the shift $\text{[math]}$ are computed.
`BE`	In this case, `neigpa` eigenpairs with eigenvalues on either side of the shift $\text{[math]}$ are computed. This is the default value of `which` when the shift is non zero ( $\text{[math]}$ ).
`mode`	Integer identifier to specify the mode in which to run ARPACK. It can take one of the following values.
`3`	This default mode, which is the shift-invert mode, is recommended for all generalized eigenvalue problems except those for which the matrix $\text{[math]}$ is indefinite. Hence, this mode is particularly not recommended for buckling analysis.
`4`	This mode is recommended for generalized eigenvalue problems where the matrix $\text{[math]}$ is indefinite. Hence, this mode is particularly recommended for buckling analysis. In this case, a nonzero shift should be specified in `SHIFT` (see above).
`lbound`	Lower bound of a set or range of eigenvalues to be computed by ARPACK (real).
`nshifts`	Number of shifts to be used by ARPACK when computing the `neigpa` eigenvalues that are greater than `lbound` (integer). The specific values of the shifts are automatically selected by ARPACK, and `neigpa`/`nshifts` eigenpairs are computed per shift.
`ubound`	Upper bound of a range of eigenvalues to be computed by ARPACK (real).
`neigps`	When a range of eigenvalues [`lbound`, `ubound`] is specified, ARPACK computes all eigenpairs whose eigenvalues lie within this range. In this case, a first shift is set to `lbound` and `neigps` consecutive eigenvalues within the range [`lbound`, `ubound`] are computed. Then, a recursive procedure in which the largest previously computed eigenvalue is chosen as a new shift and `neigps` new eigenvalues within the range [`lbound`, `ubound`] are computed using this shift is applied until all eigenvalues within the specified range are captured. The default value for `neigps` is 50.
`MAXITR`
`maxitr`	Maximum number of iterations for the eigensolver. The default value is $\text{[math]}$ `nsbspv`.

35 ELEMENT TOPOLOGY *S*

The TOPOLOGY command is used to signal that the following data lines correspond to the connectivity and type of each element.

Note 2: For flexible beam elements (type 6, 7, or 14), AERO-S supports a run-time generation of local frames that is activated either when the target flexible beam element is identified under the EFRAMES command and a third node is specified to generate its local frame, or when a third node is found in the definition of a flexible beam element within this command for the same purpose. The only requirement for the third node is that it does not be colinear with the other two nodes defining the flexible beam element and its local

\text{[math]}

-axis. Under the EFRAMES command, the third node defines the local

\text{[math]}

plane. Under this command, it defines the local

\text{[math]}

plane. Using the third node option under this command for a flexible beam element relieves the user from specifying a local frame for this element under the EFRAMES command. An example illustrating the third node option in the TOPOLOGY command can be found in APPENDIX 3.

Note 3: In a linear dynamic analysis, the freeplay-induced forces and moments are interpreted as configuration-dependent and automatically treated as piecewise constant (see PIECEWISE in STATICS).

Note 4: Currently, only the SPOOLES and MUMPS sparse direct solvers and the FETI-DP(H) solvers can handle rigid elements.

Note 5: Thermal loads (see TEMPERATURES) are currently implemented only for the truss, Euler beam, Timoshenko beam, 4-noded plane stress/plane strain, 4-noded as well as 10-noded tetrahedron, 8-noded as well as 20-noded and 32-noded brick, 6-noded as well as 15-noded and 26-noded penta elements, and all 3- and 4-noded shell elements.

Note 6: The heat radiation elements 56, 57, and 58 are primarily nonlinear thermal elements. Hence, the presence of any of these elements in a thermal model usually implies a nonlinear analysis and therefore requires specifying the NONLINEAR command in the ASCII Input Command Data file. However, in the presence of such elements in the thermal model but absence of the NONLINEAR command in the aforementioned input file, AERO-S performs a linearized thermal (perturbation) analysis where the conductivity matrix is adjusted by the Jacobian of the finite element treatment of the radiation boundary condition evaluated at an equilibrium temperature field that must be specified in this case using the ETEMP command. In principle, the equilibrium temperature field is the solution of a related nonlinear steady thermal analysis problem with radiation boundary conditions; therefore, it captures the effect of the ambient (reference) temperature of the enclosure receiving the radiation which is specified in the parameter Tr of the MATERIAL command. However, the linearized thermal (perturbation) problem solved by AERO-S in the presence of a heat radiation element in the thermal model but absence of the NONLINEAR command is not affected by this reference temperature.

Note 7: For DEM (Discontinuous Enrichment Method) and DGM (Discontinuous Galerkin Method) elements, Q, T, and H designate a quadrilateral, a triangle in two dimensions and a tetrahedron in three dimensions, and an hexahedron, respectively. In the notation Q-X-Y, T-X-Y, and H-X-Y, X denotes the number of enrichment functions in the element and Y denotes the number of Lagrange multiplier degrees of freedom per edge or face of the element. In the notation X1xX2-Y for elastodynamics, X1 denotes the number of directions of the plane wave enrichment functions, X2 denotes the number of enrichment functions per wave direction (X2 = 2 (one pressure and one shear wave) in two dimensions and X2 = 3 (one pressure and two shear waves) in three dimensions), and Y denotes the number of Lagrange multiplier degrees of freedom per edge of face of the element. The connectivity (geometry and local node numbering) of all Q, T, and H DEM and DGM elements is that of Q, T, and H higher-order isoparametric elements, respectively. Hence, for each DEM element, the degree of the polynomial field can be deduced from the number of nodes of that element.

Note 8: The fluid elements (type 301, 302, 311, 312, 321, and 331) are active only in the following cases: (1) a mass computation using the MASS command, (2) a sloshing eigen computation using the SLOSH and related commands, (3) a hydroelastic eigenvalue computation using the EIGEN, HEFRS, HEFSB and related commands.

`ELEMENT#`	Element identification number whose type and connectivity are to be specified (integer).
`ELEMENT_TYPE:`	M=Mechanic - A=Acoustic (Helmholtz or Time-Domain) - H=Heat- C=Coupled Thermoelastic - F=Fluid
1	M: 3d truss (bar) with 3 dof/node (Figure 1).
2	M: 2d 4-node plane stress/plane strain quadrilateral with 2 dof/node (Figure 2). Currently, a consistent mass matrix is not available for this element.
3	H: 3d 4-node quadrilateral with 1 dof/node (Figure 2).
4	M: 2d 3-node triangle with 2 dof/node (Figure 3). Currently, a consistent mass matrix is not available for this element.
6	M: 3d 2-node Bernoulli beam with 6 dof/node (Figure 1).
7	M: 3d 2-node Timoshenko beam with 6 dof/node (Figure 1). Currently, a consistent mass matrix is not available for this element.
8	M: 3d 3-node triangular AQR shell with 6 dof/node (Figure 3). Currently, a consistent mass matrix is not available for this element.
88	M: 3d 4-node shell with 6 dof/node that splits into 2 triangular shells of type 8 (Figure 2). Currently, a consistent mass matrix is not available for this element.
9	H: 3d 2-node line with 1 dof/node (Figure 1).
10	H: 2d 4-node quadrilateral with 1 dof/node (Figure 2).
11	M: 3d 1-node (lumped) torsional spring with 3 dof/node for linear analysis (Figure 4).
12	M: 3d 1-node (lumped) translational spring with 3 dof/node for linear analysis.
15	M: 3d 3-node triangular AQR shell with 6 dof/node and composite as well as nonlinear material capability (Figure 3). Note that only a lumped mass matrix is available for this element. Hence, this element effectively replaces the elements 8 and 20 even though both are still supported.
1515	M: 3d 4-node quadrilateral AQR shell with 6 dof/node and composite as well as nonlinear material capability (Figure 2). Note that only a lumped mass matrix is available for this element. Hence, this element effectively replaces the elements 88 and 2020 even though both are still supported.
16	M: 3d Belytschko-Tsay 4-node quadrilateral or degenerated quadrilateral (Figure 2), or 3-node triangular shell with 6 dof/node and 1-point quadrature rule (Figure 3), and nonlinear material capability. Currently, this element is available only for explicit dynamic analyses.
17	M: 3d 8-node brick with 3 dof/node (Figure 5).
18	M: 3d 4-node shear panel with 3 dof/node (Figure 2). Currently, a consistent mass matrix is not available for this element.
19	M: 3d 3-node triangular membrane with 6 dof/node (Figure 3; only in-plane and drilling stiffnesses). Currently, a consistent mass matrix is not available for this element.
20	M: 3d 3-node triangular composite or orthotropic shell with 6 dof/node (Figure 3). Currently, a consistent mass matrix is not available for this element.
2020	M: 3d 4-node composite or orthotropic shell with 6 dof/node (Figure 2). Currently, a consistent mass matrix is not available for this element.
21	M: 3d translational spring-link with 3 dof/node for linear analysis (Figure 1).
22	M: 3d torsional spring-link with 3 dof/node for linear analysis (Figure 1).
23	M: 3d 4-node tetrahedron with 3 dof/node (Figure 6) and nonlinear material capability.
24	M: 3d 6-node pentahedron with 3 dof/node (Figure 7) and nonlinear material capability.
25	M: 3d 10-node tetrahedron with 3 dof/node (Figure 8) and nonlinear material capability.
26	M: 3d 2-node damper element with 3 dof/node (Figure 1).
27	M: 3d 2-node or curved 3-node cable with 3 dof/node (Figure 26). In general, this element is designed for nonlinear analysis (NONLINEAR), in which case its constitutive law is $\text{[math]}$ $\text{[math]}$ However, this element can also be used in a linear analysis, in which case its constitutive law becomes $\text{[math]}$ Hence, for a linear analysis, this element reduces to a two-node (or curved three-node), bar-like element.
30	A: 2d 4-node quadrilateral with 1 dof/node (Figure 2).
31	A: 2d 4-node quadrilateral GLS element with 1 dof/node (Figure 2).
32*	A: 2d 8-node quadrilateral with 1 dof/node (Figure 9).
33*	A: 2d 4-node quadrilateral bubble element with 1 dof/node (Figure 2).
34*	A: 2d 4-node quadrilateral two-level bubble element with 1 dof/node (Figure 2).
35	A: 2d 3-node triangle with 1 dof/node (Figure 3).
36	A: 2d 3-node triangular GLS element with 1 dof/node (Figure 3).
38*	A: 2d 6-node triangle with 1 dof/node (Figure 10).
40	A: 3d 4-node tetrahedron with 1 dof/node (Figure 6).
41	A: 3d 4-node tetrahedral GLS element with 1 dof/node (Figure 6).
42	A: 3d 10-node tetrahedron with 1 dof/node (Figure 8).
44	A: 3d 8-node brick GLS element with 1 dof/node (Figure 5).
45*	A: 3d 8-node brick with 1 dof/node (Figure 5).
46	H: 3d 3-node triangular thermal (heat conduction) element (Figure 3).
4646	H: 3d 4-node quadrilateral thermal (heat conduction) element that splits into 2 triangular elements of type 46 (Figure 2).
47	H: 3d 2-node line with 1 dof/node for boundary convection (Figure 1).
48	H: 3d 4-node quadrilateral with 1 dof/node for boundary convection (Figure 2).
49	H: 3d 3-node triangle with 1 dof/node for boundary convection (Figure 3).
50	H: 3d 4-node, 10-node, 20-node, or 35-node tetrahedron with 1 dof/node. These "p-type" elements use a special local node-numbering for connectivity which goes line-by-line (Figure 11).
51	H: 3d 8-node brick with 1 dof/node (Figure 5).
52*	M: 3d 6-node triangular shell (Figure 10).
53	H: 2d 3-node triangular thermal (heat conduction) element (Figure 3).
56	H: 3d 2-node heat radiation element (Figure 1).
57	H: 3d 3-node triangular heat radiation element (Figure 3).
58	H: 3d 4-node quadrilateral heat radiation element (Figure 2).
59	A: 2d 6-node axisymmetric triangular element with 1 dof/node (Figure 10).
60	A: 2d 4-node axisymmetric quadrilateral with 1 dof/node (Figure 2).
61	A: 2d 3-node axisymmetric triangle with 1 dof/node (Figure 3).
62	A: 2d 8-node axisymmetric quadrilateral with 1 dof/node (Figure 9).
65	M: 3d 2-node rigid truss (bar) (Figure 1); enforces constant length of the element.
66	M: 3d 2-node rigid beam of non zero length (Figure 1); enforces constant length of the element, equal rotations of the cross sections at its two nodes, and other constraints between its rotational and translational dofs to simulate a genuinely rigid beam.
67	M: 3d 2-node rigid link (translational and rotational, Figure 1); for each specified dof at one node, it enforces equality to the corresponding dof at the other node. Therefore, this element enforces constant length like element type 66; however, it also enforces additional constraints and therefore is different from element type 66.
68	M: 3d 2-node rigid translational link (Figure 1); for each specified translational dof at one node, it enforces equality to the corresponding dof at the other node. Therefore, this element enforces constant length like element type 65; however, it also enforces additional constraints and therefore is different from element type 65.
69	M: 3d 2-node rigid rotation link (Figure 1); for each rotational dof at one node, enforces equality to the corresponding dof at the other node.
70	M: 3d 8-node rigid brick with 3 dof/node (Figure 5); enforces constant distance between each pair of its nodes (special case of element type 71).
71	M: 3d rigid line, plane, or solid element with 3 dof/node and anywhere from 3 to 32 nodes per element (Figure 12); enforces constant distance between each pair of its nodes.
72	M: 3d 20-node brick (Figure 12) with 3 dof/node and nonlinear material capability.
73	M: 3d 3-node rigid shell (Figure 3); equivalent to two rigid beam, each defined by an edge of the element (special case of type 74).
74	M: 3d rigid line, plane, or solid element with 6 dof/node and anywhere from 3 to 32 nodes per element (Figure 13); enforces constant distance between each pair of its nodes, equal values of the rotational dofs at all nodes, and other constraints to simulate a genuinely rigid element.
76	M: 3d 4-node rigid shell (Figure 2); equivalent to three rigid beam, each defined by an edge of the element (special case of type 74).
77	M: 3d 1-node point-to-point constraint element with 3 dof/node.
78	M: 3d 1-node point-to-line constraint element with 3 dof/node.
79	M: 3d 1-node point-to-plane constraint element with 3 dof/node.
81	H: 2d 4-node contact resistance thermal element with 1 dof/node that can be inserted between two thermal elements of type 10 (Figure 2).
82	H: 3d 8-node contact resistance thermal element with 1 dof/node that can be inserted between two thermal elements of type 51 (Figure 5).
83	H: 3d 6-node contact resistance thermal element with 1 dof/node that can be inserted between two thermal elements of type 50 with 4 nodes each (Figure 7).
84	H: 2d 3-node triangular bulk fluid (thermal) element with 1 dof/node. The first node appearing in the connectivity list of this element must be inside the bulk fluid, and the other two nodes must be located at the interface boundary between the bulk fluid and the surrounding material. The temperature at the first node is by definition the average temperature of the bulk fluid (Figure 14).
85	H: 3d 4-node tetrahedron bulk fluid (thermal) element with 1 dof/node. The first node appearing in the connectivity list of this element must be inside the bulk fluid, and the other three nodes must be located at the interface boundary between the bulk fluid and the surrounding material. The temperature at the first node is by definition the average temperature of the bulk fluid (Figure 15).
86	H: 3d 5-node pyramidal bulk fluid (thermal) element with 1 dof/node. The first node appearing in the connectivity list of this element must be inside the bulk fluid, and the other four nodes must be located at the interface boundary between the bulk fluid and the surrounding material. The temperature at the first node is by definition the average temperature of the bulk fluid (Figure 16).
87	M: 3d 4-node quadrilateral membrane with 6 dof/node (Figure 2; only in-plane and drilling stiffnesses). Currently, a consistent mass matrix is not available for this element.
90	A: 3d 6-node wedge with 1 dof/node (Figure 7).
91	M: 3d 32-node serendipity brick with 3 dof/node (Figure 13) and nonlinear material capability.
92	M: 3d 26-node serendipity wedge with 3 dof/node (Figure 17) and nonlinear material capability.
93	A: 3d 32-node serendipity brick with 1 dof/node (Figure 13).
94	A: 3d 26-node serendipity wedge with 1 dof/node (Figure 17).
95	A: 3d 8-node, 27-node, 64-node, or 125-node hexahedron with 1 dof/node. These "p-type" elements use a special local node-numbering for connectivity which goes line-by-line (Figure 18). They also support the PML (Perfectly Matching Layer) computational technology.
96	A: 3d 4-node, 10-node, 20-node, or 35-node tetrahedron with 1 dof/node (Figure 11). These "p-type" elements use a special local node-numbering for connectivity which goes line-by-line They also support the PML (Perfectly Matching Layer) computational technology.
97	M: 3d 15-node wedge with 3 dof/node and nonlinear material capability (Figure 31).
98	A: 2d 4-node, 9-node, 16-node, or 25-node quadrilateral with 1 dof/node. These "p-type" elements use a special local node-numbering for connectivity which goes line-by-line (Figure 19). They also support the PML (Perfectly Matching Layer) computational technology.
99	A: 2d 3-node, 6-node, or 10-node triangle with 1 dof/node. These "p-type" elements use a special local node-numbering for connectivity which goes line-by-line (Figure 20). They also support the PML (Perfectly Matching Layer) computational technology.
100	M: 2d 4-node, 9-node, 16-node, or 25-node quadrilateral with 3 dof/node. These "p-type" elements use a special local node-numbering for connectivity which goes line-by-line (Figure 19).
101	M: 2d 3-node, 6-node, or 10-node triangular element with 3 dof/node. These "p-type" elements use a special local node-numbering for connectivity which goes line-by-line (Figure 20).
102	M: 3d 8-node, 27-node, 64-node, or 125-node hexahedron with 3 dof/node. These "p-type" elements use a special local node-numbering for connectivity which goes line-by-line (Figure 18).
103	M: 3d 4-node, 10-node, 20-node, or 35-node tetrahedron with 3 dof/node. These "p-type" elements use a special local node-numbering for connectivity which goes line-by-line (Figure 11).
105	A: 3d 8-node, 27-node, 64-node, or 125-node spectral hexahedron with 1 dof/node. These spectral elements use a special local node-numbering for connectivity which goes line-by-line (Figure 18).
106	M: 3d 2-node rigid beam of arbitrary length, including zero length (Figure 1); enforces constant length of the element, equal rotations of the cross sections at its two nodes, and other constraints between its rotational and translational dofs to simulate a genuinely rigid beam.
108	A: 2d 4-node, 9-node, 16-node, or 25-node spectral quadrilateral element with 1 dof/node. These spectral elements use a special local node-numbering for connectivity which goes line-by-line (Figure 19).
109	H: 3d 8-node, 27-node, 64-node, or 125-node hexahedron with 1 dof/node. These "p-type" elements use a special local node-numbering for connectivity which goes line-by-line (Figure 18).
111	M: 3d fabric truss with 3 dof/node (Figure 1). Currently, a consistent mass matrix is not available for this element.
118	M: 3d 2-node planar joint with 6 dof/node (Figure 27). This element has a co-rotating reference frame attached to each of its two nodes. Both frames have the same orientation in the undeformed configuration and therefore can be viewed, as far as input is concerned, as the same frame. The orientation of this frame in the undeformed configuration must be specified under EFRAMES, using the same format as for a beam. In this format, the $\text{[math]}$ and $\text{[math]}$ axes of the local frame correspond to the $\text{[math]}$ and $\text{[math]}$ axes of the co-rotating reference frame at node 1 in its undeformed configuration. These axes should be defined so that the position of node 2 is constrained to lie in the plane they define.
119	M: 3d 2-node welded joint with 6 dof/node (Figure 30). This element constrains the relative translations and rotations between two nodes.
120	M: 3d 2-node spherical joint with 3 dof/node. This element constrains the relative translations between two nodes (Figure 21).
121	M: 3d 2-node translational joint with 3 rotational dof/node (Figure 28). This element constrains the relative rotations between two nodes.
122	M: 3d 2-node universal joint with 6 dof/node (Figure 22). This element has a co-rotating reference frame attached to each of its two nodes. Both frames have the same orientation in the undeformed configuration and therefore can be viewed, as far as input is concerned, as the same frame. The orientation of this frame in the undeformed configuration must be specified under EFRAMES, using the same format as for a beam. In this format, the $\text{[math]}$ axis of the local frame corresponds to the orientation in the undeformed configuration of the $\text{[math]}$ axis of the co-rotating reference frame at node 2, and the $\text{[math]}$ axis of the local frame corresponds to the orientation in the undeformed configuration of the $\text{[math]}$ axis of the co-rotating reference frame at node 1. These two axes should be defined so that they remain orthogonal during the deformations.
123	M: 3d 2-node revolute joint with 6 dof/node (Figure 23). This element has a co-rotating reference frame attached to each of its two nodes. Both frames have the same orientation in the undeformed configuration and therefore can be viewed, as far as input is concerned, as the same frame. The orientation of this frame in the undeformed configuration must be specified under EFRAMES, using the same format as for a beam. In this format, the $\text{[math]}$ axis of the local frame corresponds to the orientation in the undeformed configuration of the axis of free relative rotation.
124	M: 3d 2-node cylindrical joint with 6 dof/node (Figure 24). This element has a co-rotating reference frame attached to each of its two nodes. Both frames have the same orientation in the undeformed configuration and therefore can be viewed, as far as input is concerned, as the same frame. The orientation of this frame in the undeformed configuration must be specified under EFRAMES, using the same format as for a beam. In this format, the $\text{[math]}$ axis of the local frame corresponds to the orientation in the undeformed configuration of the axis of free relative displacement and rotation.
125	M: 3d 2-node prismatic joint with 6 dof/node (Figure 25). This element has a co-rotating reference frame attached to each of its two nodes. Both frames have the same orientation in the undeformed configuration and therefore can be viewed, as far as input is concerned, as the same frame. The orientation of this frame in the undeformed configuration must be specified under EFRAMES, using the same format as for a beam. In this format, the $\text{[math]}$ axis of the local frame defines the orientation in the undeformed configuration of the axis of free relative translation.
126	M: 3d 2-node revolute joint-with-driver and 6 dof/node (Figure 23) and a relative rotation (between node 2 and node 1, defined as rotation of node 2 - rotation of node 1) around the joint axis of rotation that can be prescribed using a time-dependent law specified in MATERIAL (for static analysis, the relative rotation is set to the initial value of the chosen law). This element has a co-rotating reference frame attached to each of its two nodes. Both frames have the same orientation in the undeformed configuration and therefore can be viewed, as far as input is concerned, as the same frame. The orientation of this frame in the undeformed configuration must be specified under EFRAMES, using the same format as for a beam. In this format, the $\text{[math]}$ axis of the local frame corresponds to the orientation in the undeformed configuration of the axis of forced relative rotation.
127	M: 3d 2-node pin-in-slot joint with 6 dof/node (Figure 29). This element has a co-rotating reference frame attached to each of its two nodes. Both frames have the same orientation in the undeformed configuration and therefore can be viewed, as far as input is concerned, as the same frame. The orientation of this frame in the undeformed configuration must be specified under EFRAMES, using the same format as for a beam. In this format, the $\text{[math]}$ -axis of the local frame corresponds to the orientation in the undeformed configuration of the axis of free relative translation, and its $\text{[math]}$ -axis corresponds to the orientation in the undeformed configuration of the axis of free relative rotation.
128	M: 3d 4-node plane stress quadrilateral membrane with 3 dof/node (Figure 2).
129	M: 3d 3-node plane stress triangular membrane with 3 dof/node (Figure 3).
131	M: 3d 1-node discrete mass and inertia element with 6 dof/node. It accepts an offset as an attribute (see MATERIAL) and therefore offers a functionality not provided by the DIMASS command.
132	M: 3d 2-node massless rigid beam of non zero length (Figure 1); enforces constant length of the element, equal rotations of the cross sections at its two nodes, and other constraints between its rotational and translational dofs to simulate a genuinely rigid beam. Because this element is designed to be always massless, it is computationally more efficient than its counterpart, element type 66, equipped with a zero density.
133	M: 3d 2-node massless rigid beam (Figure 1) of arbitrary length, including zero length; enforces constant length of the element, equal rotations of the cross sections at its two nodes, and other constraints between its rotational and translational dofs to simulate a genuinely rigid beam. Because this element is designed to be always massless, it is computationally more efficient than its counterpart, element type 106, equipped with a zero density.
134	M: 3d 2-node prismatic joint-with-driver and 6 dof/node (Figure 25) and a relative displacement (between node 2 and node 1) along the joint axis of displacement that is prescribed using a time-dependent law specified in MATERIAL (for static analysis, the relative displacement is set to the initial value of the chosen law). This element has a co-rotating reference frame attached to each of its two nodes. Both frames have the same orientation in the undeformed configuration and therefore can be viewed as far as input is concerned as the same frame. The orientation of this frame in the undeformed configuration must be specified under EFRAMES, using the same format as for a beam. Its $\text{[math]}$ axis defines the orientation in the undeformed configuration of the axis of prescribed relative translation.
150	M: 3d 4-node rigid tetrahedron with 3 dof/node (Figure 6).
151	M: 3d 6-node rigid pentahedron with 3 dof/node (Figure 7).
177	M: 3d 2-node point-to-moving-point constraint element with 3 dof/node.
178	M: 3d 3-node point-to-moving-line constraint element with 3 dof/node.
179	M: 3d 4-node point-to-moving-plane constraint element with 3 dof/node.
180	M: 3d 8-node Q1-P0 hexahedron with 3 dof/node (Figure 5) with nonlinear material capability. This element, which uses a 3-field mixed formulation, is suitable for modeling incompressible and nearly incompressible materials with large displacements.
181	M: 3d 20-node Q2-P0 hexahedron with 3 dof/node (Figure 5) with nonlinear material capability. This element, which uses a 3-field mixed formulation, is suitable for modeling incompressible and nearly incompressible materials with large displacements.
182	M: 3d 20-node Q2-P1 hexahedron with 3 dof/node (Figure 5) with nonlinear material capability. This element, which uses a 3-field mixed formulation, is suitable for modeling incompressible and nearly incompressible materials with large displacements.
183	M: 3d 4-node P1-P0 tetrahedron with 3 dof/node (Figure 6) with nonlinear material capability. This element, which uses a 3-field mixed formulation, is suitable for modeling incompressible and nearly incompressible materials with large displacements.
200	M: 3d 2-node uniaxial translational spring with 3 dof/node for linear or nonlinear analyses. The initial orientation of the spring axis is aligned with that of the element defined by its two nodes: hence, this element cannot have a zero length.
201	M: 3d 2-node uniaxial translational spring with 6 dof/node for linear or nonlinear analyses. The initial orientation of the spring axis is the local $\text{[math]}$ -axis of the element frame. It must be specified under EFRAMES, using the same format as for a beam. This translational spring can connect with any other element with 6 dof/node without raising any mechanism issue. Furthermore, it distinguishes itself from element type 200 in that it can have a zero length.
202	M: 3d 2-node uniaxial torsional spring with 3 rotational dof/node for linear or nonlinear analyses. The initial orientation of the spring axis is the local $\text{[math]}$ -axis of the element frame. It must be specified under EFRAMES, using the same format as for a beam.
203	M: 3d 2-node uniaxial tension-only translational spring with 3 dof/node and an optional freeplay model, for linear or nonlinear analyses. The parameters of the optional freeplay model can be specified in MATERIAL. The initial orientation of the spring axis is aligned with that of the element defined by its two nodes: hence, this element cannot have a zero length.
204	M: 3d 2-node uniaxial tension-only or compression-only translational spring with 6 dof/node and an optional freeplay model, for linear or nonlinear analyses. The parameters of the optional freeplay model can be specified in MATERIAL. The initial orientation of the spring axis is the local $\text{[math]}$ -axis of the element frame. It must be specified under EFRAMES, using the same format as for a beam. The element acts as a tension-only translational spring if the dot product of the local $\text{[math]}$ -axis specified under EFRAMES and the axis implied by the ordering of the two nodes defining this element is positive. Otherwise, it acts as a compression-only translational spring.
205	M: 3d 2-node uniaxial tension-only or compression-only torsional spring with 3 rotational dof/node and an optional freeplay model, for linear or nonlinear analyses. The parameters of the optional freeplay model can be specified in MATERIAL. The initial orientation of the spring axis is the local $\text{[math]}$ -axis of the element frame. It must be specified under EFRAMES, using the same format as for a beam. The element acts as a tension-only rotational spring if the dot product of the local $\text{[math]}$ -axis specified under EFRAMES and the axis implied by the ordering of the two nodes defining this element is positive. Otherwise, it acts as a compression-only rotational spring.
220	M: 3d 2-node spherical joint spring combination with 6 dof/node (Figure 21). This element is equivalent to one spherical joint (type 120) and three embedded torsional springs (type 202). The initial orientation of the first embedded spring's axis is the local $\text{[math]}$ -axis of the element frame. The initial orientation of the second embedded spring's axis is the local $\text{[math]}$ -axis of the element frame. The initial orientation of the third embedded spring's axis is the local $\text{[math]}$ -axis of the element frame. This information must be specified under EFRAMES, using the same format as for a beam element.
221	M: 3d 2-node translational joint spring combination element with 6 dof/node (Figure 28). This element is equivalent to one translational joint (type 121) and three embedded translational springs (type 201). The initial orientation of the first embedded spring's axis is the local $\text{[math]}$ -axis of the element frame. The initial orientation of the second embedded spring's axis is the local $\text{[math]}$ -axis of the element frame. The initial orientation of the third embedded spring's axis is the local $\text{[math]}$ -axis of the element frame. This information must be specified under EFRAMES, using the same format as for a beam.
222	M: 3d 2-node universal joint spring combination element with 6 dof/node (Figure 22). This element is equivalent to one universal joint (type 122) and two embedded torsional spring elements (type 202). The initial orientation of the first embedded spring's axis is the local $\text{[math]}$ -axis of the element frame. The initial orientation of the second embedded spring's axis is the local $\text{[math]}$ -axis of the element frame. This information must be specified under EFRAMES, using the same format as for a beam.
223	M: 3d 2-node revolute joint spring combination element with 6 dof/node (Figure 23). This element is equivalent to one revolute joint (type 123) and one embedded torsional spring element (type 202). The initial orientation of the embedded spring's axis is the local $\text{[math]}$ -axis of the element frame. This information must be specified under EFRAMES, using the same format as for a beam.
224	M: 3d 2-node cylindrical joint spring combination element with 6 dof/node (Figure 24). This element is equivalent to one cylindrical joint (type 124), one embedded translational spring (type 201), and one embedded torsional spring (type 202). The initial orientation of the first (translational) embedded spring's axis is the local $\text{[math]}$ -axis of the element frame. The initial orientation of the second (torsional) embedded spring's axis is also the local $\text{[math]}$ -axis of the element frame. This information must be specified under EFRAMES, using the same format as for a beam element.
225	M: 3d 2-node prismatic joint spring combination element with 6 dof/node (Figure 25). This element is is equivalent to one prismatic joint (type 125) and one embedded translational spring (type 201). The initial orientation of the embedded spring's axis is the local $\text{[math]}$ -axis of the element frame. This information must be specified under EFRAMES, using the same format as for a beam.
226	M: 3d 2-node revolute joint-with-actuator with 6 dof/node (Figure 23). This element is equivalent to one revolute joint spring combination element (type 223) and two equal and opposite embedded follower (see FORCES) moments applied to the two nodes of the element. The magnitude of these moments is prescribed using a time-dependent law specified in MATERIAL (for static analysis, the magnitude of the moments is set to the initial value of the chosen law). This element has a co-rotating reference frame attached to each of its two nodes. Both frames have the same orientation in the undeformed configuration and therefore can be viewed as far as input is concerned as the same frame. The orientation of this frame in the undeformed configuration must be specified under EFRAMES, using the same format as for a beam. Its $\text{[math]}$ -axis defines the orientation in the undeformed configuration of the axis about which the embedded moment applied to the second node of the element acts, and also the initial orientation of the embedded spring's axis.
227	M: 3d 2-node pin-in-slot joint spring combination element with 6 dof/node (Figure 29). This element is is equivalent to one pin-in-slot joint (type 127), one embedded translational spring element (type 201), and one embedded torsional spring (type 202). The initial orientation of the first embedded (translational) spring's axis is the local $\text{[math]}$ -axis of the element frame. The initial orientation of the second embedded (torsional) spring's axis is the local $\text{[math]}$ -axis of the element frame. This information must be specified under EFRAMES, using the same format as for a beam.
234	M: 3d 2-node prismatic joint-with-actuator element with 6 dof/node (Figure 25). This element is equivalent to one prismatic joint spring combination element (type 225) and two equal and opposite embedded follower (see FORCES) forces applied to the two nodes of the element. The magnitude of these forces is prescribed using a time-dependent law specified in MATERIAL (for static analysis, the magnitude of the forces is set to the initial value of the chosen law). This element has a co-rotating reference frame attached to each of its two nodes. Both frames have the same orientation in the undeformed configuration and therefore can be viewed as far as input is concerned as the same frame. The orientation of this frame in the undeformed configuration must be specified under EFRAMES, using the same format as for a beam. Its $\text{[math]}$ -axis defines the orientation in the undeformed configuration of the direction in which the embedded force applied to the second node of the element acts, and also the initial orientation of the embedded spring's axis.
280	M: 3d 8-node Q1-P0 incompressible hexahedron with 3 dof/node (Figure 5) with nonlinear material capability. This element, which uses a 4-field mixed formulation, is suitable for modeling incompressible and nearly incompressible materials with large displacements.
301	F: 2d 4-node quadrilateral with 1 dof/node (Figure 2) for modeling an incompressible, inviscid fluid — in the presence of gravity — using a displacement-potential formulation, and computing sloshing modes.
302	F: 2d 2-node element with 1 dof/node for modeling the free-surface of an incompressible, inviscid fluid using a displacement-potential formulation (Figure 1). For two-dimensional sloshing or hydroelastic mode computations, it is to be used with element type 301.
311	F: 3d 4-node tetrahedron with 1 dof/node (Figure 6) for modeling an incompressible, inviscid fluid — in the presence of gravity — using a displacement-potential formulation, and computing sloshing modes.
312	F: 3d 3-node triangle with 1 dof/node for modeling the free-surface of an incompressible, inviscid fluid using a displacement-potential formulation (Figure 3). For three-dimensional sloshing or hydroelastic mode computations, it is to be used with element type 311.
321	F: 2d 4-node quadrilateral with 1 dof/node (Figure 2) for modeling an incompressible, weightless fluid using a displacement-potential formulation, and computing hydroelastic vibration modes.
323	M: This element is a variant of element type 223 that is equipped with a freeplay model (Figure 23). Hence, it is a 3d 2-node revolute joint spring combination element with a nonlinear (or piecewise linear, see `PIECEWISE` in STATICS) torsional spring and 6 dof/node. The parameters of its freeplay model can be specified in MATERIAL. The initial orientation of the embedded spring's axis is the local $\text{[math]}$ -axis of the element frame. This information must be specified under EFRAMES, using the same format as for a beam.
325	M: This element is a variant of element type 225 that is equipped with a freeplay model (Figure 25). Hence, it is a 3d 2-node prismatic joint spring combination element with a nonlinear (or piecewise linear, see `PIECEWISE` in STATICS) translational spring and 6 dof/node. The parameters of its freeplay model can be specified in MATERIAL. The initial orientation of the embedded spring's axis is the local $\text{[math]}$ -axis of the element frame. This information must be specified under EFRAMES, using the same format as for a beam.
331	F: 3d 4-node tetrahedron with 1 dof/node (Figure 6) for modeling an incompressible, weightless fluid using a displacement-potential formulation, and computing hydroelastic vibration modes.
333	H: 3d 2-node line with 1 dof/node for ablation associated with the $\text{[math]}$ ablation model (Figure 1).
334	H: 3d 3-node triangle 1 dof/node for ablation associated with the $\text{[math]}$ ablation model (Figure 3).
335	H: 3d 4-node quadrilateral with 1 dof/node for ablation associated with the $\text{[math]}$ ablation model (Figure 2).
1100	A: 2d 4-node Helmholtz DGM element Q-4-1 (Figure 19 with p = 2).
1101	A: 2d 4-node Helmholtz DGM element Q-8-2 (Figure 19 with p = 2).
1102	A: 2d 4-node Helmholtz DGM element Q-16-4 (Figure 19 with p = 2).
1103	A: 2d 4-node Helmholtz DGM element Q-32-8 (Figure 19 with p = 2).
1110	A: 2d 3-node Helmholtz DGM element T-4-1 (Figure 20 with p = 2, or Figure 3).
1111	A: 2d 3-node Helmholtz DGM element T-8-2 (Figure 20 with p = 2, or Figure 3).
1120	A: 2d 4-node Helmholtz DEM element Q-4-1 (Figure 19 with p = 2).
1121	A: 2d 4-node Helmholtz DEM element Q-8-2 (Figure 19 with p = 2).
1122	A: 2d 4-node Helmholtz DEM element Q-16-4 (Figure 19 with p = 2).
1123	A: 2d 4-node Helmholtz DEM element Q-32-8 (Figure 19 with p = 2).
1130	A: 2d 3-node Helmholtz DEM element T-4-1 (Figure 20 with p = 2, or Figure 3).
1131	A: 2d 3-node Helmholtz DEM element T-8-2 (Figure 20 with p = 2, or Figure 3).
1150	A: 3d 8-node Helmholtz DGM element H-6-1 (Figure 18 with p = 2).
1151	A: 3d 8-node Helmholtz DGM element H-26-4 (Figure 18 with p = 2).
1152	A: 3d 8-node Helmholtz DGM element H-56-8 (Figure 18 with p = 2).
1153	A: 3d 8-node Helmholtz DGM element H-98-12 (Figure 18 with p = 2).
1160	A: 3d 4-node Helmholtz DGM element T-6-1 (Figure 11 with p = 2, or Figure 6).
1161	A: 3d 4-node Helmholtz DGM element T-26-4 (Figure 11 with p = 2, or Figure 6).
1162	A: 3d 4-node Helmholtz DGM element T-56-8 (Figure 11 with p = 2, or Figure 6).
1170	A: 3d 8-node Helmholtz DEM element H-6-1 (Figure 18 with p = 2).
1171	A: 3d 8-node Helmholtz DEM element H-26-4 (Figure 18 with p = 2).
1172	A: 3d 8-node Helmholtz DEM element H-56-8 (Figure 18 with p = 2).
1173	A: 3d 8-node Helmholtz DEM element H-98-12 (Figure 18 with p = 2).
1200	M: 2d 4-node Elastodynamic DGM element Q-4x2-2 (Figure 19 with p = 2).
1201	M: 2d 4-node Elastodynamic DGM element Q-16x2-8 (Figure 19 with p = 2).
1220	M: 2d 4-node Elastodynamic DEM element Q-4x2-2 (Figure 19 with p = 2).
1250	M: 3d 8-node Elastodynamic DGM element H-6x3-3 (Figure 18 with p = 2).
1251	M: 3d 8-node Elastodynamic DGM element H-26x3-15 (Figure 18 with p = 2).
1252	M: 3d 8-node Elastodynamic DGM element H-50x3-28 (Figure 18 with p = 2).
`CONNECTIVITY_NODES`	These should be listed in a stacked fashion on a single line. The various orderings are graphically depicted in the figures below.

Figure 1: local node numbering for element types 1, 6, 7, 9, 21, 22, 26, 47, 56, 65--69, 111, 302, 333

Figure 2: local node numbering for element types 2, 3, 88, 10, 1515, 16, 18, 2020, 30, 31, 33, 34, 4646, 48, 58, 76, 81, 87, 128, 301, 321, 335

Figure 3: local node numbering for element types 4, 8, 15, 16, 19, 20, 35, 36, 46, 49, 53, 57, 73, 129, 312, 334, 1110,1111,1130,1131

Figure 5: local node numbering for element types 17, 44, 45, 51, 70, 82, 180, 181, 182, 280

Figure 6: local node numbering for element types 23, 40, 41, 150, 183, 311, 331, 1160, 1161, 1162

Figure 11: local node numbering for element types 50, 96, 103, 1160, 1161, 1162

Figure 18: local node numbering for element types 95, 102, 105, 109, 1150, 1151, 1152, 1153, 1170, 1171, 1172, 1173, 1250, 1251, 1252

Figure 19: local node numbering for element types 98, 100, 108, 1100, 1101, 1102, 1103, 1120, 1121, 1122, 1123, 1200, 1201, 1220

Figure 20: local node numbering for element types 99, 101, 1110, 1111, 1130, 1131

36 ENABLING REDUCTION AND HYPER REDUCTION USING LOCAL REDUCED-ORDER BASES

The LOCROB command should be used to enable the reduction or hyper reduction of nonlinear structural dynamic computation using local Reduced-Order Bases (ROBs), following the theory described in D. Amsallem, M. Zahr and C. Farhat, "Nonlinear Model Order Reduction Based on Local Reduced-Order Bases," International Journal for Numerical Methods in Engineering, Vol. 92, pp. 891-916 (2012).

Note 2: Using a set of local ROBs instead of a single (global) ROB requires repeating in the same ASCII Input Command Data file and for each local ROB, the commands READMODE, ATTRIBUTES, the sub-command keywords PODROB and TRNSOL of the command RMSHC, and the sub-command keywords CENTROID and AUXI of this command. For example, the

\text{[math]}

-th occurrence of the command READMODE specifies the filename and size of the

\text{[math]}

-th local ROB, the

\text{[math]}

-th occurrence of the command ATTRIBUTES specifies the element weights of the reduced mesh associated with the

\text{[math]}

-th local ROB, etc.

`CENTROID`	Sub-command keyword for specifying a file containing the centroid of a snapshot cluster generated by ROBC (characters). This sub-command and its input are needed when sampling a mesh using RMSHC and local bases, or when performing a nonlinear structural dynamic computation using local ROBs without hyper reduction.
`<pathandfilename1>`	Path and name of a file containing the centroid of a snapshot cluster (characters).
`AUXI`	Sub-command keyword for specifying a file containing auxiliary quantities generated by RMSHC that are required for enabling a fast online selection of the appropriate local ROB during a nonlinear structural dynamic computation performed using a hyper reduced computational model (characters).
`<pathandfilename2>`	Path and name of a file containing the auxiliary quantities required for enabling a fast online selection of the appropriate local ROB during a computation performed using a hyper reduced nonlinear computational model (characters).

37 END

The END statement is used to indicate the end-of-file. It should always be the last statement.

38 EQUATION SOLVER CONFIGURATION

The main purpose of the SOLVERCNTL command statement is to support the solverhandle solver of the STATICS command, which is nothing but a properly configured equation solver (here, configuring an equation solver refers to setting its parameters, if it has any). Its main benefits are two-fold:

`SOLVER_ID`	Non-negative integer which identifies explicitly a configured equation solver – that is, an equation solver and a set of values for its parameters, when applicable (integer). This equation solver can be selected in STATICS as the solver `solverhandle` `SOLVER_ID`.
`METHOD`	See STATICS. Any `METHOD` that can be specified and configured in STATICS can also be specified and configured here.
`PARAMETERS`	See STATICS. Any solver parameter that can be specified in STATICS can also be specified here. However, only the parameters relevant to the equation solver specified in `METHOD` above should be specified here.

39 FIELD WEIGHTS FOR MESH DECOMPOSITION

In order to achieve load balancing when generating a mesh partition, the second-step of the non-trivial mesh partitioning strategy (see DECOMPOSE) accounts for the different weights (or weighting coefficients, see WEIGHTS) attributed to the elements of the given mesh according to their type (see TOPOLOGY). The default values attributed by AERO-S to these elements types are based on their relative computational complexity. For each different field — that is, Mechanic, Heat, Coupled Thermoelastic, Fluid, or Acoustic — these weights range between 1 and some higher value that is field-dependent. The command WEIGHTS can be used to reset, if desired, some or all of these weights to some user-specified values.

For a multidisciplinary simulation such as fluid-structure using AERO-S alone, the command FWEIGHTS can be used to attribute to each involved field (for example, Mechanic and Acoustic) a weight to allow DECOMPOSE to account additionally for the relative computational complexity of a typical element of this field to those of the typical elements of the other fields involved in the simulation. In this case, the weight

\text{[math]}

of each element type (whether its default value or that set using WEIGHTS) is automatically reset by AERO-S to the ratio

where

\text{[math]}

is the weight of the field of element type

\text{[math]}

, the scope of

\text{[math]}

is defined by all fields specified using this command.

ACOU acou_weight
FLUI flui_weight
MECH mech_weight
HEAT heat_weight

`ACOU`	Sub-command keyword for specifying a weight to the field Acoustic (see TOPOLOGY).
`acou_weight`	Weight to be attributed to the field Acoustic (real).
`FLUI`	Sub-command keyword for specifying a weight to the field Fluid (see TOPOLOGY).
`flui_weight`	Weight to be attributed to the field Fluid (real).
`MECH`	Sub-command keyword for specifying a weight to the field Mechanic (see TOPOLOGY).
`mech_weight`	Weight to be attributed to the field Mechanic (real).
`HEAT`	Sub-command keyword for specifying a weight to the field Heat (see TOPOLOGY).
`heat_weight`	Weight to be attributed to the field Heat (real).

40 FLUID/STRUCTURE INTERFACE

The FSINTERFACE command statement can be used to define the fluid/structure interface in a coupled elastoacoustic frequency response problem where: (1) the computational acoustic fluid and structural domains are discretized using either a single mesh, or two different meshes with matching or non-matching discrete interfaces, and (2) in either case, each of these two computational domains has its own representation of the fluid/structure interface in the form of a discrete surface defined using SURFACETOPO. In this scenario, the command statement FSINTERFACE is used to define more specifically the fluid/structure interface as the pairing of these two surfaces.

`SURF_PAIR_ID#`	Id number of the surface pair to be described (integer).
`FLUID_SURF`	Identification of the fluid surface (see SURFACETOPO) (integer).
`STR_SURF`	Identification of the structure surface (see SURFACETOPO) (integer).
`NORMAL_TOL`	Normal search tolerance used by ACME to identify interactions, default value is 0.1 (float) (see Figs. 1.2 and 1.3 in Section 1.3 of ACME's User Reference Manual).
`TANGENTIAL_TOL`	Tangential search tolerance used by ACME to identify interactions, default value is 0.001 (float) (see Figs. 1.2 and 1.3 in Section 1.3 of ACME's User Reference Manual).

41 FORCE TIME TABLE-MECHANICS AND ACOUSTICS

The MFTT command statement can be used to implement time-dependent tensor-product forms of the boundary conditions enforced by the commands FORCE, ATDDNB, ATDROB, and PRESSURE. Pairs of time and amplification values are input. Linear interpolation is also used for “in between” points.

When applied with the FORCE command, the result is the amplification of the force value. When applied with the ATDDNB command, the result is the amplification of the resulting distributed Neumann boundary condition. When applied with the ATDROB command, the result is the amplification of the right hand-side of the distributed Robin boundary condition.

`TABLE_ID`	Optional non-negative integer which uniquely identifies a force-time table so that it can be associated with a "load" set to define the "load" case for a dynamic analysis using the LOADCASE command. The default value is 0. Hence, the `MFTT` command can be repeated as many times as desired within the same input file using each time a different value for `TABLE_ID` and different data.
`TIME_1`	A specified time point (float).
`AMP_1`	A specified amplification value at time point `TIME_1` (float). This amplification factor is automatically set to zero for all times prior to the earliest specified time point and all times later than the latest specified time point.

42 GEOMETRIC RIGID BODY MODES

Command Statement: GRBM [ $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ ]

A singular finite element stiffness matrix arises in a linear or nonlinear static or quasistatic analysis, or in an eigen analysis, if, for example, any of the following conditions are encountered:

In some cases, a finite element matrix can have a larger number of singularities (also known as nullities) than that due to the presence of rigid body modes. This is true, for example, when the finite element model contains mechanisms. To address this issue, when the GRBM command is specified and skyline or sparse is chosen in STATICS as the equation solver, the generalized inverse of the stiffness matrix is computed in factored form using the aforementioned hybrid geometric-algebraic algorithm, and its pivots are monitored for small values using the second tolerance specified under this command. When these small values are correctly deemed to be zero pivot values, the solvers skyline and sparse capture the additional singular modes due to mechanisms or other model oddities.

Note 2: This command can be used together with the TRBM command. If both GRBM and TRBM commands are specified in the same AERO-S ASCII Input Command Data file, then:

Note 3: In some cases, the tangent stiffness matrix associated with an unrestrained or partially restrained nonlinear finite element model can have fewer rigid body modes than that which can be predicted for its linear finite element model counterpart. For this reason, the GRBM command cannot reliably assist the direct equation solvers sparse and skyline (see STATICS) in solving singular system of linearized equations associated with a nonlinear finite element analysis. In this case, the alternative TRBM command should be use for this purpose.

Note 4: If a FETI-1 or FETI-2 solver is specified under STATICS, the rigid body modes of the floating subdomains are computed using the same hybrid geometric-algebraic method and their singular matrices are factored using the same aforementioned algorithm (see the subsection of STATICS focused on FETI parameters). If a FETI-DP solver is specified under STATICS, the first tolerance specified under this command is used for detecting and computing the rigid body modes of the global stiffness matrix.

`$\text{[math]}$ $\text{[math]}$ $\text{[math]}$`	By default, the implementation of the hybrid geometric-algebraic method underlying this command computes the rotational rigid body modes by rotating the structure about the node of the mesh with the smallest ID number. However, this option can be used to specify a different point about which to rotate this model for the aforementioned purpose (for example, its center of gravity), by inputting the $\text{[math]}$ , $\text{[math]}$ and $\text{[math]}$ coordinates of this point.
`VALUE_1`	Tolerance for identifying the zero singular values of the constraint matrix analyzed by the hybrid geometric-algebraic method for finding the rigid body modes of a finite element model (real). Its default value is 1.0e-6.
`VALUE_2`	Tolerance for capturing algebraically the mechanisms and other model oddities that cause a finite element stiffness matrix to be singular, and which cannot be detected by the geometric-algebraic method alone (real). Its default value is 1.0e-16.
`VALUE_3`	Optional integer parameter for the case where the problem contains LMPCs. It can take either of the following two values: `VALUE_3` = 0. In this case, the nodes involved in each LMPC are assumed to be fully connected in the same way, for example, as nodes which are connected by beam elements. In this case: The `GRBM` command can be processed much faster than otherwise. However, it may also underestimate or overestimate the total number of rigid body modes. If it underestimates it, the direct equation solvers `sparse` and `skyline` (see STATICS) can be expected to recover nevertheless the correct total number of rigid body modes of the singular system they are applied to, because they automatically monitor the small pivots during the factorization of the governing matrix using the tolerance `VALUE_2`. On the other hand, if `GRBM` overestimates the total number of rigid body modes, these direct solvers will recover in general the wrong rigid body modes and therefore deliver an incorrect solution of the linear singular system of equations to which they are applied. For this reason, this setting of `VALUE_3` should be used with care — that is, when the user has sufficient insight in the problem to be solved to conclude that `GRBM` may at worst underestimate the correct number of rigid body modes. For example, this setting is perfectly safe for a problem where two bodies are connected with tied surfaces and therefore is recommended for this case. `VALUE_3` = 1 (default value). In this case, the above assumption about `GRBM` and LMPCs is not made. For this reason, `GRBM` is in general more reliable when `VALUE_3` is set to 1, but its processing may be computationally more intensive in this case.

43 GEOMETRIC STIFFENING DUE TO PRESTRESS

The GEPS command statement is essentially a switch that turns on the accounting of pre-stress effects in the form of a geometric stiffness matrix

\text{[math]}

. This geometric stiffness matrix is computed around a displacement field specified under the IDISP6 command which must be present in the input file. A sample input file illustrating the use of GEPS can be found in FEM.d/fem_examples/Buckle.d/

The effect of this switch on the EIGEN command statement is to replace the stiffness matrix by the tangent stiffness matrix and therefore compute the modes of the structure around the deformed position implied by the displacement field specified under the IDISP6 command.

Its effect on the DYNAMICS and STATICS commands is to replace the stiffness matrix by the tangent stiffness matrix around the displacement field specified under the IDISP6 command, including in aeroelastic applications.

44 GLOBAL SIMULATION PARAMETERS

The PARAMETERS command can be used to set some global parameters of a simulation of interest. Its input format is given below.

ACME flagACME
AGRESSIVE_TOLERANCES
ANDES_ALPHA $\text{[math]}$
ANDES_BETAB $\text{[math]}$
ANDES_BETAM $\text{[math]}$
ANDES_CLR clr
ANDES_CQR cqr
AUTO_TOL
DEFAULT_PENALTY
GLOBAL_SEARCH_CULL
MORTAR_INTEGRATION numPTS
MORTAR_SCALING scalingFCT
NLMEM_PTYPE flagPRS
NO_GHOSTING
NO_MULTIPLE_INTERACTIONS
NO_NORMAL_SMOOTHING
NO_SECONDARY
NO_WARPED_VOLUME
OLD_DYNAMIC_SEARCH
PARTITION_GAP
RESOLUTION_TYPE flagRT
SHARP_NON_SHARP_ANGLE theta
SHELL_SIMPLE_LOFTING
SKIP_PHYSICAL_FACES

`ACME`	Sub-command keyword for specifying the mode of execution of the contact search algorithm of the ACME library (characters).
`flagACME`	Specifies the mode of execution of the contact search algorithm of the ACME library (integer). Three choices are available:
`0`	Sequential (default). Currently, this is the only choice available for the mortar method.
`1`	Parallel with centralized input on the host machine.
`2`	Parallel with distributed input. This option requires a specialized decomposition where a pair of master and slave entities must be in the same subdomain.
`AGRESSIVE_TOLERANCES`	Sub-command keyword for activating an aggressive automatic determination of the contact search tolerances, when this search is performed using the ACME library (characters). In this context, the term aggressive implies that the tolerances are set less conservatively in an attempt to reduce the cost of the contact search, possibly sacrificing some robustness.
`ANDES_ALPHA`	Sub-command keyword for specifying the algorithmic parameter $\text{[math]}$ for shell elements 15 and 1515 (characters).
$\text{[math]}$	Specifies the value of the algorithmic parameter $\text{[math]}$ for shell elements 15 and 1515 (real). The default value is 1.5. For thin shells with high membrane stresses, the 0 value is recommended.
`ANDES_BETAB`	Sub-command keyword for specifying the algorithmic parameter $\text{[math]}$ for shell elements 15 and 1515 (characters).
$\text{[math]}$	Specifies the value of the algorithmic parameter $\text{[math]}$ for shell elements 15 and 1515 (real). The default value is 1.
`ANDES_BETAM`	Sub-command keyword for specifying the algorithmic parameter $\text{[math]}$ for shell elements 15 and 1515 (characters).
$\text{[math]}$	Specifies the value of the algorithmic parameter $\text{[math]}$ for shell elements 15 and 1515 (real). The default value is 0.32. For very thin shells with high membrane stresses, the 0 value is recommended.
`ANDES_CLR`	Sub-command keyword for specifying the algorithmic parameter `clr` for shell elements 15 and 1515 (characters).
`clr`	Specifies the value of the algorithmic parameter `clr` for shell elements 15 and 1515 (real). The default value is 0.
`ANDES_CQR`	Sub-command keyword for specifying the algorithmic parameter `cqr` for shell elements 15 and 1515 (characters).
`cqr`	Specifies the value of the algorithmic parameter `cqr` for shell elements 15 and 1515 (real). The default value is 1.
`AUTO_TOL`	Sub-command keyword for activating an automatic determination of the contact tolerances, when contact search is performed using the ACME library(characters).
`DEFAULT_PENALTY`	Sub-command keyword for activating the default penalty parameter when contact enforcement is performed using the ACME library (characters). In this case, the penalty parameter specified in the AERO-S Input Command Data file is ignored.
`GLOBAL_SEARCH_CULL`	Sub-command keyword for activating the following contact search option when contact search is performed using the ACME library (characters). When this option is activated, a full contact search is performed only once; subsequent searches can update existing interactions but cannot find new ones.
`MORTAR_INTEGRATION`	Sub-command keyword for specifying the number of integration points to be used for the mortar method (characters).
`numPTS`	Specifies the number of integration points to be used in the mortar method (integer). Six choices are avaliable: 1, 3, 6 (default value), 7, 12 and 16.
`MORTAR_SCALING`	Sub-command keyword for specifying a scaling of the constraint function in the mortar method (characters).
`scalingFCT`	Scaling factor to be applied to the constraint function in the mortar method (real). The default value is 1.
`NLMEM_PTYPE`	Sub-command keyword for specifying how the pressure load is to be defined for nonlinear membrane elements 128 and 129 (characters).
`flagPRS`	Specifies how the pressure load is to be defined for nonlinear membrane elements 128 and 129 (integer). Two choices are available:
`0`	In this case (which is the default case), the pressure is defined as the force per unit area $\text{[math]}$ , where $\text{[math]}$ is the area in the current/updated configuration.
`1`	In this case, the pressure is defined as the force per unit area $\text{[math]}$ , where $\text{[math]}$ is the area in the reference/undeformed configuration. Note that for the pressure defined on element faces identified using the SURFACETOPO command, or on elements other than elements 128 and 129, this is the only definition of pressure currently available.
`NO_GHOSTING`	Sub-command keyword for deactivating ghosting in a contact search performed using the ACME library (characters).
`NO_MULTIPLE_INTERACTIONS`	Sub-command keyword for disabling multiple interactions in the contact search, when this search is performed using the ACME library (characters).
`NO_NORMAL_SMOOTHING`	Sub-command keyword for deactivating normal smoothing in the contact search, when this search is performed using the ACME library (characters).
`NO_SECONDARY`	Sub-command keyword for deactivating the secondary decomposition in the contact search of the ACME library (characters).
`NO_WARPED_VOLUME`	Sub-command keyword for activating an option to accelerate contact search when using the ACME library (characters). This option should be activated only when none of the quadrilateral faces of the contact or tied surfaces are initially warped or can become warped during the simulation.
`OLD_DYNAMIC_SEARCH`	Sub-command keyword for disabling the so-called new augmented method for contact search when this search is performed using the ACME library (characters).
`PARTITION_GAP`	Sub-command keyword for activating the following option in the contact search, when this search is performed using the ACME library (characters). The purpose of this option is to partition a gap into the part that occurs durring the current computational time-step and that which pre-existed at the previous computational time-step.
`RESOLUTION_TYPE`	Sub-command keyword for specifying the type of normal smoothing in contact when the contact search is performed using the ACME library (characters).
`flagRT`	Specifies the type of normal smoothing (integer): 0 specifies that a node-based normal is to be used, while 1 (which is the default value) specifies that an edge-based normal is to be used.
`SHARP_NON_SHARP_ANGLE`	Sub-command keyword for specifying the minimum angle parameter used for multiple interactions and normal smoothing when contact search is performed using the ACME library (characters).
`theta`	Specifies the value of the minimum angle parameter in degrees (float). The default value is 30 degrees.
`SHELL_SIMPLE_LOFTING`	Sub-command keyword for activating an alternative simplified lofting algorithm in the contact search of the ACME library (characters).
`SKIP_PHYSICAL_FACES`	Sub-command keyword for activating the following option in the contact search, when this search is performed using the ACME library (characters). This option disables a feature of the ACME library designed to identify certain corner cases that may be difficult for the search algorithm to otherwise handle.

45 GRAVITATIONAL ACCELERATION

The GRAVITY command is used to specify directional gravitational acceleration constants. The input format is given below.

`COEFF_X`	Gravitational Acceleration Constant in the X direction.
`COEFF_Y`	Gravitational Acceleration Constant in the Y direction.
`COEFF_Z`	Gravitational Acceleration Constant in the Z direction.

46 GROUPS

The GROUPS command can be used to organize elements into groups according to their attribute number (see ATTRIBUTES), and nodes into groups according to the integer number identifying them or the surface to which they belong (see SURFACETOPO). For example, the notion of a group of elements is used by the RANDOM command to attribute a defined random material property to a group of elements. That of a group of nodes is used by the OUTPUT command to output computed results for groups of nodes.

`A`	Sub-command keyword (character) signaling that elements are to be grouped according to their attribute number — that is, all elements whose attribute is the same as `ATTRIBUTE#` or within the range [`STARTING_ATTRIBUTE#`, `ENDING_ATTRIBUTE#`] are to be put in the same group `GROUP#`.
`ATTRIBUTE#`	Attribute ID number of the elements to be placed in the same group `GROUP#` (integer).
`STARTING_ATTRIBUTE#`	First attribute ID number of a sequence of attribute ID numbers that define the group `GROUP#` (integer).
`ENDING_ATTRIBUTE#`	Last attribute ID number of a sequence of attribute ID numbers that define the group `GROUP#` (integer).
`N`	Sub-command keyword (character) signaling that nodes are to be grouped according to their node identifying number — that is, the node whose identifying number is `NODE#` or all nodes whose identifying numbers are within the range [`STARTING_NODE#`, `ENDING_NODE#`] are to be put in the same group `GROUP#`.
`N SURFACE`	Sub-command keywords (characters) signaling that nodes are to be grouped according to the surface to which they belong, and therefore according to the integer number identifying that surface (see SURFACETOPO).
`NODE#`	ID number of the node to be placed in the group `GROUP#` (integer).
`STARTING_NODE#`	First node ID number of a sequence of node ID numbers that define the group `GROUP#` (integer).
`ENDING_ATTRIBUTE#`	Last node ID number of a sequence of node ID numbers that define the group `GROUP#` (integer).
`GROUP#`	Group ID number of the constructed group of elements or nodes (integer).

47 HEAT CONDUCTION COEFFICIENT-TEMPERATURE TABLE

The CCTT command can be used to describe, for a given material, the evolution of the heat conduction coefficient with temperature. This evolution can be specified here in a curve (or one-dimensional table) defined by pairs of heat conduction coefficient and temperature values. Linear interpolation is used for "in between" points, and the extrema values are adopted for "outside" points. Several curves can be specified, one after the other. Each curve is identified by an ID number as described below.

Note 1: Currently, this command is supported only by the 4-noded tetrahedral termal element (type 50).

`CURVE`	Sub-command keyword (characters) that signals the definition of a heat conduction coefficient-temperature curve (or one-dimensional table).
`curve_id`	ID number for the following curve (or one-dimensional table) (integer).
`T_i`	A specified temperature value (real).
`YM_i`	A specified heat conduction coefficient value at temperature `T_i` (real).

48 HEAT ZERO ENERGY MODE

This command is effective only for quasistatic and transient thermal, thermoelastic, and aerothermal analyses involving thermal zero energy modes — that is, a singular conductivity matrix — when the equation solver specified under the STATICS command is the sparse or skyline solver. In this case, the constant temperature mode and the generalized inverse of the conductivity matrix are computed using a hybrid physics-algebraic algorithm, rather than the tolerance-based algorithm associated with the TRBM command.

49 HEAT ZERO ENERGY MODES FILTER

This command is effective for thermal simulations involving thermal zero energy modes. When this command is specified in the input file and the thermal problem contains zero energy modes, a non-trivial projector is constructed. In a static or quasistatic analysis, the transpose of this projector is applied to the (possibly variable) right hand-side to make sure that the external load is self-equilibrated and therefore admissible. In a dynamic analysis: a) this projector is applied to the initial solution (initial displacement and velocity fields), and b) at each time-step, the transpose of this projector is applied to the (time-dependent) right-hand side of the equation being solved. In all cases, the net effect is to work with (and output) a solution where the thermal zero energy modes have been filtered out.

The constructed projector can be written as

\text{[math]}

where I is the identity matrix, Z is the matrix of the zero energy modes of the thermal system (always computed with the HZEM method), and Q is either the identity matrix for static analysis, or the capacity matrix for quasistatic and dynamic analyses. Hence, in a quasistatic analysis, this command requires the specific heat to be present in the material properties specified under the MATERIAL command.

50 HELMHOLTZ

The command statement HELM can be used to specify an absorbing boundary condition, and/or a set of incident plane waves or point source terms associated with spherical waves for a frequency-domain acoustic or elastoacoustic (Helmholtz) problem. Its input format is given below.

Note 1: For AERO-S, the time-harmonic form of the solution of a formulated Helmholtz problem is

\text{[math]}

, where

\text{[math]}

denotes the scalar field of interest — for example, the pressure perturbation —

\text{[math]}

is its amplitude, and

\text{[math]}

denotes its circular frequency. When the formulated Helmholtz problem includes an incident wave of amplitude

\text{[math]}

(which can also be specified as a souce term), AERO-S solves this problem for the scattered amplitude

\text{[math]}

BGTL $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
POINTSOURCE $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
PLANEWAVE $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
. . .
. . .
. . .
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$

`BGTL`
$\text{[math]}$	Order (0, 1, or 2) of the generalized Bayliss-Gunburger-Turkel non reflecting condition to be applied on the artificial boundary $\text{[math]}$ specified under the `HARB` command (integer).
$\text{[math]}$	This real number (float) is to be used only when the artificial boundary $\text{[math]}$ (see HARB) is supposed to be either a sphere or an ellipsoid, and some geometric approximations generated by AERO-S are to be overwritten by values that can in that case be evaluated exactly. Otherwise, $\text{[math]}$ should simply not be inputted. For a sphere, the curvature of $\text{[math]}$ , which is otherwise automatically approximated by AERO-S is overwritten by $\text{[math]}$ . Similarly, for an ellipsoid of the form $\text{[math]}$ , $\text{[math]}$ .
$\text{[math]}$	This real number (float) is to be used only when the artificial boundary $\text{[math]}$ (see HARB) is supposed to be an ellipsoid, and some geometric approximations generated by AERO-S are to be overwritten by values that can in that case be evaluated exactly. Otherwise, $\text{[math]}$ should simply not be inputted. For an ellipsoid of the form $\text{[math]}$ , $\text{[math]}$ .
`POINTSOURCE`	Keyword indicating that the Dirichlet and/or Neumann boundary conditions (see HDIR and HDNB) of the acoustic (Helmholtz) or elastoacoustic problem defined by this command are associated with a time-harmonic spherical wave of the form $\text{[math]}$ , where $\text{[math]}$ , and propagated by a point source located at the point $\text{[math]}$ (character). Multiple spherical waves and point sources can be specified under this command leading to multiple acoustic or elastoacoustic analyses. Hence, this line should be followed by a line specifying the number of point sources and spherical waves, $\text{[math]}$ , and $\text{[math]}$ lines specifying for each wave its point source $\text{[math]}$ . When used to define Neumann boundary conditions (see HDNB), this option is available only for the faces of type 10 and 11 (see HDNB).
$\text{[math]}$	Number of point sources propagating spherical waves (integer).
$\text{[math]}$	x coordinate of the location of a point source (float).
$\text{[math]}$	y coordinate of the location of a point source (float).
$\text{[math]}$	z coordinate of the location of a point source (float).
`PLANEWAVE`	Keyword indicating that the Dirichlet and/or Neumann boundary conditions (see HDIR and HDNB) of the acoustic (Helmholtz) or elastoacoustic problem defined by this command are associated with an incident time-harmonic plane wave of the form $\text{[math]}$ (character). Multiple such waves can be specified under this command leading to multiple acoustic or elastoacoustic analyses. Hence, this line should be followed by a line specifying the number of plane waves to be considered, $\text{[math]}$ , and $\text{[math]}$ lines specifying for each wave its direction of propagation $\text{[math]}$ .
$\text{[math]}$	Number of incident planar waves (integer).
$\text{[math]}$	Normalized x component of the direction of a planar wave (float).
$\text{[math]}$	Normalized y component of the direction of a planar wave (float).
$\text{[math]}$	Normalized z component of the direction of a planar wave (float).

51 HELMHOLTZ ANALYSIS (AXISYMMETRIC/PARTIALLY AXISYMMETRIC)

Note 2: This command is currently supported by the following two-dimensional, axisymmetric element types (see TOPOLOGY): type 59 (6-node triangle), type 60 (4-node quadrilateral), type 61 (3-node triangle), and type 62 (8-node quadrilateral).

Note 3: This command is currently supported only by the FETI solver (see STATICS), with the following restrictions:

Note 4: In the case of a partially axisymmetric scatterer and Neumann (sound-hard) boundary conditions, the user must:

Note 5: When one or more planar wave incident directions is/are specified using this command, the directions specified using the commands AXIHDIR, AXIHLMPC, and/or AXIHNEURD are ignored.

PLANEWAVE $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
. . .
. . .
. . .
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
NMODES nmodes_v
NTSLICES ntslices_v

`PLANEWAVE`	Sub-command keyword to specify one or more incident planar waves (characters).
$\text{[math]}$	Number of incident planar waves (integer).
$\text{[math]}$	Normalized $\text{[math]}$ component of the planar wave incident direction (real).
$\text{[math]}$	Normalized $\text{[math]}$ component of the planar wave incident direction (real).
$\text{[math]}$	Normalized $\text{[math]}$ component of the planar wave incident direction (real).
`NMODES nmodes_v`	This pair of sub-command keyword (characters) and corresponding numerical value (integer) specifies the number of Fourier modes to be used in the expansion of the solution in the two-dimensional computational domain associated with the axisymmetric component of the scatterer.
`NTSLICES ntslices_v`	This pair of sub-command keyword (characters) and corresponding numerical value (integer) is relevant only for postprocessing the three-dimensional solution. It specifies the number of angular ( $\text{[math]}$ ) slices ( $\text{[math]}$ ) of the overall computational domain where to postprocess the solution at the locations obtained by rotating the two-dimensional mesh associated with the axisymmetric component of the scatterer (integer).

52 HELMHOLTZ ARTIFICIAL ABSORBING BOUNDARY CONDITIONS *S*

The HARB command statement is used to specify the artificial boundary

\text{[math]}

on which the absorbing condition specified in the HELMHOLTZ command (see HELMHOLTZ) is to be applied. The input format is given below.

Note 3: When using a BGTL absorbing boundary condition, the face types chosen for constructing the artificial boundary

\text{[math]}

must be compatible with the faces of the Helmholtz elements (see TOPOLOGY) they overlay (see summary table given below).

FACE_TYPE	Problem Dimension	BGTL Order	ELEMENT_TYPE
1	2D	0,1,2	30,31,33,34,35,36
2	2D	0,1,2	32,38
3	3D	0,1,2	40,41
4	3D	0	44,45
6	3D	0,1,2	42
10	3D	0	95
11	3D	0	96
12	2D	0	98
13	2D	0	99

`FACE#`	Face (or edge in two dimensions) id number whose type and connectivity are to be specified (integer). In practice, this id number is ignored by AERO-S.
`FACE_TYPE`
1	2-node line segment. To be used with two-dimensional linear elements.
2	3-node line segment. To be used with two-dimensional quadratic elements.
3	3-node triangular face. To be used with three-dimensional linear tetrahedral element.
4	4-node quad face. To be used with three-dimensional linear hexahedral element.
6	6-node triangular face. To be used with three-dimensional quadratic tetrahedral element.
10	4, 9, 16 or 25-node quadrilaterial face. To be used with three-dimensional full isoparametric hexahedral elements.
11	3, 6, 10 or 15-node triangular face. To be used with three-dimensional full isoparametric tetrahedral elements.
12	2, 3, 4 or 5-node line segment. To be used with two-dimensional full isoparametric quadrilateral elements.
13	2, 3 or 4-node line segment. To be used with two-dimensional full isoparametric triangular elements.
`CONNECTIVITY_NODES`	These should be listed in a stacked fashion on a single line, and numbered clockwise (when looking from outside in three dimensions).

53 HELMHOLTZ ARTIFICIAL ABSORBING BOUNDARY CONDITIONS (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) *S*

The command AXIHARB is relevant only to the frequency-domain acoustic (Helmholtz) analysis of an axisymmetric or partially axisymmetric scatterer (see AXIHELMHOLTZ), where it can be used to specify an axisymmetric BGTL (Bayliss-Gunzberger-Turkel-Like) absorbing boundary condition on the chosen artificial boundary of the two-dimensional mesh associated with the axisymmetric component of the scatterer. Its input format is given below.

BGTL
SURFR SURFZ
NODE1# NODE2# [NODE3#]
...
...
NODE1# NODE2# [NODE3#]

`BGTL`	Specifies the order (0, 1, or 2) of the generalized Bayliss-Gunzburger-Turkel non reflecting condition as well as the shape of the artificial boundary $\text{[math]}$ on which this condition is applied (integer). Note that the shape of $\text{[math]}$ must be consistent with that implied by the list of nodes inputted below. The following values of this parameter are supported: `0`: basic Sommerfeld condition. `-1`: first-order BGTL condition applied on an artificial boundary $\text{[math]}$ corresponding to the projection on the two-dimensional mesh associated with the axisymmetric component of the scatterer of a cylinder of revolution parameterized in three parts by: $\text{[math]}$ = $\text{[math]}$ `SURFR` $\text{[math]}$ , $\text{[math]}$ `SURFR` $\text{[math]}$ , $\text{[math]}$ `SURFR` $\text{[math]}$ $\text{[math]}$ = $\text{[math]}$ `SURFZ` $\text{[math]}$ , $\text{[math]}$ `SURFZ` $\text{[math]}$ `SURFZ` $\text{[math]}$ , $\text{[math]}$ `SURFZ` $\text{[math]}$ On the two-dimensional mesh, a corner of $\text{[math]}$ is replaced by a circle and the two edges connecting at a corner are assumed to have the same size. `1`: first-order BGTL condition applied on an artificial boundary $\text{[math]}$ corresponding to the projection on the two-dimensional mesh associated with the axisymmetric component of the scatterer of an ellipsoid of revolution parameterized by: $\text{[math]}$ `SURFR` $\text{[math]}$ , (`SURFR` $\text{[math]}$ ) $\text{[math]}$ -`SURFZ` $\text{[math]}$ , (`SURFZ` $\text{[math]}$ ) `-2`: second-order BGTL condition applied on an artificial boundary $\text{[math]}$ corresponding to the projection on the two-dimensional mesh associated with the axisymmetric component of the scatterer of a cylinder of revolution parameterized in three parts by: $\text{[math]}$ = $\text{[math]}$ `SURFR` $\text{[math]}$ , $\text{[math]}$ `SURFR` $\text{[math]}$ , $\text{[math]}$ `SURFR` $\text{[math]}$ $\text{[math]}$ = $\text{[math]}$ `SURFZ` $\text{[math]}$ , $\text{[math]}$ `SURFZ` $\text{[math]}$ `SURFZ` $\text{[math]}$ , $\text{[math]}$ `SURFZ` $\text{[math]}$ On the two-dimensional mesh, a corner of $\text{[math]}$ is replaced by a circle and the two edges connecting at a corner are assumed to have the same size. `2`: second-order BGTL condition applied on an artificial boundary $\text{[math]}$ corresponding to the projection on the two-dimensional mesh associated with the axisymmetric component of the scatterer of an ellipsoid of revolution parameterized by: $\text{[math]}$ `SURFR` $\text{[math]}$ , (`SURFR` $\text{[math]}$ ) $\text{[math]}$ -`SURFZ` $\text{[math]}$ , (`SURFZ` $\text{[math]}$ )
`SURFR`	Real-valued coefficient contributing to the parameterization of the artificial boundary $\text{[math]}$ (real). See above.
`SURFZ`	Real-valued coefficient contributing to the parameterization of the artificial boundar $\text{[math]}$ y (real). See above.
`NODE1#`	ID number of the first node of a line element of the two-dimensional mesh associated with the axisymmetric component of the scatterer, contributing to the geometrical definition of the artificial boundary $\text{[math]}$ (integer).
`NODE2#`	ID number of the second node of the same line element of the two-dimensional mesh associated with the axisymmetric component of the scatterer, contributing to the geometrical definition of the artificial boundary $\text{[math]}$ (integer).
`NODE3#`	ID number of the optional third node of the same line element of the two-dimensional mesh associated with the axisymmetric component of the scatterer, contributing to the geometrical definition of the artificial boundary $\text{[math]}$ (integer).

54 HELMHOLTZ AUXILIARY SURFACE FAR-FIELD PATTERN (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) *S*

The command AXIHASFFP is relevant only to the frequency-domain acoustic (Helmholtz) analysis of an axisymmetric or partially axisymmetric scatterer (see AXIHELMHOLTZ). It can be used to describe, using line elements that are edges of the two-dimensional mesh associated with the axisymmetric component of the scatterer, a closed auxiliary surface that can be used to compute the far-field pattern of the solution: this makes this command (and the related command AXIHNOBAS) necessary for computing (correctly) the far-field pattern (see AXIHFFP). The closed auxiliary surface should not intersect any component of the scatterer.

LINE_ELEMENT# LINE_ELEMENT_TYPE SC CONNECTIVITY_NODES
...
...
LINE_ELEMENT# LINE_ELEMENT_TYPE SC CONNECTIVITY_NODES

`LINE_ELEMENT#`	ID number of a line element corresponding to an edge of the two-dimensional mesh and contributing to the description of the auxiliary surface defined above (integer). The type and connectivity of this edge should be specified as described below (integer). Currently, this parameter is ignored by AERO-S.
`LINE_ELEMENT_TYPE`	Line element type (integer).
11	2-node line segment, to be used with two-dimensional axisymmetric linear elements.
12	3-node line segment, to be used with two-dimensional axisymmetric quadratic elements.
`SC`	Sommerfeld constant (real). Currently this value is ignored by AERO-S.
`CONNECTIVITY_NODES`	List of node ID numbers describing the connectivity of a line segment (integers).

55 HELMHOLTZ CONSTRAINED FICTITIOUS NODES (PARTIALLY AXISYMMETRIC) *S*

The command AXIHCFNO is relevant only to the frequency-domain acoustic (Helmholtz) analysis of a partially axisymmetric scatterer (see AXIHELMHOLTZ) with Neumann (sound-hard) boundary conditions. It can be used to identify the list of nodes in the fictitious domain located on the intersection between the axisymmetric and non-axisymmetric surfaces of the scatterer, where AXIHNEUFD can then compute the appropriate source term. Its input format is given below.

NODE# ID number of a node of the three-dimensional mesh located on the intersection between the axisymmetric and non-axisymmetric surfaces of the scatterer (integer).

56 HELMHOLTZ DIRICHLET BOUNDARY CONDITIONS *S*

The HDIR command statement is used to specify nodal Dirichlet boundary conditions for a frequency-domain acoustic scattering (Helmholtz) problem. The input format is given below.

`NODE#`	Node number where the Dirichlet boundary condition is specified (integer).
`DOF#`	Degree of freedom local number where the boundary condition is specified (integer). This number should be set to 8.
`REAL_PART_VALUE`	Real part of the value of the specified boundary condition (float).
`IMAGINARY_PART_VALUE`	Imaginary part of the value of the specified boundary condition (float).

57 HELMHOLTZ DIRICHLET BOUNDARY CONDITIONS (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) *S*

The command AXIHDIR is relevant only to the frequency-domain acoustic (Helmholtz) analysis of an axisymmetric or partially axisymmetric scatterer (see AXIHELMHOLTZ). It can be used to specify nodal Dirichlet (sound-soft) boundary conditions on the two-dimensional mesh associated with the axisymmetric component of the scatter of the form

\text{[math]}

, where

\text{[math]}

is the scattered wave,

\text{[math]}

is the amplitude of the incident time-harmonic planar wave specified in AXIHELMHOLTZ or below (see also HELMHOLTZ),

\text{[math]}

is the pure imaginary number satisfying

\text{[math]}

\text{[math]}

is the wavenumber specified in AXIHWAN,

\text{[math]}

is the vector position of a point in space,

\text{[math]}

is the normalized direction of the incident planar wave, and

\text{[math]}

is in general a complex-valued constant.

Note 2: In this context, the classical Dirichlet (sound-soft) boundary condition corresponds to

\text{[math]}

CR CI
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
NODE#
...
...
NODE#

`CR`	Real part of the constant $\text{[math]}$ of the Dirichlet (sound-soft) boundary condition $\text{[math]}$ (real).
`CI`	Imaginary part of the constant $\text{[math]}$ of the Dirichlet (sound-soft) boundary condition $\text{[math]}$ (real).
$\text{[math]}$	Normalized $\text{[math]}$ component of the planar wave incident direction (real).
$\text{[math]}$	Normalized $\text{[math]}$ component of the planar wave incident direction (real).
$\text{[math]}$	Normalized $\text{[math]}$ component of the planar wave incident direction (real).
`NODE#`	ID number of a node of the two-dimensional mesh where the nodal Dirichlet (sound-soft) boundary condition is specified (integer).

58 HELMHOLTZ DISTRIBUTED NEUMANN BOUNDARY CONDITION *S*

The HDNB command statement can be used to specify on all or segments of the surface of a scatterer a distributed Neumann boundary condition of the form

\text{[math]}

, where the superscripts

\text{[math]}

and

\text{[math]}

designate scattered and incident quantities, respectively. The incident time-harmonic wave can be a time-harmonic plane wave specified by PLANEWAVE, or a time-harmonic spherical wave propagating from a source located at a point specified by POINTSOURCE in HELMHOLTZ. Note that for problems involving a nonhomogenous fluid, HDNB can only be used to define a surface that is submerged entirely in one and only one fluid.

`FACE#`	Face (or edge in two dimensions) id number whose type and connectivity are to be specified (integer). In practice, this id number is ignored by FEM.
`FACE_TYPE`
1	2-node line segment. To be used with two-dimensional linear elements.
2	3-node line segment. To be used with two-dimensional quadratic elements.
3	3-node triangular face. To be used with three-dimensional linear tetrahedral elements.
4	4-node quad face. To be used with three-dimensional linear hexahedral elements.
6	6-node triangular face. To be used with three-dimensional quadratic tetrahedral elements.
10	4, 9, 16 or 25-node quadrilaterial face. To be used with three-dimensional full isoparametric hexahedral elements.
11	3, 6, 10 or 15-node triangular face. To be used with three-dimensional full isoparametric tetrahedral elements.
12	2, 3, 4 or 5-node line segment. To be used with two-dimensional full isoparametric quadrilateral elements.
13	2, 3 or 4-node line segment. To be used with two-dimensional full isoparametric triangular elements.
`CONNECTIVITY_NODES`	These should be listed in a stacked fashion on a single line, and numbered counter clockwise (when looking from infinity in three dimensions).

59 HELMHOLTZ FAR-FIELD PATTERN (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) *S*

The command AXIHFFP is relevant only to the frequency-domain acoustic (Helmholtz) analysis of an axisymmetric or partially axisymmetric scatterer (see AXIHELMHOLTZ), where it can be used to activate the outputting to a file of the far-field pattern of the acoustic pressure field. However: this field is computed only if the user also specifies in the AERO-S ASCII Input Command Data file the command AXIHASFFP; and it is correctly computed only if the user also specifies in the aforementioned file the command AXIHNOBAS.

The output file will have the prefix specified in OUTPUT for the result GHELMHOL and the extension ".ffp". It will contain on each line four values "

\text{[math]}

\text{[math]}

, real-part(ffp), imaginary-part(ffp)". The first two quantities are the spherical angles (expressed in radians) that determine the direction

\text{[math]}

. The number of output lines depends on the parameter INCREMENT (see below).

INCREMENT Specifies the number of longitudinal directions where to evaluate the far-field pattern: (INCREMENT/2)+1) latitudinal directions are also considered and therefore the far-field pattern is evaluated at ((INCREMENT/2)+1))*INCREMENT points uniformly distributed in spherical coordinates.

60 HELMHOLTZ LINEAR MULTIPOINT CONSTRAINTS

The HLMPC command statement is used to specify a set of complex linear multipoint constraint equations of the form

in a frequency-domain acoustic model. There is no limitation on the number of multipoint constraints, or number of degrees of freedom related by the same constraint equation. The format of this command statement is as follows.

CONSTRAINT# RHS CONSTRAINT_METHOD
NODE# DOF# REAL-PART-COEFF IMAGINARY-PART-COEFF
.
.
NODE# DOF# REAL-PART-COEFF IMAGINARY-PART-COEFF

`CONSTRAINT#`	This corresponds to the constraint equation number `i` (integer).
`RHS`	This is the right-hand side $\text{[math]}$ of the `i`-th constraint equation (float). It can have both a real and an imaginary part, in which case the real part is specified first and followed by the imaginary part.
`CONSTRAINT_METHOD`	This is the method for enforcing the constraint (characters). The default method is set in CONSTRAINTS and used whenever this entry is omitted.
`multipliers`	The Lagrange multiplier method.
`elimination`	The elimination method.
`penalty` [`beta`]	The penalty method. The parameter `beta` should be a large positive number, typically of the order of $\text{[math]}$ (no default value is provided).
`NODE#`	This is the number of the node contributing the coefficient $\text{[math]}$ of the `i`-th constraint equation (integer).
`DOF#`	This is the local number of the degree of freedom at the node specified above contributing the coefficient $\text{[math]}$ of the `i`-th constraint equation (integer).
`REAL_PART_VALUE`	This is the real part of the coefficient $\text{[math]}$ of the `i`-th constraint equation (float).
`IMAGINARY_PART_VALUE`	This is the imaginary part of the coefficient $\text{[math]}$ of the `i`-th constraint equation (float).

61 HELMHOLTZ LINEAR MULTIPOINT CONSTRAINTS (PARTIALLY AXISYMMETRIC) *S*

The command AXIHLMPC is relevant only to the frequency-domain acoustic (Helmholtz) analysis of a partially axisymmetric scatterer (see AXIHELMHOLTZ). It specifies the (weak) enforcing of a set of complex-valued linear multipoint constraint equations corresponding to:

Currently, the axisymmetric and non-axisymmetric components of the scatterer are assumed to have matching discrete interfaces, which simplifies the expression, input, and processing of these constraints.

Note 2: In this context, the classical Dirichlet (sound-soft) boundary condition corresponds to

\text{[math]}

CR CI
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
NODE# ANGLE1 ANGLE2 NWEDGES
...
...
NODE# ANGLE1 ANGLE2 NWEDGES

`CR`	The setting of this real-valued parameter (real) depends on the boundary conditions of the analysis: In the case of Dirichlet (sound-soft) boundary conditions, `CR` is the real part of the constant $\text{[math]}$ in the boundary condition $\text{[math]}$ . In the case of Neumann (sound-hard) boundary conditions, `CR` should be set to $\text{[math]}$ .
`CI`	The setting of this real-valued parameter (real) depends on the boundary conditions of the analysis: In the case of Dirichlet (sound-soft) boundary conditions, `CI` is the imaginary part of the constant $\text{[math]}$ in the boundary condition $\text{[math]}$ (real). In the case of Neumann (sound-hard) boundary conditions, `CI` should be set to $\text{[math]}$ .
$\text{[math]}$	Normalized $\text{[math]}$ component of the planar wave incident direction (real).
$\text{[math]}$	Normalized $\text{[math]}$ component of the planar wave incident direction (real).
$\text{[math]}$	Normalized $\text{[math]}$ component of the planar wave incident direction (real).
`NODE#`	ID number of a node of the two-dimensional mesh associated with the axisymmetric component of the scatterer, where any of the constraints outlined above is to be enforced (integer).
`ANGLE1`	Lower bound $\text{[math]}$ of the angular interval $\text{[math]}$ in which the two-dimensional mesh associated with the axisymmetric component of the scatterer has to be rotated to match the three-dimensional mesh associated with the non-axisymmetric component of the scatterer at the interface between both components (real).
`ANGLE2`	Upper bound $\text{[math]}$ of the angular interval $\text{[math]}$ in which the two-dimensional mesh associated with the axisymmetric component of the scatterer has to be rotated to match the three-dimensional mesh associated with the non-axisymmetric component of the scatterer at the interface between both components (real).
`NWEDGES`	Number of uniform wedges in the interval $\text{[math]}$ (integer) that: In the case of Dirichlet (sound-soft) boundary conditons, generate the locations of the rotated nodes of the two-dimensional mesh associated with the axisymmetric component of the scatterer, where to apply the linear multipoint constraints. In the case of Neumann (sound-hard) boundary conditions, recover the locations of the nodes of the three-dimensional mesh associated with the non-axisymmetric component of the scatterer.

62 HELMHOLTZ LOCATIONS WHERE TO COMPUTE THE KIRCHHOFF INTEGRAL

When KIRCHHOFF is selected as an OUTPUT result and the surface of the scatterer is defined using the command HSCB, this command should be used to specify the locations of the points where the (far-field) solution of a frequency-domain acoustic or elastoacoustic (Helmholtz) problem is to be evaluated using the Kirchhoff integral and outputted. These points do not need to be nodes of the mesh. Usually, but not necessarily, they are outside the computational domain, in the far-field. The keyword KIRLOC should be followed by as many lines as there are points where it is desired to evaluate the solution of the aforementioned Helmholtz problem. Each line contains the coordinates of such a point.

`X-ORDINATE`	X-ordinate of a point where to evaluate the solution of the Helmholtz problem to be solved using the Kirchhoff integral (real).
`Y-ORDINATE`	Y-ordinate of a point where to evaluate the solution of the Helmholtz problem to be solved using the Kirchhoff integral (real).
`Z-ORDINATE`	Z-ordinate of a point where to evaluate the solution of the Helmholtz problem to be solved using the Kirchhoff integral (real).

63 HELMHOLTZ NEUMANN BOUNDARY CONDITIONS *S*

The HNEU command statement is used to specify the nodal Neumann boundary conditions for a frequency-domain acoustic scattering (Helmholtz) problem. The input format is given below.

`LOADSET_ID`	Optional non-negative integer which identifies explicitly the "load" set to which the source term generated by this command belongs to (integer). The default value is 0. Hence, the `HNEU` command can be repeated as many times as desired within the same input file using each time a different value for `LOADSET_ID` and different data. The LOADCASE command can refer to `LOADSET_ID` to define one or multiple "load" cases for static analysis (see the STATICS command and the explanation of its sub-command keyword `CASES`), and/or the "load" case for dynamic analysis.
`NODE#`	Node number where the Neumann boundary condition is specified (integer).
`REAL_PART_VALUE`	Real part of the value of the specified boundary condition (float).
`IMAGINARY_PART_VALUE`	Imaginary part of the value of the specified boundary condition (float).

64 HELMHOLTZ NEUMANN BOUNDARY CONDITIONS – FICTITIOUS DOMAIN (PARTIALLY AXISYMMETRIC) *S*

The command AXIHNEUFD is only relevant to the frequency-domain acoustic (Helmholtz) analysis of a partially axisymmetric scatterer (see AXIHELMHOLTZ) with Neumann (sound-hard) boundary conditions. It can be used to activate the computation of the source term acting on the external surfaces of the non-axisymmetric component of the scatterer and that acting on the intersection between its axisymmetric and non-axisymmetric surfaces. Its input format is given below.

`EL_TYPE`	Line element or surface element type (integer).
4	4-node quadrilateral element, to be used with three-dimensional linear hexahedral elements, to compute the source term acting on the intersection between the axisymmetric and non-axisymmetric surfaces of the scatterer.
8	8-node quadrilateral, to be used with three-dimensional quadratic hexahedral elements, to compute the source term acting on the intersection between the axisymmetric and non-axisymmetric surfaces of the scatterer.
11	2-node line segment, to be used with two-dimensional axisymmetric linear elements, to compute the source term acting on the external surfaces of the non-axisymmetric component of the scatterer.
12	3-node line segment, to be used with two-dimensional axisymmetric quadratic elements, to compute the source term acting on the external surfaces of the non-axisymmetric component of the scatterer.
14	4-node quadrilateral, to be used with three-dimensional linear hexahedral elements, to compute the source term acting on the external surfaces of the non-axisymmetric component of the scatterer.
18	8-node quadrilateral, to be used with three-dimensional quadratic hexahedral elements, to compute the source term acting on the external surfaces of the non-axisymmetric component of the scatterer.
`INT`	Integer number that must be set as follows:
`-1`	for `EL_TYPE` = 4 and 8.
`0`	for `eL_TYPE` = 11, 12, 14, and 18.
`NYSLICES`	Number of slices in the $\text{[math]}$ (vertical) direction, to compute the source term acting on the external surfaces of the non-axisymmetric component of the scatterer, or that acting on the intersection between its axisymmetric and non-axisymmetric surfaces (integer).
`Y1`	Lower bound $\text{[math]}$ (real) of the interval $\text{[math]}$ (see `NYSLICES` above).
`Y2`	Upper bound $\text{[math]}$ (real) of the interval $\text{[math]}$ (see `NYSLICES` above).
`CONNECTIVITY_NODES`	List of node ID numbers describing the connectivity of the line or surface element (integers).

65 HELMHOLTZ NEUMANN BOUNDARY CONDITIONS – REAL DOMAIN (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) *S*

The command AXIHNEURD is relevant only to the frequency-domain acoustic (Helmholtz) analysis of an axisymmetric or partially axisymmetric scatterer (see AXIHELMHOLTZ). It can be used to specify, in the real part of the computational domain, nodal boundary conditions corresponding to the Neumann (sound-hard) boundary condition of the form

\text{[math]}

, where the superscripts

\text{[math]}

and

\text{[math]}

designate scattered and incident waves, respectively,

\text{[math]}

denotes the normalized outward normal to the surface of the scatterer,

\text{[math]}

is the amplitude of the incident time-harmonic planar wave specified in AXIHELMHOLTZ or below (see also HELMHOLTZ),

\text{[math]}

is the pure imaginary number satisfying

\text{[math]}

\text{[math]}

is the wavenumber specified in AXIHWAN,

\text{[math]}

is the vector position of a point in space,

\text{[math]}

is the normalized direction of the incident planar wave, and

\text{[math]}

is in general a complex-valued constant.

Note 2: In this context, the classical Dirichlet (sound-soft) boundary condition corresponds to

\text{[math]}

CR CI
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
NODE1# NODE2# [NODE3#]
...
...
NODE1# NODE2# [NODE3#]

`CR`	Real part of the constant $\text{[math]}$ of the specified Neumann (sound-hard) boundary condition associated with $\text{[math]}$ (real).
`CI`	Imaginary part of the constant $\text{[math]}$ of the specified Neumann (sound-hard) boundary condition associated with $\text{[math]}$ (real).
$\text{[math]}$	Normalized $\text{[math]}$ component of the planar wave incident direction (real).
$\text{[math]}$	Normalized $\text{[math]}$ component of the planar wave incident direction (real).
$\text{[math]}$	Normalized $\text{[math]}$ component of the planar wave incident direction (real).
`NODE1#`	ID number of the first node of an element of the two-dimensional mesh associated with the axisymmetric component of the scatterer where the Neumann (sound-hard) boundary condition is specified (integer).
`NODE2#`	ID number of the second node of an element of the two-dimensional mesh associated with the axisymmetric component of the scatterer where the Neumann (sound-hard) boundary condition is specified (integer).
`NODE3#`	ID number of the optional third node of an element of the two-dimensional mesh associated with the axisymmetric component of the scatterer where the Neumann (sound-hard) boundary condition is specified (integer).

66 HELMHOLTZ NODES BELOW AUXILIARY SURFACE (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) *S*

The command AXIHNOBAS is relevant only to the frequency-domain acoustic (Helmholtz) analysis of an axisymmetric or partially axisymmetric scatterer (see AXIHELMHOLTZ). It can be used to list all nodes of the two-dimensional mesh associated with the axisymmetric component of the scatterer that are enclosed by the auxiliary surface defined in AXIHASFFP for the purpose of computing the far-field pattern of the solution, so that these nodes can be skipped during the computation of the far-field pattern. Hence, this command is necessary for correctly computing the far-field pattern (see AXIHFFP).

NODE# ID number of a node of the two-dimensional mesh associated with the axisymmetric component of the scatterer that is enclosed by the auxiliary surface defined in AXIHASFFP (integer).

67 HELMHOLTZ SCATTERER BOUNDARY *S*

The HSCB command statement is used to specify the surface of a scatterer. It is used to compute the farfield pattern of a frequency-domain acoustic solution, and therefore is necessary for the output of that farfield pattern (see OUTPUT).

`FACE#`	Face (or edge in two dimensions) id number whose type and connectivity are to be specified (integer). In practice, this id number is ignored by FEM.
`FACE_TYPE`
1	2-node line segment. To be used with two-dimensional linear elements.
2	3-node line segment. To be used with two-dimensional quadratic elements.
3	3-node triangular face. To be used with three-dimensional linear tetrahedral elements.
4	4-node quad face. To be used with three-dimensional linear hexahedral elements.
6	6-node triangular face. To be used with three-dimensional quadratic tetrahedral elements.
10	4, 9, 16 or 25-node quadrilaterial face. To be used with three-dimensional full isoparametric hexahedral elements.
11	3, 6, 10 or 15-node triangular. To be used with three-dimensional full isoparametric tetrahedral elements.
12	2, 3, 4 or 5-node line segment. To be used with two-dimensional full isoparametric quadrilateral elements.
13	2, 3 or 4-node line segment. To be used with two-dimensional full isoparametric triangular elements.
`CONNECTIVITY_NODES`	These should be listed in a stacked fashion on a single line, and numbered counter clockwise (when looking from outside in three dimensions).

68 HELMHOLTZ WAVE NUMBER (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) *S*

The command AXIHWAN is relevant only to the frequency-domain acoustic (Helmholtz) analysis of an axisymmetric or partially axisymmetric scatterer (see AXIHELMHOLTZ), where it can be used to specify the wavenumber for such an analysis. Its input format is given below.

KAPPA Wavenumber at which the frequency-domain acoustic analysis is to be performed (real).

69 HELMHOLTZ WET INTERFACE BOUNDARY *S*

The HWIB command satement can be used to describe the wet interface boundary of the structure in a coupled frequency response elastoacoutic (fluid-structure) problem where a single mesh is used to discretize both of the computional acoustic fluid and structural domains. Its input format is given below.

`FACE#`	Face (or edge in two dimensions) id number whose type and connectivity are to be specified (integer). In practice, this id number is ignored by FEM.
`FACETYPE`
10	4, 9, 16 or 25-node quadrilaterial face (to be used appropriately with three-dimensional full isoparametric hexahedral elements).
11	3, 6, 10 or 15-node triangular (to be used appropriately with three-dimensional full isoparametric tetrahedral elements).
12	2, 3, 4 or 5-node line segment (to be used appropriately with two-dimensional full isoparametric quadrilateral elements).
13	2, 3 or 4-node line segment (to be used appropriately with two-dimensional full isoparametric triangular elements).
`CONNECTIVITY_NODES`	These should be listed in a stacked fashion on a single line, and numbered as shown in the following examples:
	9-noded quad:
	7 8 9
	4 5 6
	1 2 3
	6-noded triangle:
	6
	4 5
	1 2 3
	etc.

70 HYDROELASTIC FLUID/STRUCTURE BOUNDARY

The HEFSB command is used to specify the fluid-structure interface boundary in a hydroelastic eigenvalue problem. The underlying discrete model assumes that each node on this interface is shared by fluid and structural elements. The input format of this command is given below.

`FACE#`	Face (or edge in two dimensions) identification number whose type and connectivity are to be specified (integer).
`FACE_TYPE`
1	2-node line segment (to be used appropriately with two-dimensional linear elements).
2	3-node line segment (to be used appropriately with two-dimensional quadratic elements).
3	3-node triangular face (to be used appropriately with three-dimensional linear tetrahedral and prismatic elements).
4	4-node quadrilateral face (to be used appropriately with three-dimensional linear hexahedral and prismatic elements).
6	6-node triangular face (to be used appropriately with three-dimensional quadratic tetrahedral elements).
10	Quadrilateral face (to be used appropriately with higher-order iso-parametric hexahedral elements).
11	Triangular face (to be used appropriately with higher-order iso-parametric tetrahedral elements).
12	Line segment (to be used appropriately with higher-order iso-parametric quadrilateral elements).
13	Line segment (to be used appropriately with higher-order iso-parametric triangular elements).
`CONNECTIVITY_NODES`	These should be listed in a stacked fashion on a single line. The nodes of low-order faces should be ordered counter-clockwise (when looking from infinity in three dimensions). Those of higher-order faces (type 10–13) should be ordered from left to right and bottom to top using any convenient axis system (when viewed from infinity in three dimensions).

71 HYDROELASTIC FREE SURFACE BOUNDARY

The HEFRS command can be used to specify the free surface boundary either in a hydroelastic eigenvalue problem, or in an acoustic or elastoacoustic (fluid-structure interaction) problem where the fluid is assumed to be weightless. At each node located on this free surface, AERO-S automatically applies a zero Dirichlet boundary condition for the fluid potential equation in the first case, and for the scattered pressure in the second case. For this reason, this command can be also used to apply these specific Dirichlet boundary conditions wherever desired in the fluid mesh.

`FACE#`	Face (or edge in two dimensions) identification number whose type and connectivity are to be specified (integer).
`FACE_TYPE`	Currently, this entry is ignored by AERO-S. Still, it must be assigned a dummy integer value (integer).
`CONNECTIVITY_NODES`	These should be listed in a stacked fashion on a single line.

72 HYPER REDUCTION OF THE INERTIA FORCES ASSOCIATED WITH A CONSTANT MASS MATRIX

The command WEIGHTMASS can be used to request during an online computation the hyper reduction of the inertia forces associated with a constant mass matrix using an inputted reduced mesh and associated weights, computed using the command RMSHC and the hyper reduction method ECSW.

73 IMPEDANCE ANALYSIS

For the purpose of frequency response analysis, structural damping can be represented in AERO-S using two different approaches:

If the physical domain of the acoustic fluid is unbounded but its computational support is truncated by an artificial boundary surface,

\text{[math]}

is a complex sparse matrix that arises from the discretization on this surface of the absorbing boundary specified in HELMHOLTZ. Alternatively, if the computational support of an infinite acoustic fluid domain is truncated using a perfectly matched layer (PML) whose properties are specified in MATERIAL,

\text{[math]}

is a complex, non-Hermitian matrix with non-zero entries only at the degrees of freedom inside the PML. If the parameters of the PML are kept constant when the frequency is varied, or the physical acoustic fluid domain is bounded and delimited by boundary surfaces of the structural domain, the above block matrix equation can be re-written in terms of complex non-Hermitian matrices

\text{[math]}

and

\text{[math]}

so that

\text{[math]}

The coupling matrix

\text{[math]}

is automatically constructed by AERO-S when the HWIB or FSINTERFACE command is present in the input file, and set to zero otherwise. The amplitude vector of the time-harmonic structural external forcing input,

\text{[math]}

, can be modeled using either the FORCES or PRESSURE command, as appropriate. The amplitude vector of the time-harmonic acoustic fluid external forcing input,

\text{[math]}

, can be modeled using the HNEU command, or a combination of the HELMHOLTZ, HDIR, and HDNB commands, as appropriate.

The case of a purely acoustic problem is governed by the second row of the above block matrix equation after setting

\text{[math]}

. That of a purely structural dynamic problem is given by the first row of the above block matrix equation after setting

\text{[math]}

FREQ $\text{[math]}$
RAYDAMP $\text{[math]}$ $\text{[math]}$
FREQSWEEP1 $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
FREQSWEEP $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
FREQSWEEP $\text{[math]}$
$\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$
FREQSWEEPA $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ IMOR $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
FREQSWEEPAW $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ IMOR $\text{[math]}$ localflag $\text{[math]}$ tol tole1f]
RECONS alg para_1 para_2 para_3
PADEPOLES $\text{[math]}$ $\text{[math]}$

`SWEEP_ID`	Optional non-negative integer which identifies explicitly a sweep case (integer). The default value is 0. Hence, the `IMPEDANCE` command can be repeated as many times as desired within the same input file using each time a different value for `SWEEP_ID` and different parameters. Doing so defines a multiple sweep case that is managed by the IMPEDANCE command itself.
`FREQ`	Sub-command keyword for specifying a forced frequency in the case of a single frequency response analysis (characters).
$\text{[math]}$	Value of the forced frequency (real). The corresponding value of $\text{[math]}$ is $\text{[math]}$ .
`RAYDAMP`	Sub-command keyword for specifying Rayleigh proportional damping coefficients for the entire structure (characters).
$\text{[math]}$	Rayleigh damping stiffness coefficient (real).
$\text{[math]}$	Rayleigh damping mass coefficient (real).
`FREQSWEEP1`	Sub-command keyword for requesting a frequency sweep analysis using a one-point configuration of the reconstruction algorithm specified after the sub-command keyword `RECONS` (characters). In this case, the following ( $\text{[math]}$ ) frequencies $\text{[math]}$ are swept in the frequency band $\text{[math]}$ $\text{[math]}$ This sub-command does not support frequency sweep problems with multiple right hand-sides.
$\text{[math]}$	Frequency defining the center of the frequency band $\text{[math]}$ (real).
$\text{[math]}$	Frequency sweep increment (real).
$\text{[math]}$	Together with $\text{[math]}$ and $\text{[math]}$ , this parameter defines the frequency band $\text{[math]}$ (integer).
`FREQSWEEP`	Sub-command keyword for requesting a frequency sweep analysis in a frequency band $\text{[math]}$ of interest using a reconstruction algorithm specified after the sub-command keyword `RECONS` (characters). In this case, the user can choose between two different schemes for specifying a set of interpolation frequency points within $\text{[math]}$ — that is, a set of frequencies where the response and its first few consecutive frequency derivatives are to be computed using the brute force approach — and then sampling frequencies in $\text{[math]}$ and rapidly computing the frequency response function at these points using the reconstruction algorithm `alg` specified after the sub-command keyword `RECONS` discussed below. The first scheme, referred to here as the "regular" sampling scheme, introduces $\text{[math]}$ equally-spaced interpolation frequencies $\text{[math]}$ in $\text{[math]}$ , including $\text{[math]}$ and $\text{[math]}$ . Hence, these frequencies are given by $\text{[math]}$ Then, the regular scheme samples each interval $\text{[math]}$ into $\text{[math]}$ equal frequency increments, and therefore into ( $\text{[math]}$ ) frequency points including $\text{[math]}$ and $\text{[math]}$ , where it rapidly reconstructs the frequency response function using the algorithm `alg`. Hence, the first scheme computes the frequency response at $\text{[math]}$ frequencies in the frequency band $\text{[math]}$ (counting $\text{[math]}$ and $\text{[math]}$ ). The second scheme, referred to here as the "irregular" sampling scheme, requires the user to specify first on the first line after the keyword `FREQSWEEP` the lower end of the frequency spectrum, $\text{[math]}$ , and then every other desired interpolation frequency $\text{[math]}$ (in ascending order) on a separate line together with an integer number $\text{[math]}$ specifying the sampling of the interval $\text{[math]}$ into $\text{[math]}$ equal frequency increments. Hence, it defines ( $\text{[math]}$ ) sampling frequencies in $\text{[math]}$ including $\text{[math]}$ and $\text{[math]}$ . The upper end of the frequency spectrum, $\text{[math]}$ , is in this case the last inputted interpolation frequency. It follows that if, for example, $\text{[math]}$ interpolation frequencies are inputted by the user, and $\text{[math]}$ is set to $\text{[math]}$ for all $\text{[math]}$ (again, for example), the second scheme computes the frequency response also at $\text{[math]}$ frequencies in the frequency band $\text{[math]}$ , including $\text{[math]}$ and $\text{[math]}$ . This sub-command does not support frequency sweep problems with multiple right hand-sides, except when performing the brute force approach (see `alg` below).
$\text{[math]}$	Lower end of the frequency band of interest $\text{[math]}$ (real).
$\text{[math]}$	Upper end of the frequency band of interest $\text{[math]}$ (real).
$\text{[math]}$	Number of equally-spaced interpolation frequencies $\text{[math]}$ to introduce in the frequency band of interest $\text{[math]}$ , including $\text{[math]}$ and $\text{[math]}$ (integer). Hence, these frequencies are given by $\text{[math]}$
$\text{[math]}$	When part of the definition of `FREQSWEEP`, this parameter specifies the number of equally-spaced frequency intervals in which a frequency "sub-band" $\text{[math]}$ — where $\text{[math]}$ and $\text{[math]}$ are interpolating frequencies (see above) — is to be sampled (integer). In this case, $\text{[math]}$ is sampled into ( $\text{[math]}$ ) frequencies, including $\text{[math]}$ and $\text{[math]}$ . When part of the definition of `FREQSWEEPA` or `FREQSWEEPAW`, this parameter specifies the number of equal size frequency intervals in which the frequency band of interest $\text{[math]}$ is to be sampled (integer). In this case, $\text{[math]}$ is sampled into ( $\text{[math]}$ ) frequencies, including $\text{[math]}$ and $\text{[math]}$ . When part of the definition of `FREQSWEEP`, the inputted value of this parameter must satisfy $\text{[math]}$ . When part of the definition of `FREQSWEEPA` or `FREQSWEEPAW`, it must satisfy $\text{[math]}$ . In both cases, the frequency response function is computed at all sampled frequency points.
$\text{[math]}$	Interpolation frequency (real).
$\text{[math]}$	Number of equal size frequency increments in which a frequency interval of the form $\text{[math]}$ is to be sampled (integer). In this case, $\text{[math]}$ is sampled into ( $\text{[math]}$ ) frequency points.
`FREQSWEEPA`	Sub-command keyword requesting an adaptive frequency sweep analysis in a frequency band $\text{[math]}$ of interest using a reconstruction algorithm specified after the sub-command keyword `RECONS` (characters). In this case, the user can set the maximum number of interpolation frequencies, specifiy the number of frequencies to sample and at which to reconstruct the frequency response function, specify the reconstruction algorithm, and tune some of the parameters of the automatic adaptation procedure. This sub-command supports frequency sweep problems with multiple right hand-sides.
`FREQSWEEPAW`	Sub-command keyword requesting an adaptive sweep analysis in the $\text{[math]}$ or $\text{[math]}$ domain using a windowing strategy with a rotating buffer along the frequency axis, and a reconstruction algorithm specified after the sub-command keyword `RECONS` (characters). The frequency $\text{[math]}$ is varied in the band $\text{[math]}$ of interest, and the parameter $\text{[math]}$ , when applicable, is varied in another band of interest $\text{[math]}$ or in a set of values $\text{[math]}$ . This sub-command supports frequency sweep problems with multiple right hand-sides.
`IMOR`	Speficies an interpolatory model order reduction algorithm for the adaptive frequency sweep procedures associated with the sub-command keywords `FREQSWEEPA` and `FREQSWEEPAW` (characters). Currently, three options are available: (1) `KrylovGalProjection`, (2) `GalProjection`, and (3) `WCAWEGalProjection`. These three algorithms are the same as those associated with the sub-command keyword `RECONS` and are described below. It is recommended to use `KrylovGalProjection` as much as possible, except for acoustic scattering problems and coupled fluid-structure interaction problems with structural damping and/or absorbing boundary conditions where `KrylovGalProjection` is not valid.
$\text{[math]}$	Specifies the tolerance level for assessing the convergence of the adaptive frequency sweep procedures associated with the sub-command keyword `FREQSWEEPA` and `FREQSWEEPAW` using the criterion $\text{[math]}$ where $\text{[math]}$ is the reconstructed value of $\text{[math]}$ using the chosen interpolatory model order reduction algorithm (real). The recommended setting for this parameter is $\text{[math]}$ , and the default setting is $\text{[math]}$ .
$\text{[math]}$	Specifies the maximum number of interpolation frequencies for the adaptive frequency sweep procedure associated with the sub-command keyword `FREQSWEEPA`. The recommended practice is $\text{[math]}$ (integer). If for such a setting of this parameter the value of the tolerance level $\text{[math]}$ (see below) is not reached, a higher value of $\text{[math]}$ should be used, or the frequency band of interest should be split in two smaller bands and a separate frequency sweep should be performed in each one of them instead. The default value of $\text{[math]}$ is 6.
$\text{[math]}$	Specifies the minimum number of solution vectors to be computed per interpolation frequency for the adaptive frequency sweep procedure associated with the sub-command keyword `FREQSWEEPA` (integer). The recommended value is the default value $\text{[math]}$ .
$\text{[math]}$	Specifies the maximum number of solution vectors to be computed per interpolation frequency for the adaptive frequency sweep procedure associated with the sub-command keyword `FREQSWEEPA` (integer). The recommended values are $\text{[math]}$ for the `KrylovGalProjection` algorithm, and $\text{[math]}$ - $\text{[math]}$ for the `GalProjection` algorithm. The default values for this parameter are 16 when `IMOR` = `GalProjection`, and 48 when `IMOR` = `KrylovGalProjection`.
$\text{[math]}$	Specifies the increment number of solution vectors per interpolation frequency to be considered for computation for the adaptive frequency sweep procedure associated with the sub-command keyword `FREQSWEEPA` (integer). The recommended value is the default value $\text{[math]}$ .
`localflag`	This integer parameter can be be set either to 0 or to 1. It controls the functioning of the adaptive frequency sweep with a windowing strategy command `FREQSWEEPAW` for problems with multiple right hand-sides specified using the command LOADCASE or the sub-command `PLANEWAVE` in HELMHOLTZ. If `localflag` = 0, a global Interpolatory Reduced-Order Model (IROM) is constructed for the strip $\text{[math]}$ or $\text{[math]}$ using the information computed at the interpolatory parameter points determined at the boundaries of this strip, and applied to the reconstruction of the solution at every sampled point inside this strip. This setting is suitable for frequency sweep problems with multiple right hand-sides specified using the sub-command `PLANEWAVE` in HELMHOLTZ because the underlying computational strategy relies on the describability of the multiple right hand-sides by a continuous function of a single parameter. If `localflag` = 1, the reduced-order basis $\text{[math]}$ is computed during the windowing strategy using the same interpolatory parameters $\text{[math]}$ as those determined for the computation of $\text{[math]}$ , and the solutions in the strip $\text{[math]}$ or the set $\text{[math]}$ are computed using a set of local IROMs. Each local IROM is constructed for an interval $\text{[math]}$ using information computed at the two points $\text{[math]}$ and $\text{[math]}$ , and used to reconstruct the solutions at all parameter points sampled inside the interval $\text{[math]}$ . Hence, the setting `localflag` = 1 is suitable for frequency sweep problems with multiple right hand-sides specified using the command `LOADCASE` as the underlying computational approach builds independent projections for each right hand-side.
$\text{[math]}$	Specifies the total number of snapshot vectors to be computed per interpolation frequency or interpolation point $\text{[math]}$ for the adaptive sweep procedure with a windowing strategy `FREQSWEEPAW` (integer).
`tol`	Tolerance for determining the placement of the next interpolation frequency $\text{[math]}$ in the context of the adaptive sweep procedure with a windowing strategy `FREQSWEEPAW`. A suitable value is such that `tol`*`epsilon` $\text{[math]}$ (real).
`tol1f`	Tolerance for controling the global-within-one-frequency algorithm (`localflag` = 0) that attempts to ensure that residual at the interpolation frequency is less than `tol`*`tol1f` (real). A suitable value is `tol1f` = $\text{[math]}$ .
`RECONS`	Sub-command keyword for defining a reconstruction algorithm in the case of a frequency sweep analysis and setting its parameters (characters).
`alg`	Name of the reconstruction algorithm (characters). Six such algorithms are available and listed below. The default value is `Taylor` with 8 derivatives. The brute force reconstruction algorithm corresponds to `Taylor` with 0 derivative.
`Taylor`	Taylor series expansion algorithm (characters).
`Pade`	Conventional multipoint Pade series expansion algorithm (characters).
`PadeLanczos`	Multipoint Pade series expansion algorithm based on a Lanczos procedure (characters). This algorithm is less prone to ill-conditioning and therefore better performing than the `Pade` algorithm. However, it is available only for purely structural or acoustic undamped frequency response problems where furthermore $\text{[math]}$ and $\text{[math]}$ are symmetric.
`KrylovGalProjection`	Interpolatory model order reduction algorithm based on a Galerkin projection and a Krylov subspace (characters). This algorithm, which cannot be used for acoustic scattering problems and coupled fluid-structure problems with structural damping and/or absorbing boundary conditions, delivers nevertheless a much better performance than both of the `Pade` and `GalProjection` algorithms for all other frequency response problems of the form given at the beginning of the description of the `IMPEDANCE` command. It is also known as the `KGP` algorithm.
`GalProjection`	Interpolatory model order reduction algorithm based on a Galerkin projection and orthogonalized frequency derivatives (characters). This algorithm is also known as the `DGP` algorithm.
`WCAWEGalProjection`	Interpolatory model order reduction algorithm based on the combination of the Well-Conditioned Asymptotic Waveform Evaluation (WCAWE) scheme, and the multipoint Galerkin projection interpolatory scheme with orthogonalized vectors. This algorithm is also known as the `WCAWE+DGP` algorithm. It is is preferred to `GalProjection` for acoustic scattering problems and coupled fluid-structure interaction problems with structural damping or absorbing boundary conditions.
`para_1`	For the `Taylor` algorithm, this parameter specifies the order of the Taylor series (integer). For the `Pade`, `PadeLanczos`, `GalProjection`, and `KrylovGalProjection` algorithms, it specifies how many of the $\text{[math]}$ interpolation frequencies to use at a time to apply a multipoint version of the chosen reconstruction algorithm. (Note however that for `GalProjection` and `KrylovGalProjection`, `para_1` = 1 and `para_1` = $\text{[math]}$ are currently the only options).
`para_2`	This parameter is relevant only for the `Pade`, `GalProjection`, and `KrylovGalProjection` reconstruction algorithms (integer). For `Pade`, it specifies the order of the numerator of the rational function (L of [L/M]) (integer). For `GalProjection`, it specifies the number of frequency derivatives of the response to compute at each interpolation frequency. For `KrylovGalProjection`, it specifies the number of Krylov vectors to compute at each interpolation frequency.
`para_3`	This parameter is relevant only for the `Pade` and `PadeLanczos` reconstruction algorithms. It specifies the order of the denominator of the rational function (M of [L/M]) (integer).
`PADEPOLES`	This sub-command keyword is active only with `alg` = `PadeLanczos` and needs input from the sub-command `FREQSWEEP` (see above) (characters). It also requires the presence in the input file of the MODE command to retrieve the EIGENMODES file or files associated with a previous eigen computation. This (these) file(s) should be placed in the execution path. In this case, this sub-command instructs AERO-S to: (1) compute the approximation by a multipoint Pade expansion of a rational transfer function whose poles are exactly the eigenvalues of the symmetric pencil of interest ( $\text{[math]}$ ), and (2) exploit these poles to identify, in a specified range of interest $\text{[math]}$ , the eigenvalues that may have been missed by a previous eigen computation in which the MODE command was used to store the results in the EIGENMODES file or files (characters). The multipoint Pade expansion is constructed using points $\text{[math]}$ that should be generated by the sub-command `FREQSWEEP` with $\text{[math]}$ playing the role of $\text{[math]}$ , $\text{[math]}$ and $\text{[math]}$ (and for example, $\text{[math]}$ ). The parameters of this expansion should be specified in `para_1`, `para_2` and `para_3` (see above). At the end of the computation, AERO-S outputs on the screen the poles of the Pade rational function in the specified range $\text{[math]}$ , excluding those poles corresponding to the modes read from the EIGENMODES file or files. The specified range $\text{[math]}$ can be narrower than that of the eigenvalues read in the EIGENMODES file or files. However, if it is wider, some of the poles of the Pade rational function may, in some cases, not correspond to missed eigenvalues. In any case, the output of the eigenvectors associated with the poles or missed eigenvalues is not currently implemented in AERO-S.
$\text{[math]}$	Lower end of an eigenvalue interval of interest (real).
$\text{[math]}$	Upper end of an eigenvalue interval of interest (real).

74 INITIAL ACCELERATIONS (Not Supported Yet)

The IACCELERATIONS command statement is used to specify a nodal acceleration type of initial conditions. Each node can have up to six degrees of freedom.

`NODE#`	Node number where the initial acceleration is specified (integer).
`DOF#`	Degree of freedom local number where the initial acceleration is specified (integer).
`VALUE`	Value of the specified initial acceleration (float).

75 INITIAL DISPLACEMENTS *S*

For a structural analysis, the IDISPLACEMENTS command can be used to specify initial conditions for the nodal displacement degrees of freedom (dofs), or the generalized coordinates of a reduced-order representation of the displacement field. For a time-domain acoustic analysis, this command can be used to specify nodal values of the initial solution by setting DOF# to 8 (see below).

Note 6: For a dynamic simulation based on a hyper reduced projection-based reduced-order model and its associated reduced mesh, a high-dimensional initial displacement condition — from which the corresponding low-dimensional initial condition can be inferred by projection onto the Reduced-Order Basis (ROB) inputted using READMODE — can be specified using this command: only on the nodes attached to the elements of the inputted reduced mesh; and if the high-dimensional initial displacement field is zero at all other nodes of the original mesh. On the other hand, such an initial condition can be specified on all or an arbitrary subset of nodes of the high-dimensional mesh in the same ASCII Input Command Data file containing the RMSHC command, and therefore in the same simulation performed to construct the reduced mesh: in this case, the initial condition for the vector of generalized coordinates is computed offline and outputted in the same output file containing the reduced mesh (see SAMPLMSH in OUTPUT). Furthermore, if for some reason only the trace of the ROB on the degrees of freedom of the reduced mesh is available — for example, when the ROB is randomized — a specified high-dimensional initial displacement condition must be hyper reduced using the RMSHC command.

`NODE#`	Node number where the initial displacement or acoustic field is specified (integer).
`DOF#`	Local identification number of the degree of freedom where the initial displacement or acoustic field is specified (integer).
`VALUE`	Value of the specified initial displacement or acoustic field (real).
`ZERO`	This initializes the entire intital displacement or acoustic field to zero. No other `IDISPLACEMENTS` data has to be entered when this option is selected (characters).

For displacement generalized coordinates, the format of this command is as follows.

`MODAL`	This sub-command keyword (characters) can be used to: Input the initial conditions for the generalized coordinates associated with the ROB chosen for initializing the displacement field. Superpose to the initial conditions specified in the finite element coordinates system additional initial conditions formulated in the generalized coordinates system associated with the ROB chosen for this purpose, subject to any restriction implied by the content of Note 3. An example where no restriction applies is one where `IDISPLACEMENTS` is used to input both modal and non-modal initial displacement conditions, where modal means in this context an initial condition specified for the generalized coordinates associated with a chosen ROB, and non-modal means an initial condition specified for the nodal displacement dofs. An example where a restriction applies, is that where `IDISPLACEMENTS` is used to input modal initial displacement conditions, and IDISP6 is used to input non-modal initial displacement conditions. In the second case, `IDISPLACEMENTS` should be specified only once and the `MODAL` sub-command and its associated data can be inserted either before or after the data set associated with the initial conditions specified in the finite element coordinates system. This option can also be used to perform a "Ping-Pong" analysis (AERO). In all cases, the primal displacement ROB must be inputted in READMODE.
`rob_id`	This parameter is relevant only when the second format of the READMODE command is used to input one or multiple ROBs. In this case, it is an integer number identifying the primal ROB inputted in READMODE to be used to initialize the displacement field (integer).
`MODE#`	Mode ID number (or column number of the ROB identified above) whose generalized coordinate is to be initialized below (integer).
`VALUE`	Value of the specified initial condition (real).

76 INITIAL DISPLACEMENT 6 COLUMNS (IDISP6 completely spelled out) *S*

The IDISP6 command statement is used to specify a nodal displacement type of initial conditions in a different format than that of the IDISPLACEMENTS command. This format is specified below.

$\text{[math]}$	Amplification factor that multiplies each VAL_DOFi value for each node (real).
`NODE#`	Node number where the initial displacement is specified (integer).
`VAL_DOFi#`	Value of the specified initial displacement for the i-th degree of freedom (real).

77 INITIAL OR SEED DISPLACEMENT FOR PITA (IDISP6PITA completely spelled out)

The IDISP6PITA command statement can be used to specify the time-slices' initial or seed displacements for the PITA methodology (see PITA), thus overriding the alternative approach consisting of generating this information by applying the basic time-integrator on the coarse time-grid. It is applicable in both linear and nonlinear settings. Its syntax is similar to that of the IDISP6 (see IDISP6) command except that it can introduce up to as many sets of initial displacements as there are time-slices, one set per time-slice. Each set of initial displacements must be input after the previous one, starting with that corresponding to the first time-slice and continuing in consecutive order. All those time-slices for which a set of seed displacement values is not specified are initialized by the aforementioned alternative approach.

`NUMSLICES`	Number of consecutive time-slices for which seed displacements are specified (integer).
`NODE#`	Node number where the seed displacement is specified (integer).
`VAL_DOFi#`	Value of the seed displacement for the i-th degree of freedom at the beginning of a time-slice (float).

78 INITIAL OR SEED VELOCITY FOR PITA (IVEL6PITA completely spelled out)

The IVEL6PITA command statement can be used to specify the time-slices' initial or seed velocities for the PITA methodology (see PITA), thus overriding the alternative approach consisting of generating this information by applying the basic time-integrator on the coarse time-grid. It is applicable in both linear and nonlinear settings. Its syntax is similar to that of the IDISP6 (see IDISP6) command except that it can introduce up to as many sets of initial velocities as there are time-slices, one set per time-slice. Each set of initial velocities must be input after the previous one, starting with that corresponding to the first time-slice and continuing in consecutive order. All those time-slices for which a set of seed velocity values is not specified are initialized by the aforementioned alternative approach.

`NUMSLICES`	Number of consecutive time-slices for which seed velocities are specified (integer).
`NODE#`	Node number where the seed velocity is specified (integer).
`VAL_DOFi#`	Value of the seed velocity for the i-th degree of freedom at the beginning of a time-slice (float).

79 INITIAL TEMPERATURES *S*

The ITEMPERATURES command can be used to specify initial conditions for the nodal temperature degrees of freedom (dofs) or temperature generalized coordinates of a thermal model.

`NODE#`	Node number where the initial temperature is specified (integer).
`VALUE`	Value of the specified initial temperature (real).

`MODAL`	This sub-command keyword can be used to input the initial conditions for the generalized coordinates associated with the Reduced-Order Basis (ROB) chosen for initializing the temperature field. When this option is used, it must also be specified in DYNAMICS, and the primal temperature Reduced-Order Basis (ROB) must be inputted using READMODE.
`rob_id`	This parameter is relevant only when the second format of the READMODE command is used to input one or multiple ROBs. In this case, it is an integer number identifying the primal ROB inputted in READMODE to be used to initialize the temperature field (integer).
`MODE#`	Mode ID number (or column number of the ROB identified above) whose generalized coordinate is to be initialized below (integer).
`VALUE`	Value of the specified initial condition (real).

80 INITIAL VELOCITIES *S*

For a structural analysis, the IVELOCITIES command can be used to specify initial conditions for the nodal velocity degrees of freedom (dofs), or the generalized coordinates of a reduced-order representation of the velocity field. For a time-domain acoustic analysis, this command can be used to specify nodal values of the initial time-derivative of the solution by setting DOF# to 8 (see below).

Note 1: All degrees of freedom referred to by this command are defined in the nodal degree of freedom reference frames defined at the nodes where these degrees of freedom are attached (see NODES and NFRAMES). By default, the nodal degree of freedom reference frames are the same as the global reference frame.

Note 2: For a dynamic simulation based on a hyper reduced projection-based reduced-order model and its associated reduced mesh, a high-dimensional initial velocity condition — from which the corresponding low-dimensional initial condition can be inferred by projection onto the Reduced-Order Basis (ROB) inputted using READMODE — can be specified using this command: only on the nodes attached to the elements of the inputted reduced mesh; and if the high-dimensional initial velocity field is zero at all other nodes of the original mesh. On the other hand, such an initial condition can be specified on all or an arbitrary subset of nodes of the original mesh in the same ASCII Input Command Data file containing the RMSHC command, and therefore in the same simulation performed to construct the reduced mesh: in this case, the initial condition for the vector of generalized coordinates is computed offline and outputted in the same output file containing the reduced mesh (see SAMPLMSH in OUTPUT). Furthermore, if for some reason only the trace of the ROB on the degrees of freedom of the reduced mesh is available — for example, when the ROB is randomized — a specified high-dimensional initial velocity condition must be hyper reduced using the RMSHC command.

`NODE#`	Node number where the initial velocity is specified (integer).
`DOF#`	Degree of freedom local number where the initial velocity is specified (integer).
`VALUE`	Value of the specified initial temperature (real).

`MODAL`	This sub-command keyword (characters) can be used to: Input the initial conditions for the generalized coordinates associated with the Reduced-Order Basis (ROB) chosen for initializing the velocity field. Superpose to the initial conditions specified in the finite element coordinates system additional initial conditions formulated in the generalized coordinates system associated with the ROB chosen for this purpose. In the second case, `IVELOCITIES` should be specified only once, and the `MODAL` sub-command and its associated data can be inserted either before or after the data set associated with the initial conditions specified in the finite element coordinates system. This option can also be used to perform a "Ping-Pong" analysis (AERO). In all cases, the primal velocity ROB must be inputted using READMODE.
`rob_id`	This parameter is relevant only when the second format of the READMODE command is used to input one or multiple ROBs. In this case, it is an integer number identifying the primal ROB inputted in READMODE to be used to initialize the velocity field (integer).
`MODE#`	Mode ID number (or column number of the ROB identified above) whose generalized coordinate is to be initialized below (integer).
`VALUE`	Value of the specified initial condition (real).

81 INTRUSIVE POLYNOMIAL CHAOS

The INPC command signals to the AERO-S code to perform an intrusive non deterministic analysis using the Polynomial Chaos representation of the solution. It requires that the input file also contains the GROUPS, RANDOM, and STATICS commands and their respective data.

DEG_OUT Degree of the polynomial chaos representation of the solution (integer).

82 LINEAR MATERIAL PROPERTIES *S*

Note 2: Even for a given input format, the interpretation of a data entry can change from one element type to another. For example for the first input format, the main interpretation of some data entries changes when the element type is that of a lumped torsional spring, a torsional spring connector, a linear spring connector, a Timoshenko beam, a thermal element, a rigid translational link, or a rigid rotational link.

Note 3: A non-structural mass is defined here and throughout this User's Reference Manual as a discrete mass that is attributed to an element, and which therefore affects the mass matrix of this element and its contribution to a gravity load. Specifically, it affects only the translational degrees of freedom attached to this element, in the same manner as a discrete mass that is specified for a translational degree of freedom attached to a specified node (see the command DIMASS).

Note 4: For composite elements, this command is not required unless stress and/or strain output is requested. Even in this case, only the total thickness of the element must be specified under this command. Dummy or zero values can be entered for the other properties as their real values should be specified under the COMPOSITE command.

Note 5: The Perfectly Matched Layer (PML) method is supported only by the elements type 95, 96, 98, and 99.

Note 6: Specifying under this command a method for enforcing the constraints associated with joint and/or rigid elements sharing a certain material ID number overrides for these elements the specification under CONSTRAINTS of a default method for enforcing constraints.

MID A E $\text{[math]}$ $\text{[math]}$ h k t P Ta $\text{[math]}$ $\text{[math]}$ Ixx Iyy Izz ymin ymax zmin zmax DAMPING_TYPE $\text{[math]}$ $\text{[math]}$

`MID`	The material id number.
`A`	Cross sectional area for trusses, beams, and lineal thermal elements (float).
`E`	Young's Modulus for all element types (float). However, this field can also be filled by a negative integer in which case it means that Young's Modulus is a function of temperature and is to be determined from the `YMTT` and `TEMPERATURES` commands. In the latter case, the integer specified here points to the id of the Young's modulus-temperature table in the `YMTT` command (negative integer).
$\text{[math]}$	Poisson's ratio for all element types except trusses (float).
$\text{[math]}$	Mass density per unit volume accounting for both structural and non-structural types of mass (see definition in the Notes section above), except in the following situations (float): For a composite or orthotropic shell element (type 15, 1515, 20, and 2020) and when the composite properties are defined using the `COEF` option (see COMPOSITE), this parameter denotes the mass density per unit area and accounts for both structural and non-structural types of mass. For a composite or orthotropic shell element (type 15, 1515, 20, and 2020) and when the composite properties are defined using the `LAYC` option (or a combination of `LAYD` and `LAYMAT`, see COMPOSITE) or the `LAYN` option (or a combination of `LAYO` and `LAYMAT`, see COMPOSITE), and for any other composite shell element (type 8, 88, 16, 73, and 76), this parameter denotes the mass density per unit area of the non-structural type of mass only. In this case, the density associated with the structural type of mass should be specified for each individual material layer using the command COMPOSITE. For nonlinear thermal and fluid-thermal (aerothermal) analysis, the mass density may be a function of temperature. In this case, this parameter should be set to a negative number, the temperature-dependent mass density should be inputted using the command DCTT, and the absolute value of the negative integer inputted here is interpreted by AERO-S to be the ID of the mass density-temperature table inputted using the command DCTT (negative integer).
`h`	Heat convection coefficient (only for boundary convection elements: type 47, 48, and 49 (float)).
`k`	Heat conduction coefficient (float). For nonlinear thermal and fluid-thermal (aerothermal) analysis, this coefficient may be a function of temperature. In this case, this parameter should be set to a negative number, the temperature-dependent heat conduction coefficient should be inputted using the command CCTT, and the absolute value of the negative integer inputted here is interpreted by AERO-S to be the ID of the heat conduction coefficient-temperature table inputted using the command CCTT (negative integer).
`t`	Element thickness (float).
`P`	Perimeter/circumference area for thermal elements (float), or the depth of the boundary where convection occurs when element type 47 is used to model non-lateral boundary convection (float).
`Ta`	Reference temperature (Absolute) of the element (float). WARNING: if this value is different from the nodal temperature of that element (see TEMPERATURES), it creates a thermal loading even in a pure structural analysis.
$\text{[math]}$	Specific heat coefficient in a thermal analysis (float). For nonlinear thermal and fluid-thermal (aerothermal) analysis, this coefficient may be a function of temperature. In this case, this parameter should be set to a negative number, the temperature-dependent specific heat coefficient should be inputted using the command SCTT, and the absolute value of the negative integer inputted here is interpreted by AERO-S to be the ID of the specific heat coefficient-temperature table inputted using the command SCTT (negative integer).
$\text{[math]}$	Coefficient of thermal expansion in either a thermal analysis, or a structural analysis if the specified reference temperature `Ta` is different from the specified nodal temperatures (see TEMPERATURES and THERMOE) (float). In a thermal analysis, this field can also be filled by a negative integer meaning that the coefficient of thermal expansion is a function of temperature and is to be determined from the TETT and TEMPERATURES commands. In this case, the integer specified here points to the id of the coefficient of thermal expansion-temperature table in the TETT command (negative integer).
`Ixx/ss`	For a mechanical analysis (`MECH` under the `DYNAMICS` command), this is the cross-sectional moment of inertia about the local and centroidal x-axis. For an acoustic analysis in the time-domain (`ACOU` under the `DYNAMICS` command), this is the speed of sound in the medium represented by the attribute number.
`Iyy`	Cross-sectional moment of inertia about the local and centroidal principal y-axis.
`Izz`	Cross-sectional moment of inertia about the local and centroidal principal z-axis.
`ymin`	Negative local y-coordinate of the bottom fiber of a beam cross section.
`ymax`	Positive local y-coordinate of the top fiber of a beam cross section.
`zmin`	Negative local z-coordinate of the top fiber of a beam cross section.
`zmax`	Positive local z-coordinate of the top fiber of a beam cross section.
`DAMPING_TYPE`	Optional sub-command keyword to specify a type of damping (characters). Two options are currently available:
`RAYDAMP`	This option specifies a Rayleigh proportional type of damping for structural dynamic (see DYNAMICS) or frequency response (see IMPEDANCE) analysis. In this case, damping is introduced at the element level in the form of a finite element damping matrix $\text{[math]}$ that is constructed as $\text{[math]}$ where $\text{[math]}$ and $\text{[math]}$ denote the element-level mass and stiffness matrices, respectively, and $\text{[math]}$ and $\text{[math]}$ are two real coefficients that are specfied below.
`STRDAMP`	This option specifies a structural type of damping for frequency response analysis (see IMPEDANCE). In this case, damping is introduced in the form of the following modified local (element-level) Young modulus $\text{[math]}$ where $\text{[math]}$ denotes here the element-level Young modulus, the star superscript designates the modified Young modulus, $\text{[math]}$ denotes the pure imaginary number satisfying $\text{[math]}$ , the minus sign in $\text{[math]}$ is due to the convention $\text{[math]}$ (see IMPEDANCE), and $\text{[math]}$ is the Young modulus loss factor. In general, $\text{[math]}$ is a function of the forced frequency $\text{[math]}$ . If in the frequency range of interest $\text{[math]}$ can be represented as a linear function of $\text{[math]}$ — that is, $\text{[math]}$ this linear representation can be specified in the `MATERIAL` command by inputting $\text{[math]}$ and $\text{[math]}$ below and specifying $\text{[math]}$ in IMPEDANCE. Otherwise, an arbitrary variation of the Young modulus loss factor with the frequency can be inputted in the form a lookup table (or curve) using SDETAFT, in which case given a frequency $\text{[math]}$ specified in IMPEDANCE, $\text{[math]}$ is determined by local interpolation.
`RUBDAMP`	This option is supported only for the tetrahedral and hexahedral (brick) solid elements (type = 17, 23, 25, 72, 91, 102, or 103). It specifies a rubber material type of damping for frequency response analysis (see IMPEDANCE). In this case, damping is introduced in the form of the following modified local (element-level) Young modulus and shear modulus $\text{[math]}$ $\text{[math]}$ where $\text{[math]}$ and $\text{[math]}$ denote here the element-level Young modulus and shear modulus, respectively, the star superscript designates the modified moduli, $\text{[math]}$ denotes the pure imaginary number satisfying $\text{[math]}$ , the minus sign in $\text{[math]}$ is due to the convention $\text{[math]}$ (see IMPEDANCE), and $\text{[math]}$ and $\text{[math]}$ are the Young modulus loss factor and shear modulus loss factor, respectively. To specify $\text{[math]}$ , $\text{[math]}$ , $\text{[math]}$ , and $\text{[math]}$ , a distinction should be made between two cases: The particular case where all of $\text{[math]}$ , $\text{[math]}$ , $\text{[math]}$ , and $\text{[math]}$ are frequency independent. In this case, and only in this case, $\text{[math]}$ should be specified as usual, Poisson's ratio $\text{[math]}$ should be also specified as usual, $\text{[math]}$ is deduced by AERO-S from $\text{[math]}$ and $\text{[math]}$ , and $\text{[math]}$ and $\text{[math]}$ should be inputted in $\text{[math]}$ and $\text{[math]}$ , respectively (see below). The general case where some or all of the parameters $\text{[math]}$ , $\text{[math]}$ , $\text{[math]}$ , and $\text{[math]}$ are functions of the forced frequency $\text{[math]}$ . In this case, arbitrary variations of these properties with the frequency (including a constant behavior, if any) must be inputted in the form of a lookup table that is defined in RUBDAFT and assigned using the parameter $\text{[math]}$ (see below); then, given a frequency $\text{[math]}$ specified under IMPEDANCE, $\text{[math]}$ , $\text{[math]}$ , $\text{[math]}$ , $\text{[math]}$ are determined by AERO-S by local interpolation.
$\text{[math]}$	If `DAMPING_TYPE` is set to `RAYDAMP`, $\text{[math]}$ specifies the Rayleigh damping stiffness coefficient (real) — that is, the stiffness coefficient in the Rayleigh proportional damping matrix $\text{[math]}$ for the material identified by `MID`. In the nonlinear case, this coefficient is assigned at each iteration to the linearized stiffness matrix and the product of these two quantities, which varies with the nonlinear iterations, constitutes the stiffness contribution to the damping term. In a structural dynamic analysis, this value overrides for the material identified by `MID` any value of the Rayleigh damping stiffness coefficient specified under DYNAMICS. In any analysis performed using the IMPEDANCE command, this value overrides for the material identified by `MID` any value of the Rayleigh damping stiffness coefficient specified under IMPEDANCE. On the other hand, if `DAMPING_TYPE` is set to `STRDAMP`, $\text{[math]}$ has a different meaning that pertains to the loss factor $\text{[math]}$ briefly discussed above. In this case, if the loss factor of the material identified by `MID` is to be represented as a linear function of the frequency $\text{[math]}$ of the form $\text{[math]}$ (see above), then $\text{[math]}$ and should be specified as such. However, if the loss factor is to be interpolated using an arbitrary lookup table defined in SDETAFT, $\text{[math]}$ should be set to the negative integer value `-curve_id` (integer), where `curve_id` is the "id number" of the relevant lookup table defined in SDETAFT using the sub-command keyword `CURVE`. In that case, $\text{[math]}$ (see below) should be simply ignored. If `DAMPING_TYPE` is set to `RUBDAMP` however, then: If all of the parameters $\text{[math]}$ , $\text{[math]}$ , $\text{[math]}$ , and $\text{[math]}$ are frequency independent, $\text{[math]}$ . Otherwise — that is, if $\text{[math]}$ , $\text{[math]}$ , $\text{[math]}$ , or $\text{[math]}$ is a frequency dependent parameter — $\text{[math]}$ should be set to the negative integer value `-table_id` (integer), where `table_id` is the "id number" of the relevant lookup table defined in RUBDAFT using the sub-command keyword `TABLE` and containing the arbitrary variations of $\text{[math]}$ , $\text{[math]}$ , $\text{[math]}$ , and $\text{[math]}$ with the frequency $\text{[math]}$ (including a constant behavior of some of these parameters, if any).
$\text{[math]}$	If `DAMPING_TYPE` is set to `RAYDAMP`, $\text{[math]}$ specifies the Rayleigh damping mass coefficient (real) — that is, the mass coefficient in the Rayleigh proportional damping matrix $\text{[math]}$ (real) for the material identified by `MID` (see above). In a structural dynamic analysis, this value overrides for the material identified by `MID` any value of the Rayleigh damping mass coefficient specified under DYNAMICS. In any analysis performed using the IMPEDANCE command, this value overrides for the material identified by `MID` any value of the Rayleigh damping mass coefficient specified under IMPEDANCE. On the other hand, if `DAMPING_TYPE` is set to `STRDAMP`, $\text{[math]}$ has a different meaning that pertains to the loss factor $\text{[math]}$ briefly discussed above. In this case, if the loss factor of the material identified by `MID` is to be represented as a linear function of the frequency $\text{[math]}$ of the form $\text{[math]}$ (see above), then $\text{[math]}$ and should be specified as such. However, if the loss factor is to be interpolated using an arbitrary lookup table defined in SDETAFT, $\text{[math]}$ (see above) should be set to the negative integer value `-curve_id` (integer), where `curve_id` is the "id number" of the relevant lookup table defined in SDETAFT using the sub-command keyword `CURVE`, and $\text{[math]}$ should be simply ignored. If `DAMPING_TYPE` is set to `RUBDAMP` however, then: If all of the parameters $\text{[math]}$ , $\text{[math]}$ , $\text{[math]}$ , and $\text{[math]}$ are frequency independent, $\text{[math]}$ . Otherwise — that is, if $\text{[math]}$ , $\text{[math]}$ , $\text{[math]}$ , or $\text{[math]}$ is a frequency dependent parameter — $\text{[math]}$ is ignored.

MID Kx Ky Kz lx1 ly1 lz1 lx2 ly2 lz2 lx3 ly3 lz3 DAMPING

\text{[math]}

`MID`	The material id number from element attribute table.
`Kx`	Torsional/Translational spring constant along local x-axis (float).
`Ky`	Torsional/Translational spring constant along local y-axis (float).
`Kz`	Torsional/Translational spring constant along local z-axis (float).
`lx1` `ly1` `lz1`	The first axis of the local frame expressed in the global frame (floats).
`lx2` `ly2` `lz2`	The first axis of the local frame expressed in the global frame (floats).
`lx3` `ly3` `lz3`	The first axis of the local frame expressed in the global frame (floats).
`DAMPING`	Sub-command keyword for specifying the Rayleigh damping stiffness coefficient (characters).
$\text{[math]}$	Rayleigh damping stiffness coefficient (real).

`MID`	The material ID number from the element attribute table (integer).
`MASS`	Keyword indicating that the following data entries specify the properties of a discrete mass and inertia.
`m`	Discrete mass (real).
`Ixx`	`Ixx` component of the discrete inertia tensor (real). This tensor is defined in the element frame if one is speficied under EFRAMES. Otherwise, it is defined in the global frame.
`Iyy`	`Iyy` component of the discrete inertia tensor (real). This tensor is defined in the element frame if one is speficied under EFRAMES. Otherwise, it is defined in the global frame.
`Izz`	`Izz` component of the discrete inertia tensor (real). This tensor is defined in the element frame if one is speficied under EFRAMES. Otherwise, it is defined in the global frame.
`Ixy`	`Ixy` component of the discrete inertia tensor (real). This tensor is defined in the element frame if one is speficied under EFRAMES. Otherwise, it is defined in the global frame.
`Ixz`	`Ixz` component of the discrete inertia tensor (real). This tensor is defined in the element frame if one is speficied under EFRAMES. Otherwise, it is defined in the global frame.
`Iyz`	`Iyz` component of the discrete inertia tensor (real). This tensor is defined in the element frame if one is speficied under EFRAMES. Otherwise, it is defined in the global frame.
`cx`	`x` component of the offset vector from the node to the center of the discrete mass (real).
`cy`	`y` component of the offset vector from the node to the center of the discrete mass (real).
`cz`	`z` component of the offset vector from the node to the center of the discrete mass (real).

MID A E $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ C1 P Ta $\text{[math]}$ $\text{[math]}$ Ixx Iyy Izz ymin ymax zmin zmax DAMPING_TYPE $\text{[math]}$ $\text{[math]}$

`MID`	The material id number from element attribute table.
`A`	Cross sectional area (float).
`E`	Young's Modulus (float).
$\text{[math]}$	Poisson's ratio (float).
$\text{[math]}$	Mass density per unit volume (float).
$\text{[math]}$	Shear deflection constant associated with $\text{[math]}$ (float). This shear deflection constant is defined as the ratio of the cross-sectional area and the effective shear area associated with the local $\text{[math]}$ axis specified in EFRAMES. This effective shear area is defined in chapter 12 of Timoshenko and Goodier, “Theory of Elasticity”. Note that this shear deflection constant is the inverse of the shear coefficient defined in https://en.wikipedia.org/wiki/Timoshenko_beam_theory#Shear_coefficient and used by other finite element codes such as NASTRAN.
$\text{[math]}$	Shear deflection constant associated with $\text{[math]}$ (float). This shear deflection constant is defined as the ratio of the cross-sectional area and the effective shear area associated with the local $\text{[math]}$ axis specified in EFRAMES. This effective shear area is defined in chapter 12 of Timoshenko and Goodier, “Theory of Elasticity”. Note that this shear deflection constant is the inverse of the shear coefficient defined in https://en.wikipedia.org/wiki/Timoshenko_beam_theory#Shear_coefficient and used by other finite element codes such as NASTRAN.
`C1`	Non-uniform torsion constant (float).
`P`	Not Applicable
`Ta`	Not Applicable
$\text{[math]}$	Not Applicable
$\text{[math]}$	Not Applicable
`Ixx`	Cross-sectional moment of inertia about the local and centroidal x-axis
`Iyy`	Cross-sectional moment of inertia about the local and centroidal principal y-axis.
`Izz`	Cross-sectional moment of inertia about the local and centroidal principal z-axis.
`ymin`	Negative local y-coordinate of the bottom fiber of a beam cross section.
`ymax`	Positive local y-coordinate of the top fiber of a beam cross section.
`zmin`	Negative local z-coordinate of the top fiber of a beam cross section.
`zmax`	Positive local z-coordinate of the top fiber of a beam cross section.
`DAMPING_TYPE`	Optional sub-command keyword to specify a type of damping (characters). Two options are currently available:
`RAYDAMP`	This option specifies a Rayleigh proportional type of damping for structural dynamic (see DYNAMICS) or frequency response (see IMPEDANCE) analysis (see above for further details).
`STRDAMP`	This option specifies a structural type of damping for frequency response analysis (see IMPEDANCE) (see above for further details).
$\text{[math]}$	If `DAMPING_TYPE` is set to `RAYDAMP`, $\text{[math]}$ specifies the Rayleigh damping stiffness coefficient (real). On the other hand, if `DAMPING_TYPE` is set to `STRDAMP`, then: If the loss factor of the material identified by `MID` is to be represented as a linear function of the frequency $\text{[math]}$ of the form $\text{[math]}$ (see above), then $\text{[math]}$ and should be specified as such. However, if the loss factor is to be interpolated using an arbitrary lookup table defined in SDETAFT, $\text{[math]}$ should be set to the negative integer value `-curve_id` (integer), where `curve_id` is the "id number" of the relevant lookup table defined in SDETAFT using the sub-command keyword `CURVE`. In that case, $\text{[math]}$ (see below) should be simply ignored.
$\text{[math]}$	If `DAMPING_TYPE` is set to `RAYDAMP`, $\text{[math]}$ specifies the Rayleigh damping mass coefficient (real). On the other hand, if `DAMPING_TYPE` is set to `STRDAMP`, then: If the loss factor of the material identified by `MID` is to be represented as a linear function of the frequency $\text{[math]}$ of the form $\text{[math]}$ (see above), then $\text{[math]}$ and should be specified as such. However, if the loss factor is to be interpolated using an arbitrary lookup table defined in SDETAFT, $\text{[math]}$ (see above) should be set to the negative integer value `-curve_id` (integer), where `curve_id` is the "id number" of the relevant lookup table defined in SDETAFT using the sub-command keyword `CURVE`, and $\text{[math]}$ should be simply ignored.

MID x y z dum dum dum dum dum dum dum dum dum dum dum dum dum dum dum

`MID`	The material id number from element attribute table.
`x`	Any nonzero value implies a rigid motion in this direction (float).
`y`	Any nonzero value implies a rigid motion in this direction (float).
`z`	Any nonzero value implies a rigid motion in this direction (float).
`dum`	Any dummy value (float).

`MID`	The material ID number from the element attribute table (integer).
`CONMAT`	Keyword indicating that the following data entries specify the method chosen for enforcing the constraints associated with the joint, rigid, or constraint function elements sharing the material id number `MID` (characters).
`MODE`	Optional sub-command keyword to specify whether a constraint is of the equality or inequality type (characters).
`mode_v`	Setting this parameter to 0, which is its default value, specifies that the contraint `CONSTRAINT#` is of the equality type. Setting it to 1 specifies that it is of the inequality type (integer).
`CONSTRAINT_METHOD`	Optional parameter which specifies the method for enforcing the constraints associated with the joint, rigid, or constraint function elements sharing the material ID number `MID` (characters or characters and real). The default method is set in CONSTRAINTS and used whenever this entry is omitted.
`multipliers`	The Lagrange multiplier method.
`elimination`	The elimination method.
`penalty` `beta`	The penalty method. The real-valued parameter `beta` should be a large positive number, typically of the order of $\text{[math]}$ (no default value is provided).
`augmented` `beta`	The augmented Lagrangian method. The real-valued parameter `beta` should be a large positive number, typically of the order of $\text{[math]}$ (no default value is provided).

`MID`	The material id number from element attribute table.
`CONMAT`	Keyword indicating that the following data entries specify the method chosen for enforcing the constraints associated with the joint, rigid, or constraint function elements sharing the material id number `MID` (characters).
`CONSTRAINT_METHOD`	Optional parameter which specifies the method for enforcing the constraints associated with the joint, rigid, or constraint function elements sharing the material id number `MID` (characters or characters and real). The default method is set in CONSTRAINTS and used whenever this entry is omitted.
`multipliers`	The Lagrange multiplier method.
`elimination`	The elimination method.
`penalty` `beta`	The penalty method. The real-valued parameter `beta` should be a large positive number, typically of the order of $\text{[math]}$ (no default value is provided).
`augmented` `beta`	The augmented Lagrangian method. The real-valued parameter `beta` should be a large positive number, typically of the order of $\text{[math]}$ (no default value is provided).
`MASS`	Optional keyword indicating that the rigid elements with eltyp = 65, 66, 70, 73, or 76 sharing the material id number `MID` are to be attributed an element level (lumped or consistent) mass matrix computed as in the case of flexible elements, using the following data entries (characters).
`DENSITY`	Optional parameter which specifies the density for the rigid elements with eltyp = 65, 66, 70, 73, or 76 sharing the material id number `MID` (real).
`GEOPARA`	Optional parameter which specifies the cross sectional area for those rigid truss (eltyp = 65) and beam (eltyp = 66) elements, or the thickness for those rigid shell (eltyp = 73 or 76) elements sharing the material id number `MID` (real).

`MID`	The material id number from element attribute table.
`SPRINGMAT`	Keyword indicating that the following data entry specifies the stiffness constant of the nonlinear spring elements sharing the material id number `MID` (characters).
`k`	Stiffness constant of the nonlinear spring elements sharing the material id number `MID` (real).
`FREEPLAY`	Optional keyword indicating that the following data entry specifies the freeplay parameter for the spring elements of type 203, 204, or 205 sharing the material ID number `MID` (characters). For each such spring element, freeplay is modeled using this parameter as follows: $\text{[math]}$ $\text{[math]}$ where $\text{[math]}$ is the stiffness coefficient `k` of the spring, and $\text{[math]}$ is its displacement. In a linear dynamic analysis, the freeplay-induced forces and moments are interpreted as configuration-dependent and automatically treated as piecewise constant (see `PIECEWISE` in STATICS).
`freeplay_ul`	Freeplay upper displacement limit which should be specified in the unit of length chosen for the computational model.

MID CONMAT [CONSTRAINT_METHOD] SPRINGMAT k1 k2 k3 FREEPLAY freeplay_ll1 freeplay_ul1 factor_lz1 factor_dz1 factor_uz1 freeplay_ll2 freeplay_ul2 factor_lz2 factor_dz2 factor_uz2 freeplay_ll3 freeplay_ul3 factor_lz3 factor_dz3 factor_uz3

`MID`	The material id number from element attribute table.
`CONMAT`	Keyword indicating that the following data entries specify the method chosen for enforcing the constraints associated with the joint spring combination elements sharing the material id number `MID` (characters).
`CONSTRAINT_METHOD`	Optional parameter which specifies the method for enforcing the constraints associated with the joint spring combination elements sharing the material id number `MID` (characters or characters and real). The default method is set in CONSTRAINTS and used whenever this entry is omitted.
`multipliers`	The Lagrange multiplier method.
`elimination`	The elimination method.
`penalty` `beta`	The penalty method. The real-valued parameter `beta` should be a large positive number, typically of the order of $\text{[math]}$ (no default value is provided).
`augmented` `beta`	The augmented Lagrangian method. The real-valued parameter `beta` should be a large positive number, typically of the order of $\text{[math]}$ (no default value is provided).
`SPRINGMAT`	Keyword indicating that the following data entry specifies the stiffness coefficient of the joint spring combination elements sharing the material ID number `MID` (characters).
`k1` `k2` `k3`	Stiffness constants of the joint spring combination elements sharing the material ID number `MID` (real). More specifically `k1` is the stiffness of the first embedded spring, `k2` that of the second embedded spring when applicable, and `k3` that of the third embedded spring when applicable.
`FREEPLAY`	Keyword indicating that the following data entries specify the freeplay parameters for the springs embedded in the joint spring combination elements sharing the material ID number `MID` (characters). For each embedded spring $\text{[math]}$ (`i` = 1, 2, or 3), freeplay is modeled using 5 parameters: A pair of lower and upper deflection limits `freeplay_lli` and `freeplay_uli` for defining the "dead zone" $\text{[math]}$ . Three factors `factor_lzi`, `factor_dzi`, and `factor_uzi` for defining the effective stiffness coefficient $\text{[math]}$ as follows $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ where $\text{[math]}$ is the stiffness coefficient `ki` of the embedded spring $\text{[math]}$ , the deflection $\text{[math]}$ of this spring is a rotation in the case of a rotational spring, and a displacement in the case of a translational spring. Note however that: Currently, freeplay is supported only for the element type 323 which has a single embedded spring with a stiffness coefficient `k1`. In a linear dynamic analysis, the freeplay-induced forces and moments are interpreted as configuration-dependent and automatically treated as piecewise constant (see `PIECEWISE` in STATICS).
`freeplay_ll1` (`freeplay_ll2`, or `freeplay_ll3`)	Freeplay deflection lower limit for the first (second, or third) embedded spring. For a torsional spring, the deflection corresponds to the rotation associated with this spring, in which case this parameter should be specified in radians. For a translational spring, the deflection corresponds to the displacement associated with this spring, in which case this parameter should be specified in the unit of length chosen for the computational model.
`freeplay_ul1` (`freeplay_ul2`, or `freeplay_ul3`)	Freeplay deflection upper limit for the first (second, or third) embedded spring. For a torsional spring, the deflection corresponds to the rotation associated with this spring, in which case this parameter should be specified in radians (real). For a translational spring, the deflection corresponds to the displacement associated with this spring, in which case this parameter should be specified in the unit of length chosen for the computational model.
`factor_lz1` (`factor_lz2`, or `factor_lz3`)	Freeplay correction factor for the stiffness coefficient `k1` (`k2`, or `k3`) for $\text{[math]}$ ( $\text{[math]}$ , or $\text{[math]}$ ), where the deflection $\text{[math]}$ ( $\text{[math]}$ , or $\text{[math]}$ ) is a rotation in the case of a rotational spring, and a displacement in the case of a translational spring.
`factor_dz1` (`factor_dz2`, or `factor_dz3`)	Freeplay correction factor for the stiffness coefficient `k1` (`k2`, or `k3`) for $\text{[math]}$ ( $\text{[math]}$ , or $\text{[math]}$ ), where the deflection $\text{[math]}$ ( $\text{[math]}$ , or $\text{[math]}$ ) is a rotation in the case of a rotational spring, and a displacement in the case of a translational spring.
`factor_uz1` (`factor_uz2`, or `factor_uz3`)	Freeplay correction factor for the stiffness coefficient `k1` (`k2`, or `k3`) for $\text{[math]}$ ( $\text{[math]}$ , or $\text{[math]}$ ), where the deflection $\text{[math]}$ ( $\text{[math]}$ , or $\text{[math]}$ ) is a rotation in the case of a rotational spring, and a displacement in the case of a translational spring.

MID CONMAT [CONSTRAINT_METHOD] FUNCTION_TYPE SCALE_FACTOR SHIFT

\text{[math]}

\text{[math]}

\text{[math]}

\text{[math]}

SPRINGMAT

\text{[math]}

`MID`	The material id number from element attribute table.
`CONMAT`	Keyword indicating that the following data entries specify the method chosen for enforcing the constraints also fixed the items belowassociated with the revolute or primsatic joint-with-driver or joint-with-actuator elements sharing the material id number `MID` (characters).
`CONSTRAINT_METHOD`	Optional parameter which specifies the method for enforcing the constraints associated with the revolute or prismatic joint-with-driver or joint-with-actuator elements sharing the material id number `MID` (character or characters and real). The default method is set in CONSTRAINTS and used whenever this entry is omitted.
`multipliers`	The Lagrange multiplier method.
`elimination`	The elimination method.
`penalty` `beta`	The penalty method. The real-valued parameter `beta` should be a large positive number, typically of the order of $\text{[math]}$ (no default value is provided).
`augmented` `beta`	The augmented Lagrangian method. The real-valued parameter `beta` should be a large positive number, typically of the order of $\text{[math]}$ (no default value is provided).
`FUNCTION_TYPE`	Type of the relative rotation/applied moment/relative translation/applied force prescribed by the revolute joint-with-driver/revolute joint-with-actuator/prismatic joint-with-driver/prismatic joint-with-actuator elements sharing the material id number `MID` (characters). There are five types to choose from:
`SINE`	Sets $\text{[math]}$ / $\text{[math]}$ / $\text{[math]}$ / $\text{[math]}$ to a sinusoidal relative rotation/applied moment/relative translation/applied force partially described by $\text{[math]}$ , where $\text{[math]}$ and $\text{[math]}$ are two parameters specified below.
`RAMP`	Sets $\text{[math]}$ / $\text{[math]}$ / $\text{[math]}$ / $\text{[math]}$ to a time-dependent relative rotation/applied moment/relative translation/applied force partially described by a bounded ramp function of the form $\text{[math]}$ where $\text{[math]}$ and $\text{[math]}$ are two parameters specified below.
`TRIA`	Sets $\text{[math]}$ / $\text{[math]}$ / $\text{[math]}$ / $\text{[math]}$ to a time-dependent relative rotation/applied moment/relative translation/applied force partially described by a triangular (hat) function of the form $\text{[math]}$ where $\text{[math]}$ , $\text{[math]}$ and $\text{[math]}$ are three parameters specified below.
`TRAP`	Sets $\text{[math]}$ / $\text{[math]}$ / $\text{[math]}$ to a time-dependent relative rotation/applied moment/relative translation/applied force partially described by a trapezoidal function of the form $\text{[math]}$ where $\text{[math]}$ , $\text{[math]}$ , $\text{[math]}$ and $\text{[math]}$ are four parameters specified below.
`SSHA`	Sets $\text{[math]}$ / $\text{[math]}$ / $\text{[math]}$ / $\text{[math]}$ to a time-dependent relative rotation/applied moment/relative translation/applied force partially described by an S-shaped function of the form $\text{[math]}$ where $\text{[math]}$ , $\text{[math]}$ and $\text{[math]}$ are three parameters specified below.
`SCALE_FACTOR`	Constant amplification factor (real).
`SHIFT`	Constant shift (real).
$\text{[math]}$	Time parameter (real).
$\text{[math]}$	Time parameter (real).
$\text{[math]}$	Time parameter (real).
$\text{[math]}$	Time parameter (real).
`SPRINGMAT`	Keyword indicating that the following data entry specifies the stiffness constant of the revolute or prismatic joint-with-actuator elements sharing the material id number `MID` (characters).
$\text{[math]}$	Stiffness constant of the revolute or prismatic joint-with-actuator elements sharing the material id number `MID` (real).

MID THRMAT A $\text{[math]}$ $\text{[math]}$ h/ $\text{[math]}$ $\text{[math]}$ k t P Tr

`MID`	The material id number from element attribute table.
`THRMAT`	keyword that specifies that the following data entries are associated with thermal elements.
`A`	Cross sectional area for lineal thermal elements (float).
$\text{[math]}$	Mass density per unit volume (float).
$\text{[math]}$	Specific heat coefficient (float).
`h`/ $\text{[math]}$	Heat convection coefficient for a heat convection or bulk fluid thermal element, or transfer factor for a heat radiation element (float). When radiation is exchanged between two bodies $\text{[math]}$ (identified here by this value of `MID`) and $\text{[math]}$ (any other body), the transfer factor $\text{[math]}$ depends on the emittances of both bodies as well as the geometrical view. In the special case of a gray object in a large environment — that is, when $\text{[math]}$ represents a smaller body and $\text{[math]}$ a larger isothermal environment (for example, the atmosphere at some temperature) — $\text{[math]}$ becomes the emissivity $\text{[math]}$ of the first body. In this case, $\text{[math]}$ if $\text{[math]}$ is furthermore a black body.
$\text{[math]}$	Stefan's constant, also known as the Stefan-Boltzmann constant (in SI units, $\text{[math]}$ Js $\text{[math]}$ m $\text{[math]}$ K $\text{[math]}$ ) (float).
`k`	Heat conduction coefficient (float).
`t`	Thickness of a (two-dimensional) thermal element (float).
`P`	Perimeter/circumference area for thermal elements (float), or depth of the boundary where convection (radiation) occurs when element type 47 (56) is used to model non-lateral boundary convection (radiation) (float).
`Tr`	For a heat radiation element, reference temperature of the enclosure receiving the radiation (float).

MID AMAT $\text{[math]}$ $\text{[math]}$ pml_type $\text{[math]}$ pmlx1 pmlx2 pmly1 pmly2 pmlz1 pmlz2

MID AMAT $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ pml_type $\text{[math]}$ pmlx1 pmlx2 pmly1 pmly2 pmlz1 pmlz2

`MID`	The material id number from element attribute table.
`AMAT`	Keyword that specifies that the following data entries are associated with acoustic fluid elements.
$\text{[math]}$	Speed of sound in the material identified by `MID` (float).
$\text{[math]}$	Real part of the speed of sound in the material identified by `MID` (float).
$\text{[math]}$	Imaginary part of the speed of sound in the material identified by `MID` (float).
$\text{[math]}$	Density (mass per unit volume) of the material identified by `MID` (float).
`pml_type`	Type of PML (Perfectly Matched Layer) (integer).
	`pml_type` = 1 designates a box PML. In this case the PML elements are assumed to be in the region defined by `pmlx1` < x < `pmlx2`, -`pmlx2` < x < -`pmlx1`, `pmly1` < y < `pmly2`, -`pmly2` < y < -`pmly1`, `pmlz1` < z < `pmlz2`, and -`pmlz2` < z < -`pmlz1`.
	`pml_type` = 2 designates a spherical PML. In this case the PML elements are assumed to be in the region defined by `pmlx1` < r < `pmlx2`, where r = sqrt(xx+yy+z*z).
	`pml_type` = 3 designates a cylindrical PML. In this case the PML elements are assumed to be in the region defined by `pmlx1` < r < `pmlx2`, where r = sqrt(xx+yy), `pmlz1` < z < `pmlz2`, and -`pmlz2` < z < -`pmlz1`.
$\text{[math]}$	PML attenuation parameter (real). Given the speed of sound $\text{[math]}$ specified above, the circular frequency $\text{[math]}$ where $\text{[math]}$ is the frequency specified in IMPEDANCE — and therefore the wavenumber $\text{[math]}$ — the thickness of the PML layer $\text{[math]}$ , and this attenuation parameter $\text{[math]}$ , the PML damps the outgoing waves by the factor $\text{[math]}$ where $\text{[math]}$ . The recommended value for $\text{[math]}$ is $\text{[math]}$ . Note that the mesh within the PML must be designed so that it properly resolves the decaying solution. To this effect, also note that in practice, using two cubic elements through the thickness of the PML is sufficient to resolve a decaying solution characterized by a damping factor $\text{[math]}$ — that is, a solution that decays exponentially within the PML, from a relative amplitude of 1 to a relative amplitude of 0.001.
`pmlx1`	PML geometrical parameter (see above) (real).
`pmlx2`	PML geometrical parameter (see above) (real).
`pmly1`	PML geometrical parameter (see above) (real).
`pmly2`	PML geometrical parameter (see above) (real).
`pmlz1`	PML geometrical parameter (see above) (real).
`pmlz2`	PML geometrical parameter (see above) (real).

MID FABMAT type E $\text{[math]}$ A $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ h d $\text{[math]}$ $\text{[math]}$ $\text{[math]}$

`MID`	The material id number from element attribute table (integer).
`FABMAT`	Keyword specifying that the following data entries are associated with fabric elements (characters).
`type`	Type of fabric material (integer). If `type` = 1, the fabric properties are automatically determined by AERO-S using a micro-scale computation. If `type` = 2, they are determined using Gaussian distribution.
`E`	If `type` = 1, this is Young's modulus for the fibrils that make up the yarn (float). If `type = 2`, it is the mean value of Young's modulus for the yarn.
$\text{[math]}$	Mass density per unit volume of the fibril/yarn (float).
`A`	Cross sectional area of the entire yarn element (float).
$\text{[math]}$	If `type` = 1, this is the breaking stretch ( $\text{[math]}$ ) of the fibrils (float). If `type = 2`, it is the stretch level at which the yarn begins to damage.
$\text{[math]}$	Stretch level at which the entire yarn has failed (i.e. the stress response is approximately zero) (float).
$\text{[math]}$	If `type` = 1, this is the initial guess for the parameter controlling the damage rate of the yarn; its actual value is positive and determined by Newton's method (float). If `type = 2`, it is the slope of the assumed linear variation of the damage parameter with Young's modulus.
`h`	If `type` = 1, this is the length of an unstretched yarn (initial length of the truss element) (float). If `type = 2`, it is the value of the damage parameter for a zero Young's modulus.
`d`	If `type` = 1, this is the standard deviation for the inclination distance of the fibrils (misalignment of the fibrils) (float). If `type = 2`, it is the standard deviation associated with the assumed Gaussian distribution of Young's modulus.
$\text{[math]}$	If `type` = 1, this parameter is set to 0 and ignored (float). If `type = 2`, it is the standard deviation associated with the assumed Gaussian distribution of the damage parameter.
$\text{[math]}$	If `type` = 1, this is the maximum number of Newton iterations for fitting the damage parameter $\text{[math]}$ to micro-scale data (integer). If `type = 2`, this parameter is ignored.
$\text{[math]}$	If `type` = 1, this is the number of fibers in a typical yarn (integer). If `type = 2`, this parameter is ignored.

83 LINEAR MULTIPOINT CONSTRAINTS FOR MECHANICAL ANALYSIS

The LMPC command can be used to specify a set of linear multipoint constraint equations for an otherwise linear or nonlinear (see NONLINEAR) analysis. These constraints equations can be of the form

where

\text{[math]}

is a constant coefficient and

\text{[math]}

denotes a degree of freedom of the structural model. There is no limitation on the number of multipoint constraints, or number of degrees of freedom related by the same constraint equation.

Note 2: Whereas the constraints specified under this command must be linear, the degrees of freedom

\text{[math]}

can be governed by nonlinear equations of equilibrium. Therefore, this command is also supported for linear analysis with geometric stiffening due to prestress (see GEPS), and NONLINEAR analysis. It is noted however that for linear analysis using GEPS, linear multipoint constraints involving rotational degrees of freedom may be violated by the solution computed by AERO-S if the initial displacement field underlying the prestress contains large rotations.

Note 3: The Lagrange multiplier method for enforcing the constraints associated with this command is supported only by the FETI-DP family of iterative solvers, the GMRES solver, and the sparse direct solvers SPOOLES and MUMPS (with pivoting enabled), and in all but explicit dynamic analyses (see STATICS).

Note 4: For time-dependent problems, the specified initial conditions must verify the specified linear multipoint constraints.

CONSTRAINT# RHS [MODE] [mode_v] CONSTRAINT_METHOD
NODE# DOF# COEFF
.
.
NODE# DOF# COEFF

`CONSTRAINT#`	This corresponds to the constraint equation number `i` (integer).
`RHS`	This is the right-hand side $\text{[math]}$ of the `i`-th constraint equation (real).
`MODE`	Optional sub-command keyword to specify whether a constraint is of the equality or inequality type (characters).
`mode_v`	Setting this parameter to 0, which is its default value, specifies that the contraint `CONSTRAINT#` is of the equality type. Setting it to 1 specifies that it is of the inequality type (integer).
`CONSTRAINT_METHOD`	This is the method for enforcing the constraint (characters). The default method is set in CONSTRAINTS and used whenever this entry is omitted.
`multipliers`	The Lagrange multiplier method.
`elimination`	The elimination method.
`penalty` [`beta`]	The penalty method. The parameter `beta` should be a large positive number, typically of the order of $\text{[math]}$ (no default value is provided).
`NODE#`	This is the number of the node contributing the coefficient $\text{[math]}$ of the `i`-th constraint equation (integer).
`DOF#`	This is the local number of the degree of freedom at the node specified above contributing the coefficient $\text{[math]}$ of the `i`-th constraint equation (integer).
`COEFF`	This is the coefficient $\text{[math]}$ of the `i`-th constraint equation (real).

84 LOAD

The LOAD command statement is used to inform AERO-S where the user defined subroutines for user defined forces and/or displacements and/or control are located. An example input file using the LOAD command can be found in FEM.d/fem_examples/Control.d

pathandfilename Specifies between quotes “ ” the path and filename of the LOAD file. The extension of this file must be “.so”.

85 LOADCASE DEFINITION

The LOADCASE command can be used to define one or more "load" cases. Each "load" case is defined as a linear combination of "load" sets. Defining no "load" case is equivalent to defining a load case 0 which combines the "load" set 0 and all "loads" generated by the commands which do not support the "load" set construct (LOADSET_ID). Note also that any "load" generated by a command which does not support the "load" set construct (LOADSET_ID) is automatically added to every "load" case defined herein.

`LOADCASE_ID`	Optional non-negative integer which uniquely identifies a "load" case. The default value is 0. For static analysis, multiple "load" cases can be defined by repeating this command in the same input file using different values for `LOADCASE_ID` and different data. For dynamic analysis, only one "load" case can be defined and must be attributed the identifier 0.
`LOADSET_ID_1`	Integer identifying a "load" set.
`COEFF_1`	For static and dynamic analyses, this parameter is a real coefficient that can be used to amplify the "load" set identified by `LOADSET_ID_1` (real). For dynamic analysis, this parameter can also consist of the keyword `MFTT` or `HFTT` followed by an integer identifying a `TABLE_ID` defined in MFTT or HFTT. In this case, the amplification factor for the "load" set identified by `LOADSET_ID_1` is the time-dependent function defined by `MFTT`[`TABLE_ID`] or `HFTT`[`TABLE_ID`].

86 LUMPED

By default, AERO-S computes all element mass matrices and gravity (see GRAVITY) loads by a consistent approach, except for explicit dynamic computations (see DYNAMICS), in which case AERO-S always uses a lumped approach for this purpose. If a consistent mass matrix is not available for a particular element (see TOPOLOGY), then AERO-S uses in all cases a lumped mass matrix and gravity load for that element.

Alternatively, this command can be used to instruct AERO-S to compute all element mass matrices and gravity loads by a lumping method.

87 MASS EVALUATION

The MASS command statement is used to signal that the user would like that the total mass of the structural system be computed. The result is output on the screen by FEM. In addition to the total mass of the structure, the center of gravity (cg), the center of volume, and the closest node to the cg are also computed and printed on the screen.

88 MATERIAL LAW

Because the MATERIAL command can be used to input the parameters of a linear elastic material law, the MATLAW and MATUSAGE commands should be used primarily for defining and assigning nonlinear material laws. To this end, it is noted that by default, the following material law is assigned by AERO-S to an element of a computational structural model:

Note 2: In the presence of the NONLINEAR command in the ASCII Input Command Data file, the material laws and properties specified under this command and assigned using MATUSAGE take precedence over those inputted using MATERIAL, when a conflict arises.

Note 3: In the absence of the MATLAW command but presence of the NONLINEAR command in the ASCII Input Command Data file:

Note 4: In the absence of both NONLINEAR and MATLAW commands in the ASCII Input Command Data file, the linear elastic material law with infinitesimal strains is assigned by default to all elements of the computational structural model.

Note 5: The various pre-defined material laws that can be specified using this command are supported by different structural and solid mechanics elements (see TOPOLOGY) as follows:

Note 6: The element deletion method is supported only for nonlinear explicit dynamic computations. In such computations, the mass matrix is lumped. For this reason, and because no node is deleted when an element is deleted from the finite element model, neither the mass matrix nor a gravity load is affected by such an event, and mass is conserved.

Note 7: Anisotropic material laws defined using this command (including user-defined and pre-defined materials such as FabricMat, FabricMap, and TorchMat) are typically defined using a local material frame of reference specified using the CFRAMES command.

WARNING: for formatting issues pertaining to this User's Reference Manual only, the data associated with some pre-defined material laws has been described below on separate lines; when preparing an AERO-S ASCII Input Command Data file however, this data should be specified on a single line.

READ MATERIAL_NAME <pathandfilename>
MATERIAL_ID MATERIAL_NAME PARA#1 ... PARA#N
MATERIAL_ID Linear $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
[ $\text{[math]}$ $\text{[math]}$ TulerButcher
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$ ]
MATERIAL_ID LinearPlaneStress $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ [ $\text{[math]}$ $\text{[math]}$ ]
MATERIAL_ID HyperElasticPlaneStress $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ [ $\text{[math]}$ $\text{[math]}$ ]
MATERIAL_ID HenckyElastic $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
[ $\text{[math]}$ $\text{[math]}$ TulerButcher
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$ ]
MATERIAL_ID HypoElastic $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
MATERIAL_ID MooneyRivlin $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ [TulerButcher $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ ]
MATERIAL_ID NeoHookean $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
[TulerButcher $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ ]
MATERIAL_ID Ogden $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
[ $\text{[math]}$ ] $\text{[math]}$ $\text{[math]}$
[ $\text{[math]}$ ] $\text{[math]}$ [ $\text{[math]}$ ]
MATERIAL_ID StVenantKirchhoff $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
[ $\text{[math]}$ $\text{[math]}$ TulerButcher
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$ ]
MATERIAL_ID BilinearPlastic $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
[ $\text{[math]}$ $\text{[math]}$ ] MAXEPS
$\text{[math]}$ YSSFSRT-ID
MATERIAL_ID FiniteStrainPlastic $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
[ $\text{[math]}$ $\text{[math]}$ ] MAXEPS
$\text{[math]}$ YSSFSRT-ID
MATERIAL_ID J2Plasticity $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ MAXEPS YSSFSRT-ID
MATERIAL_ID KK1 $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ MAXEPS YSSFSRT-ID
MATERIAL_ID KK2 $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$
MATERIAL_ID LogStrainPlastic $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
[ $\text{[math]}$ $\text{[math]}$ ] MAXEPS
$\text{[math]}$ YSSFSRT-ID
MATERIAL_ID SimoPlastic $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
MATERIAL_ID ViscoLinearElastic $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
[ $\text{[math]}$ $\text{[math]}$ ] $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ [TulerButcher
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$ ]
MATERIAL_ID ViscoLinearPlaneStress $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ [ $\text{[math]}$ $\text{[math]}$ ]
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$
MATERIAL_ID ViscoHyperElasticPlaneStress $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ [ $\text{[math]}$ $\text{[math]}$ ]
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
MATERIAL_ID ViscoMooneyRivlin $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ [TulerButcher $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ ]
MATERIAL_ID ViscoNeoHookean $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
[TulerButcher $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ ]
MATERIAL_ID ViscoStVenantKirchhoff $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
[ $\text{[math]}$ $\text{[math]}$ ] $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ [TulerButcher
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$ ]
MATERIAL_ID PlaneStressMooneyRivlin $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ [TulerButcher
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$ ]
MATERIAL_ID PlaneStressNeoHookean $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ [TulerButcher $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ ]
MATERIAL_ID PlaneStressBilinearPlastic $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
[ $\text{[math]}$ $\text{[math]}$ ] $\text{[math]}$
MAXEPS $\text{[math]}$ YSSFSRT-ID
MATERIAL_ID PlaneStressFiniteStrainPlastic $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
[ $\text{[math]}$ $\text{[math]}$ ] $\text{[math]}$
MAXEPS $\text{[math]}$ YSSFSRT-ID
MATERIAL_ID PlaneStressViscoMooneyRivlin $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ [TulerButcher
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$ ]
MATERIAL_ID PlaneStressViscoNeoHookean $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ [TulerButcher $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ ]
MATERIAL_ID FabricMap $\text{[math]}$ XX-SS2DT-ID YY-SS2DT-ID
XY-SS1DT-ID $\text{[math]}$ [ $\text{[math]}$
$\text{[math]}$ ]
MATERIAL_ID ShellFabricMap $\text{[math]}$ XX-SS2DT-ID YY-SS2DT-ID
XY-SS1DT-ID $\text{[math]}$ [ $\text{[math]}$
$\text{[math]}$ ]
MATERIAL_ID FabricMat $\text{[math]}$ XX-YMST-ID YY-YMST-ID
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ [ $\text{[math]}$ $\text{[math]}$ ]
MATERIAL_ID ShellFabricMat $\text{[math]}$ XX-YMST-ID YY-YMST-ID
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ [ $\text{[math]}$ $\text{[math]}$ ]
MATERIAL_ID ViscoFabricMap $\text{[math]}$ XX-SS2DT-ID YY-SS2DT-ID
XY-SS1DT-ID $\text{[math]}$ [ $\text{[math]}$
$\text{[math]}$ ] $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$
MATERIAL_ID ShellViscoFabricMap $\text{[math]}$ XX-SS2DT-ID YY-SS2DT-ID
XY-SS1DT-ID $\text{[math]}$ [ $\text{[math]}$
$\text{[math]}$ ] $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$
MATERIAL_ID ViscoFabricMat $\text{[math]}$ XX-YMST-ID YY-YMST-ID
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ [ $\text{[math]}$ $\text{[math]}$ ]
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
MATERIAL_ID ShellViscoFabricMat $\text{[math]}$ XX-SS2DT-ID YY-SS2DT-ID
XY-SS1DT-ID $\text{[math]}$ [ $\text{[math]}$
$\text{[math]}$ ] $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$
MATERIAL_ID TorchMat $\text{[math]}$ module $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ [ $\text{[math]}$ $\text{[math]}$ ]
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$

`READ`	Sub-command keyword used to introduce a material name (characters) and associate it with the library located and stored in `<pathandfilename.so>` (characters) and linked with aeros.
`MATERIAL_ID`	ID number of the material law (integer).
`MATERIAL_NAME`	Name of the material law (characters).
`<pathandfilename>`	Name of the file (including path, if needed) containing the material law library. This entry must be specified between quotes (" "), and the file it specifies must have the extension `.so`.
`PARA#1`	First parameter expected by the library `<pathandfilename.so>`.
`PARA#N`	Last parameter expected by the library `<pathandfilename.so>`.
`Linear`	Name of the pre-defined standard linear elastic material law with linear kinematics (characters). Its conjugate strain and stress are the infinitesimal strain and the first Piola-Kirchhoff stress. This material law has an anisotropic variant which can be specified using the sub-command `COEF` of COMPOSITE: in this case, the constitutive matrix and coefficients of thermal expansion are defined using the information inputted under `COEF`, and the parameters $\text{[math]}$ , $\text{[math]}$ , $\text{[math]}$ , and $\text{[math]}$ inputted under this command are ignored.
`LinearPlaneStress`	Name of the pre-defined material law that is the plane stress counterpart of the linear elastic material law `Linear` described above (characters).
`HyperElasticPlaneStress`	Name of the pre-defined finite strain hyperelastic material law that is the plane stress counterpart of the material law `StVenantKirchhoff` described above (characters).
`HenckyElastic`	Name of another pre-defined finite strain hyperelastic material law (appropriate for larger strains) (characters). Its conjugate strain and stress are the Lagrangian Hencky (engineering) strain and the rotated Kirchhoff stress. This material law has an anisotropic variant which can be specified using the `COEF` sub-command of COMPOSITE, in which case the parameters $\text{[math]}$ , $\text{[math]}$ , and $\text{[math]}$ inputted under this command are ignored.
`HypoElastic`	Name of the pre-defined plane stress version of the hypoelastic material law (characters).
`MooneyRivlin`	Name of the pre-defined compressible version of the finite strain Mooney-Rivlin hyperelastic material law (characters).
`NeoHookean`	Name of the pre-defined compressible version of the finite strain hyperelastic material law (characters).
`Ogden` (with $\text{[math]}$ only)	Name of the pre-defined Ogden hyperelastic material law with 1 to 9 terms in the Ogden series that defines the strain energy density in terms of the deviatoric principal stretches $\text{[math]}$ characterizing the distorsional response, and a 1-term bulk volumetric response function $\text{[math]}$ Here, $\text{[math]}$ denotes the determinant of the deformation gradient, $\text{[math]}$ to $\text{[math]}$ and $\text{[math]}$ to $\text{[math]}$ are material properties that characterize the distorsional response of the material, and $\text{[math]}$ is its bulk modulus.
`Ogden` (with $\text{[math]}$ and $\text{[math]}$ )	Name of the pre-defined Ogden hyperelastic material law with 2 to 9 terms in the Ogden series that defines the strain energy density in terms of the deviatoric principal stretches $\text{[math]}$ characterizing the distorsional response, and a 2-term bulk volumetric response function $\text{[math]}$ Here, $\text{[math]}$ denotes the determinant of the deformation gradient, $\text{[math]}$ to $\text{[math]}$ and $\text{[math]}$ to $\text{[math]}$ are material properties that characterize the distorsional response of the material, and $\text{[math]}$ and $\text{[math]}$ are material properties that characterize its volumetric response.
`StVenantKirchhoff`	Name of a pre-defined finite strain hyperelastic material law (appropriate for metals and moderate strains) (characters). Its conjugate strain and stress are the Green-Lagrange (engineering) strain – which introduces in the problem to be solved a geometric nonlinearity – and the second Piola-Kirchhoff stress. This material law has an anisotropic variant which can be specified using the `COEF` sub-command of COMPOSITE, in which case the parameters $\text{[math]}$ , $\text{[math]}$ , and $\text{[math]}$ inputted under this command are ignored.
`BilinearPlastic`	Name of a pre-defined infinitesimal strain bilinear plastic material law featuring kinematic hardening (characters). Its conjugate strain and stress are the infinitesimal strain and the first Piola-Kirchhoff stress.
`FiniteStrainPlastic`	Name of a pre-defined finite strain plastic material law featuring kinematic hardening (characters). Its conjugate strain and stress are the Green-Lagrange (engineering) strain – which introduces in the problem to be solved a geometric nonlinearity – and the second Piola-Kirchhoff stress.
`J2Plasticity`	Name of the pre-defined plane stress version of the von Mises plasticity material law based on the second stress invariant featuring kinematic and/or isotropic hardening (characters). Its conjugate strain and stress are the infinitesimal strain and the first Piola-Kirchhoff stress.
`KK1`	Name of the pre-defined plane stress plasticity material law due to Korkolis and Kydiakides featuring kinematic and/or isotropic hardening and an advanced yield function including deformation-induced anisotropy (characters). Its conjugate strain and stress are the infinitesimal strain and the first Piola-Kirchhoff stress.
`KK2`	Name of the pre-defined plane stress plasticity material law for aluminum Al-6260-T4 due to Korkolis and Kydiakides featuring an advanced yield function including deformation-induced anisotropy and an experimental-based stress-strain curve (characters). Its conjugate strain and stress are the infinitesimal strain and the first Piola-Kirchhoff stress.
`LogStrainPlastic`	Name of another pre-defined finite strain plastic material law featuring logarithmic strains and kinematic hardening (characters). Its conjugate strain and stress are the Lagrangian Hencky (engineering) strain and the rotated Kirchhoff stress.
`SimoPlastic`	Name of a pre-defined finite strain elasto-plastic material law formulated in the logarithmic principal stretches and based on a multiplicative decomposition of the deformation gradient (see J. C. Simo, "Algorithms for Static and Dynamic Multiplicative Plasticity that Preserve the Classical Return Mapping Schemes of the Infinitesimal Theory," Computer Methods in Applied Mechanics and Engineering, Vol. 99, pp. 61-112 (1992))
`ViscoLinearElastic`	Name of a pre-defined infinitesimal strain linear elastic material law equipped with a 3-term Prony series viscoelastic model (see, for example, S.M. Goh, M.N. Charalambides, J.G. Williams, "Determination of the Constitutive Constants of Non-Linear Viscoelastic Materials," Mechanics of Time-Dependent Materials, Vol. 8, pp 255-268 (2004)).
`ViscoLinearPlaneStress`	Name of a pre-defined infinitesimal strain plane-stress material law for membrane elements (types 128 and 129, only), based on the material law `LinearPlaneStress` with a Prony series viscoelastic model (characters).
`ViscoHyperElasticPlaneStress`	Name of a pre-defined finite strain plane-stress material law for membrane elements (types 128 and 129, only), based on the material law `HyperElasticPlaneStress` with a Prony series viscoelastic model (characters).
`ViscoMooneyRivlin`	Name of a pre-defined finite strain Mooney-Rivlin material law equipped with a 3-term Prony series viscoelastic model (see, for example, S.M. Goh, M.N. Charalambides, J.G. Williams, "Determination of the Constitutive Constants of Non-Linear Viscoelastic Materials," Mechanics of Time-Dependent Materials, Vol. 8, pp 255-268 (2004)).
`ViscoNeoHookean`	Name of a pre-defined finite strain Neo-Hookean material law equipped with a 3-term Prony series viscoelastic model (see, for example, S.M. Goh, M.N. Charalambides, J.G. Williams, "Determination of the Constitutive Constants of Non-Linear Viscoelastic Materials," Mechanics of Time-Dependent Materials, Vol. 8, pp 255-268 (2004)).
`ViscoStVenantKirchhoff`	Name of a pre-defined finite strain hyperelastic material law equipped with a 3-term Prony series viscoelastic model (see, for example, S.M. Goh, M.N. Charalambides, J.G. Williams, "Determination of the Constitutive Constants of Non-Linear Viscoelastic Materials," Mechanics of Time-Dependent Materials, Vol. 8, pp 255-268 (2004)).
`PlaneStressMooneyRivlin`	Name of the pre-defined material law that is the plane stress counterpart of the material law `MooneyRivlin` described above (characters). It is implemented by numerically enforcing the plane-stress condition as described in S. Klinkel and S. Govindjee, "Using Finite Strain 3D-Material Models in Beam and Shell Elements," Engineering Computations, Vol. 19, pp. 254-271 (2002), which involves solving a nonlinear equation at each Gauss point of an element.
`PlaneStressNeoHookean`	Name of the pre-defined material law that is the plane stress counterpart of the material law `NeoHookean` described above (characters). It is implemented by numerically enforcing the plane-stress condition as described in S. Klinkel and S. Govindjee, "Using Finite Strain 3D-Material Models in Beam and Shell Elements," Engineering Computations, Vol. 19, pp. 254-271 (2002), which involves solving a nonlinear equation at each Gauss point of an element.
`PlaneStressBilinearPlastic`	Name of the pre-defined material law that is the plane stress counterpart of the material law `BilinearPlastic` described above (characters). It is implemented by numerically enforcing the plane-stress condition as described in S. Klinkel and S. Govindjee, "Using Finite Strain 3D-Material Models in Beam and Shell Elements," Engineering Computations, Vol. 19, pp. 254-271 (2002), which involves solving a nonlinear equation at each Gauss point of an element.
`PlaneStressFiniteStrainPlastic`	Name of the pre-defined material law that is the plane stress counterpart of the material law `FiniteStrainPlastic` described above (characters). It is implemented by numerically enforcing the plane-stress condition as described in S. Klinkel and S. Govindjee, "Using Finite Strain 3D-Material Models in Beam and Shell Elements," Engineering Computations, Vol. 19, pp. 254-271 (2002), which involves solving a nonlinear equation at each Gauss point of an element.
`PlaneStressViscoMooneyRivlin`	Name of the pre-defined finite strain material law that is the plane stress counterpart of the material law `ViscoMooneyRivlin` described above (characters). It is implemented by numerically enforcing the plane-stress condition as described in S. Klinkel and S. Govindjee, "Using Finite Strain 3D-Material Models in Beam and Shell Elements," Engineering Computations, Vol. 19, pp. 254-271 (2002), which involves solving a nonlinear equation at each Gauss point of an element.
`PlaneStressViscoNeoHookean`	Name of the pre-defined finite strain material law that is the plane stress counterpart of the material law `ViscoNeoHookean` described above (characters). It is implemented by numerically enforcing the plane-stress condition as described in S. Klinkel and S. Govindjee, "Using Finite Strain 3D-Material Models in Beam and Shell Elements," Engineering Computations, Vol. 19, pp. 254-271 (2002), which involves solving a nonlinear equation at each Gauss point of an element.
`FabricMap`	Name of a pre-defined finite strain plane-stress material law for membrane elements (types 128 and 129, only) in which the stress response is given exclusively by tables (characters). This material law is equivalent to material 034M (MAT_FABRIC_MAP) in LS-DYNA.
`ShellFabricMap`	Name of a pre-defined infinitesimal strain plane-stress material law for shell elements (types 15 and 1515, only) in which the stress response is given exclusively by tables (characters). This material law is equivalent to material 034M (MAT_FABRIC_MAP) in LS-DYNA.
`FabricMat`	Name of a pre-defined finite strain orthotropic plane-stress material law for membrane elements (types 128 and 129, only) in which the material Young modulii are specified in tables (characters). This material law is equivalent to material 034 (MAT_FABRIC) in LS-DYNA.
`ShellFabricMat`	Name of a pre-defined infinitesimal strain orthotropic plane-stress material law for shell elements (types 15 and 1515, only) in which the material Young modulii are specified in tables (characters). This material law is equivalent to material 034 (MAT_FABRIC) in LS-DYNA.
`ViscoFabricMap`	Name of a pre-defined finite strain plane-stress material law for membrane elements (types 128 and 129, only), based on the material law `FabricMap` with a Prony series viscoelastic model (characters).
`ShellViscoFabricMap`	Name of a pre-defined infinitesimal strain plane-stress material law for shell elements (types 15 and 1515, only), based on the material law `ShellFabricMap` with a Prony series viscoelastic model (characters).
`ViscoFabricMat`	Name of a pre-defined finite strain plane-stress material law for membrane elements (types 128 and 129, only), based on the material law `FabricMat` with a Prony series viscoelastic model (characters).
`ShellViscoFabricMat`	Name of a pre-defined infinitesimal strain plane-stress material law for shell elements (types 15 and 1515, only), based on the material law `ShellFabricMat` with a Prony series viscoelastic model (characters).
`TorchMat`	Name of a pre-defined plane-stress material law for membrane elements (types 128 and 129, only), in which the stress response is given by a regression artificial neural network function (characters). The constitutive function associated with this material law can be written as $\text{[math]}$ where $\text{[math]}$ is a $\text{[math]}$ symmetric matrix, $\text{[math]}$ is the regression artificial neural network function, $\text{[math]}$ is the second Piola-Kirchhoff stress tensor, $\text{[math]}$ is the Green-Lagrange strain, and $\text{[math]}$ is a user-specified scaling factor for the outputs of the regression artificial neural network function.
$\text{[math]}$	Mass density per unit volume (real).
$\text{[math]}$	Material Young modulus (real).
$\text{[math]}$	Material Poisson ratio (real).
$\text{[math]}$	Ambient (reference) temperature of the element assigned this material law (real). The default value is 0. WARNING: if this value is different from the nodal temperature (see TEMPERATURES) of that element, it causes the generation of a thermal load even in a pure structural analysis. This parameter can be skipped (and therefore is optional) if the parameter $\text{[math]}$ is simultaneously skipped (see below).
$\text{[math]}$	Coefficient of thermal expansion (real). The default value is 0. This parameter can be skipped (and therefore is optional) if the parameter $\text{[math]}$ is simultaneously skipped (see above).
`TulerButcher`	Optional sub-command keyword (characters) for specifying the Tuler-Butcher brittle failure criterion and its parameters. When a material is subjected to dynamic loading, crack propagation strongly depends on the strain rate, stress wave amplitude, and the exposure time. In this case, the Tuler-Butcher failure criterion can be used as a material brittle failure criterion. It can be expressed as $\text{[math]}$ for $\text{[math]}$ , where $\text{[math]}$ denotes the maximum principal stress, $\text{[math]}$ is a specific threshold stress, $\text{[math]}$ is time for the fracture and $\text{[math]}$ is the stress impulse for failure. Note that this brittle damage model degenerates to the maximum principle stress model when $\text{[math]}$ is set to zero. Specifying this sub-command keyword and inputting after it the parameters of the Tuler-Butcher failure criterion activates the method of element deletion during a nonlinear dynamic computation. Specifically, the stress at a Gauss point is set in this case to zero when the damage accumulation function described above becomes greater than or equal to $\text{[math]}$ at this point. When this criterion is met at all Gauss points of an element, this element is deleted from the finite element model.
$\text{[math]}$	Specific threshold stress parameter of the Tuler-Butcher brittle failure criterion (real).
$\text{[math]}$	Exponent in the damage accumulation function of the Tuler-Butcher brittle failure criterion (real).
$\text{[math]}$	Stress impulse failure (or macroscopic fracture threshold) parameter of the Tuler-Butcher brittle failure criterion (real).
$\text{[math]}$ , $\text{[math]}$ , $\text{[math]}$	Coefficients of the compressible version of the Mooney-Rivlin model (real) where the strain energy density function can be written as $\text{[math]}$ and $\text{[math]}$ denotes the determinant of the deformation gradient and $\text{[math]}$ , $\text{[math]}$ and $\text{[math]}$ are its three invariants.
$\text{[math]}$ – $\text{[math]}$	Material properties of the pre-defined hyperelastic material law named `Ogden` that characterize the distorsional response of the material (real).
$\text{[math]}$ – $\text{[math]}$	Material properties of the pre-defined hyperelastic material law named `Ogden` that characterize the distorsional response of the material (real).
$\text{[math]}$	Material property (or Bulk modulus) of the pre-defined hyperelastic material law named `Ogden` that characterizes the volumetric response of the material (real).
$\text{[math]}$	Material property of the pre-defined hyperelastic material law named `Ogden` that characterizes the volumetric response of the material (real).
$\text{[math]}$	Tangent modulus (for any material with linear hardening and requiring the explicit input of this parameter) representing the slope of the inelastic portion of uniaxial stress vs uniaxial strain curve (real). Note that if a YSST curve is specified for the material, this parameter is used only to define the kinematic hardening modulus and the curve is used to obtain the isotropic hardening modulus..
$\text{[math]}$	Yield stress for the bilinear, finite strain, J2, and KK1 plastic material laws (real). If a negative integer value -INT (note the minus sign) is specified for this otherwise positive real parameter, the yield stress is understood to be that function of the effective plastic strain that is tabulated in YSST and identified by `curve_id` = `INT`.
$\text{[math]}$	Free-parameter of the hardening model (real): $\text{[math]}$ corresponds to pure kinematic hardening, $\text{[math]}$ to pure isotropic hardening, and $\text{[math]}$ to a combination of kinematic and isotropic hardening.
`MAXEPS`	Effective plastic strain at failure (default value is infinity). Specifying a finite and strictly positive value for this parameter activates the method of element deletion during a nonlinear explicit dynamic computation. Specifically, the stress at a Gauss point is set in this case to zero when the effective plastic strain becomes greater than or equal to `MAXEPS` at this point. When this criterion is met at all Gauss points of an element, this element is deleted from the finite element model.
$\text{[math]}$	Relative tolerance for the convergence of the nonlinear material solver at each material point (real). The default value is $\text{[math]}$ .
`YSSFSRT-ID`	Integer ID (integer) of the yield stress scaling factor vs effective plastic strain rate curve (see YSSFSRT). Ommitting this parameter sets the default mode of computations where the yield stress scaling factor is set to $\text{[math]}$ and therefore its dependence on the effective plastic strain rate is ignored.
$\text{[math]}$	Isotropic hardening modulus for the J2 plasticity and KK1 material laws (real). Note that in theory, $\text{[math]}$ , but in AERO-S, $\text{[math]}$ is specified directly for these material laws. Note also that if a YSST curve is specified for the material, then this parameter is ignored.
$\text{[math]}$	Kinematic hardening modulus for the J2 plasticity and KK1 material laws (real). Note that in theory, $\text{[math]}$ , but in AERO-S, $\text{[math]}$ is specified directly for these material laws.
$\text{[math]}$ – $\text{[math]}$	Characteristic amplitudes for the 3-term Prony series viscoelastic model used in the pre-defined material laws `ViscoLinearElastic`, `ViscoNeoHookean`, and `ViscoMooneyRivlin` (real).
$\text{[math]}$ – $\text{[math]}$	Relaxation times for the 3-term Prony series viscoelastic model used in the pre-defined material laws `ViscoLinearElastic`, `ViscoNeoHookean`, and `ViscoMooneyRivlin` (real).
$\text{[math]}$	Element material thickness (real).
`XY-SS1DT-ID`	Integer ID (integer) identifying the one-dimensional table (i.e. curve) giving the local second Piola-Kirchhoff $\text{[math]}$ -stress as a function of the local Green-Lagrange $\text{[math]}$ -strain (see SS1DT).
`XX-SS2DT-ID`	Integer ID (integer) identifying the two-dimensional table (i.e. surface) giving the local $\text{[math]}$ -stress as a function of the local $\text{[math]}$ -strain and $\text{[math]}$ -strain (see SS2DT).
`YY-SS2DT-ID`	Integer ID (integer) identifying the two-dimensional table (i.e. surface) giving the local $\text{[math]}$ -stress as a function of the engineering local $\text{[math]}$ -strain and $\text{[math]}$ -strain (see SS2DT).
`XX-YMST-ID`	Integer ID (integer) identifying the one-dimensional table (i.e. curve) giving the material Young modulus $\text{[math]}$ as a function of the local $\text{[math]}$ -strain (see YMST).
`YY-YMST-ID`	Integer ID (integer) of the one-dimensional table (i.e. curve) giving the material Young modulus $\text{[math]}$ as a function of the local $\text{[math]}$ -strain (see YMST).
$\text{[math]}$	Material shear modulus (real).
$\text{[math]}$	Material Poisson ratio (real).
$\text{[math]}$	Material Poisson ratio (real).
`module`	Path and filename of a `PyTorch` module encoding the regression artificial neural network function underlying the material law `TorchMat` (characters).
$\text{[math]}$	Scaling factor for the outputs of the regression artificial neural network function underlying the material law `TorchMat` (float). It can be used, for example, to allow using different systems of units for the the second Piola-Kirchhoff stress tensor $\text{[math]}$ when training offline the regression artificial neural network and exploiting it online in the constitutive model shown above, in which case $\text{[math]}$ should be set to the appropriate unit conversion factor. The default value is $\text{[math]}$ .
$\text{[math]}$	Scaling factor for the $\text{[math]}$ component of the input of the regression artificial neural network function underlying the material law `TorchMat`(float). For consistency, this factor must be the same as that used during the offline training of the regression artificial neural network for the purpose of optimal convergence.
$\text{[math]}$	Scaling factor for the $\text{[math]}$ component of the input of the regression artificial neural network function underlying the material law `TorchMat`(float). For consistency, this factor must be the same as that used during the offline training of the regression artificial neural network for the purpose of optimal convergence.
$\text{[math]}$	Scaling factor for the $\text{[math]}$ component of the input of the regression artificial neural network function underlying the material law `TorchMat`(float). For consistency, this factor must be the same as that used during the offline training of the regression artificial neural network for the purpose of optimal convergence.
$\text{[math]}$	Coefficient located at the $\text{[math]}$ -th row and $\text{[math]}$ -th column of the matrix $\text{[math]}$ defining the linear term of the regression artificial neural network function underlying the material law `TorchMat` (see above), $\text{[math]}$ = $\text{[math]}$ , $\text{[math]}$ = $\text{[math]}$ (float). The default value is $\text{[math]}$ . When a non-zero matrix $\text{[math]}$ is specified, the regression artificial neural network function can be interpreted as a correction to a linear stress-strain model (see above).
$\text{[math]}$	$\text{[math]}$ -th coordinate of a strain-space bounding box used by the material law `TorchMat` as follows (float). The contribution of the regression artificial neural network function to the linear stress-strain model (see above) is added only when the components of the strain tensor satisfy the following conditions: $\text{[math]}$ The default values are as follows: $\text{[math]}$ , $\text{[math]}$ ; and $\text{[math]}$ , $\text{[math]}$ .

89 MATERIAL LAW USAGE

The MATUSAGE command can be used to assign a material law specified under MATLAW to one or several elements.

Note 2: To be active, this command requires the presence of the NONLINEAR command in the same ASCII Input Command Data file (in this case, if this command is used to assign one or several material laws defined in MATLAW that are linear and based on linear kinematics, and provided that the computational model does not contain any other source of nonlinearity such as, for example, a follower force, the nonlinear solution strategy specified in NONLINEAR is guaranteed to converge in a single iteration). Otherwise, this command is ignored, the linear elastic material law is assigned to all elements of the computational structural model, and the properties of this material law should be set in MATERIAL.

Note 3: In the presence of the NONLINEAR command in the ASCII Input Command Data file, the material laws and properties specified under the MATLAW command and assigned using this command take precedence over those inputted using MATERIAL, when a conflict arises.

Note 4: In the absence of the MATLAW command but presence of the command NONLINEAR in the ASCII Input Command Data file:

Note 5: In the absence of both the NONLINEAR and MATLAW commands in the ASCII Input Command Data file, the linear elastic material law with infinitesimal strains is assigned by default to all elements of the computational structural model.

`ELEMENT#`	Element number whose material law number is to be specified (integer).
`MATLAW_LABEL`	Material law identification number (integer).
`MATERIAL_LABEL`	First element of a sequence of elements that have the same `MATLAW_LABEL` (integer).
`MATERIAL_NAME`	Last element of a sequence of elements that have the same `MATLAW_LABEL` (integer).

90 MESH DECOMPOSITION

The command DECOMPOSE can be used to perform an element-based mesh partitioning (or domain decomposition) of the computational domain, and exit or continue with a finite element analysis. For this purpose, four different mesh partitioning strategies suitable for different objectives are available:

aeros --dec --nsub <number_of_subdomains> [--trivial --deter --load --mem --exit --allow-mechanisms --use-scotch] <filename.aeros.aicdf>

Note 2: When this command is executed from the command line (see above) and specified in the AERO-S ASCII Input Command Data file, the value of any argument specified on the command line overrides that specified in the ASCII Input Command Data file.

Note 3: When a decomposition file is already available, the syntax of the command line for running AERO-S with this decomposition file on a shared memory is

aeros -d <decomposition_pathandfilename> [-v <verbose_frequency>] -n <number_of_processors> <filename.aeros.aicdf>

In this case, the above command can also be combined with some of the other features of the command DECOMPOSE as in the following syntax

aeros -d <decomposition_pathandfilename> [--load --mem] [-v <verbose_frequency>] [-n <number_of_processors>] <filename.aeros.aicdf>

Note 4: Using this command to generate an element-based mesh partition (or domain decomposition) of the computational domain does not imply that the global finite element model data will be distributed across all (subdomain-based) computational processes. By default, the entire finite element model data is duplicated in each MPI process, which is not a memory-efficient strategy. To distribute the global finite element model data across the MPI processes according to the generated domain decomposition — that is, to store in each MPI process only the part of the global data pertaining to the subdomains assigned to this MPI process — the following additional steps should also be performed. First, the finite element model data should be re-arranged into a set of binary distributed input files associated with the generated domain decomposition using SOWER (see SOWER's User's Reference Manual). Then, the aforementioned binary distributed input files should be inputted to the desired simulation via the ASCII Input Command Data file using the command BINARY and its sub-commands. In the case of a parallel system with a hybrid memory, if the user does not wish to use SOWER for the aforementioned purpose, the user should at least use the command mpirun with the "--bynode" option in order to limit the number of MPI processes — and therefore memory duplications — per shared memory sub-system.

TRIVIAL or ALLOW_MECHANISMS or USE_SCOTCH
NSUBS nsubs
DETER
FSGL
OUTFILE decomposition_pathandfilename
OUTLOAD
OUTMEM
EXIT
SKIP

`TRIVIAL`	The two-step strategy based on the greedy algorithm (STRAT2) is the default mesh partitioning strategy (characters). This sub-command keyword can be used to request instead the trivial mesh partitioning strategy (STRAT1).
`ALLOW_MECHANISMS`	The two-step strategy based on the greedy algorithm (STRAT2) is the default mesh partitioning strategy (characters). This sub-command keyword can be used to request instead a modified version of this strategy (STRAT3) where mechanisms due to various arrangements of spring, truss, and membrane elements are allowed in order to produce superior mesh partitions where the number of generated subdomains is as close as possible to the requested number of subdomains `NSUBS` (see below).
`USE_SCOTCH`	The two-step strategy based on the greedy algorithm (STRAT2) is the default mesh partitioning strategy (characters). This sub-command keyword can be used to request instead the mesh partitioning strategy based on SCOTCH (STRAT4), the software package and libraries for sequential and parallel graph partitioning, static mapping and clustering, sequential mesh and hypergraph partitioning, and sequential and parallel sparse matrix block ordering.
`NSUBS`	Sub-command keyword for specifying the desired number of subdomains (characters).
`nsubs`	Number of subdomains (integer). The generated mesh partition is guaranteed to contain `nsubs` subdomains only if the `TRIVIAL` mesh partitioning strategy is chosen (see above). Otherwise, the generated mesh partition may contain a different or slightly different number of subdomains, because of some optimizations that could be performed by the other mesh partitioning strategies. The default value is 1.
`DETER`	This sub-command keyword is relevant only for the two-step mesh partitioning strategy based on the greedy algorithm (STRAT2), whose second step is performed by default using a simulated annealing procedure (characters). It requests using instead a deterministic approach in order to reduce the CPU time of the second step.
`FSGL`	This sub-command keyword is relevant only for the two-step mesh partitioning strategy based on the greedy algorithm (STRAT2) and vibro-acoustic (aka elastoacoustic and fluid-structure) analysis (for example, see IMPEDANCE) (characters). It requests performing the mesh decomposition in such a way that the fluid-structure interface is embedded within the subdomains as much as possible.
`OUTFILE`	Sub-command keyword to request outputting the decomposition in `<decomposition_pathandfilename>` (characters).
`<decomposition_pathandfilename>`	Name of the mesh decomposition file (characters). The format of this file is essentially the number and list of the elements in each subdomain. The default is `FNAME.optDec` where `FNAME` is the prefix specified under the command CONTROL or its own default value.
`OUTLOAD`	This sub-command keyword is relevant only for the two-step mesh partitioning strategy based on the greedy algorithm (STRAT2) (characters). It requests outputting the load distribution in the file `<decomposition_pathandfilename>`.`load`. The load distribution is based on the weights of the elements in the subdomains (see WEIGHTS and FWEIGHTS). The default value is `off`.
`OUTMEM`	This sub-command keyword is relevant only for the two-step mesh partitioning strategy based on the greedy algorithm (STRAT2), and when an iterative FETI method is chosen as an equation solver (see STATICS) (characters). It requests outputting in the file `<decomposition_pathandfilename>`.`mem` an estimate of the subdomain-based memory consumption. This estimate is based on the requirements for factoring the subdomain matrices by a direct skyline method. By default, mid-side nodes are ignored by the overall mesh partitioning algorithm. However, when this option is specified, mid-side nodes are taken into account. Default value is `off`.
`EXIT`	Sub-command keyword to request exiting from AERO-S after the mesh partition is generated (characters). Default value is `off`.
`SKIP`	Sub-command keyword to request skipping this command (characters). Default value is `off`.

91 NODAL CONTACT

The NODALCONTACT command can be used to specify node-to-node contact of the form

NODE_1 NODE_2 N_X N_Y N_Z MODE mode_v GAP gap_v CONSTRAINT_METHOD

`NODE_1`	Id number of the first node (integer).
`NODE_2`	Id number of the second node (integer).
`N_X`	x-component of the normal to the contact surface oriented from `NODE_1` to `NODE_2` (float).
`N_Y`	y-component of the normal to the contact surface oriented from `NODE_1` to `NODE_2` (float).
`N_Z`	z-component of the normal to the contact surface oriented from `NODE_1` to `NODE_2` (float).
`GAP`	Keyword to be spelled out (characters).
`gap_v`	Initial gap between `NODE_1` and `NODE_2`. A negative gap means an initial penetration (float).
`MODE`	Keyword to be spelled out (characters).
`mode_v`	Specifying `mode_v` = 0 designates a tie-of-the-normal-component-of-the-displacement constraint. Specifying `mode_v` = 1 designates a normal contact constraint. Specifying `mode_v` = 2 designates a tie-of-the-normal-and-tangential-components-of-displacement constraint. Specifying `mode_v` = 3 designates both normal contact and tie-of-the-tangential-components-of-displacement constraints (integer).
`default_mode_v`	Default `mode_v` for all constraints. If not specified, the default mode is set to 1, i.e. normal contact (integer).
`CONSTRAINT_METHOD`	This is the method for enforcing the associated constraints (characters). The default method is set in CONSTRAINTS and used whenever this entry is omitted.
`multipliers`	The Lagrange multiplier method.
`elimination`	The elimination method.
`penalty` [`beta`]	The penalty method. The parameter `beta` should be a large positive number, typically of the order of $\text{[math]}$ (no default value is provided).

92 NODAL FRAMES

The NFRAMES command statement can be used to specify nodal reference frames to which any node defined in NODES can refer to either for the purpose of specifying in which frame the nodal coordinates are inputted, or in which frame the nodal degrees of freedom are defined, or both.

NFRAME# $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ $\text{[math]}$

`NFRAME#`	ID number of a nodal position (if 13 entries are inputted on the same line) or degree of freedom (if 10 entries are inputted on the same line) reference frame (integer).
$\text{[math]}$	$\text{[math]}$ coordinate of the origin of the nodal position frame identified by the ID number specified above (float).
$\text{[math]}$	$\text{[math]}$ coordinate of the origin of the nodal position frame identified by the ID number specified above (float).
$\text{[math]}$	$\text{[math]}$ coordinate of the origin of the nodal position frame identified by the ID number specified above (float).
$\text{[math]}$	First axis of the nodal reference frame identified by the ID number specified above, the nodal x-axis, expressed in the global reference frame (floats).
$\text{[math]}$	Second axis of the nodal reference frame identified by the ID number specified above, the nodal y-axis, expressed in the global reference frame (floats).
$\text{[math]}$	Third axis of the nodal reference frame identified above, the nodal z-axis, expressed in the global reference frame (floats).

93 NODES *S*

The NODES command statement is used to signal that the following data lines correspond to the coordinates, position frame, and degree of freedom frame of each node. The input data format is given below. There should be as many lines as the number of nodes in the mesh.

`NODE#`	ID number of a node (integer).
`X-ORDINATE`	x-ordinate of the node identified by the specified node ID number (float).
`Y-ORDINATE`	y-ordinate of the node identified by the specified node ID number (float).
`Z-ORDINATE`	z-ordinate of the node identified by the specified node ID number (float).
`POS_FRM`	ID number of the nodal position frame (see NFRAMES) in which the coordinates of the node identified by the node ID number specified above are defined (integer). The value 0, which is the default value, specifies that the nodal position frame is the global frame. (See NFRAMES).
`DOF_FRM`	ID number of the nodal degree of freedom frame (see NFRAMES) in which the degrees of freedom of the node identified by the node ID number specified above are defined (integer). The value 0, which is the default value, specifies that the nodal degree of freedom frame is the global frame. (See NFRAMES).

94 NON INTRUSIVE POLYNOMIAL CHAOS

The NONINPC command signals to the AERO-S code to perform a non intrusive uncertainty quantification analysis using the Polynomial Chaos (PC) representation. It requires that the input file also contains the GROUPS, RANDOM, and STATICS commands as well as their respective data. Essentially, AERO-S computes in this case the mean and standard deviation of a computed primal field v as follows

where

\text{[math]}

denotes the constant of the PC expansion of the non deterministic

\text{[math]}

field (“the output”),

\text{[math]}

denotes the number of realizations,

\text{[math]}

denotes the deterministic solution of the field

\text{[math]}

associated with the i-th realization of the random system,

\text{[math]}

denotes the probability density function,

\text{[math]}

denotes the j-th “basic” random variable which is assumed to be Gaussian,

\text{[math]}

denotes the deterministic coefficient of the i-th PC shape function

\text{[math]}

\text{[math]}

denotes the total number of PC shape functions

\text{[math]}

representing the non deterministic output, and

\text{[math]}

denotes the evaluation of

\text{[math]}

at the j-th realization of the random system.

`DEG_OUT`	Degree of the PC representation of the output which, together with the data of the RANDOM command, determines $\text{[math]}$ .
`NUM_RLZ`	Number of realizations $\text{[math]}$ of the random system (which implies the number of deterministic solutions) (integer).

95 NONLINEAR ANALYSIS

When the formulated static, quasistatic, or implicit dynamic finite element (FE) model is nonlinear, this command must be used to define a nonlinear solution strategy and specify its parameters. For structural problems, this is the case if:

In the presence of this command in the ASCII Input Command Data file, if an element of the FE model is not assigned a material law – either linear or nonlinear – (specified in MATLAW) using MATUSAGE, it is assigned by default the following material law:

In the absence of this command in the ASCII Input Command Data file however, all elements are assigned linear elasticity as the material law and the kinematics are assumed to be linear, even when otherwise implied or specified.

`METHOD`
`Newton`	This sub-command keyword specifies Newton's method for solving the governing nonlinear equations (characters). This method is also the default nonlinear solution method.
`arclength`	This sub-command keyword specifies an arclength method for solving the nonlinear equations associated with a nonlinear static computation (characters). Such a method differs from the standard Newton method in the path through which the captured solution converges, which in this case follows at each step a direction orthogonal to the tangent of the solution curve. Specifically, an arc length method causes Newton's method to converge along an arc, thereby often preventing divergence, even when the slope of the "load" vs. solution becomes zero or negative. For this reason, such a method is typically used to enable the nonlinear solution algorithm to pass limit points, such as maximum and minimum loads, and snap-through and snap-back responses. At these limit points, the stability of the numerical system is dependent on whether the analysis is performed under load or solution control. In structural analysis, these limit points are characteristic of buckling or failure.
`PARAMETERS`
`MAXITR maxitr_v`	For a nonlinear static, quasistatic, or implicit dynamic computation, this sub-command keyword (characters) followed by its integer value specifies the maximum number of iterations per solve to be performed by the chosen solution `METHOD`. The default value is 100.
`NLTOL nt1_v nt2_v nt3_v nt4_v`	For a nonlinear static, quasistatic, or implicit dynamic computation, this sub-command keyword (characters) and the four real values following it specify the various tolerances needed for assessing the convergence of the chosen solution `METHOD`. More specifically, the first two parameters `nt1_v` and `nt2_v` specify the tolerances for the convergence of the relative residual and solution increment, respectively (real, real). Their default values are $\text{[math]}$ and infinity, respectively. The third and fourth parameters `nt3_v` and `nt4_v` specify the tolerances for the convergence of the absolute residual and solution increment, respectively (real, real). Their default values are zero and infinity, respectively. The convergence of the chosen solution `METHOD` is declared when either of the following occurs (a) both of the relative residual and relative increment are below their specified respective tolerance levels, or (b) both of the absolute residual and absolute increment are below their specified respective tolerance levels. Note that a tolerance can be set to infinity using the characters "`INF`", and to machine epsilon $\text{[math]}$ using the characters "`EPS`".
`DLAMBDA real_1 real_2`	This sub-command keyword (characters) followed by two real numbers specifies the external "loading" parameters for a nonlinear static or quasistatic analysis only. However, for a quasistatic analysis where the material nonlinearities do not involve any inelasticity, the effect of this sub-command applies only to the first coupling cycle (see QSTATICS. The first real number, `real_1`, specifies the load fraction increment. The second real number, `real_2`, specifies the total load factor. For example, "DLAMBDA 0.25 1.0" specifies applying the external load in 4 steps, using a load increment equal to 0.25(Original Inputted Source Terms). On the other hand, "DLAMBDA 0.25 2.0" specifies amplifying first the external loads by the factor 2, then applying the resulting external load in 8 steps using a load increment equal to 0.25(Original Inputted Source Terms). This incremental loading strategy can help the convergence of the chosen solution `METHOD`.
`FITALG fitalg_v`	For structural problems, this sub-command keyword (characters) followed by an integer value specifies the fitting algorithm for the corotational formulation. For `fitalg` = `1` the tangent stiffness matrix is not consistent but the corotational framework is supposed to be more robust. For `fitalg` = `2` (default value), the tangent stiffness matrix is consistent (integer).
`FAILSAFE real_1`	For a nonlinear static or implicit dynamic computation, this keyword activates a fail-safe computational strategy when the chosen solution `METHOD` fails to converge and the absolute residual is less than the tolerance specified in `real_1` (real). The fail-safe strategy consists in repeating a load-step or time-step computation during which the aforementioned events occur using half the value of the load-step or time-step, until Newton's method converges. Upon convergence, the value of the load-step or time-step is doubled in each subsequent static or dynamic step computation until the original value of the load-step or time-step is restored. The default value of `real_1` is machine precision.
`UNSYMMETRIC`	The contributions to the tangent stiffness of various types of configuration-dependent external forces (for example, pressure, follower forces, and both follower and axial moments) lead to an unsymmetric geometric tangent stiffness matrix. For dynamic analysis, the contribution to the dynamic tangent stiffness matrix of some rotary inertial forces (for example, discrete inertial moments and rotary intertial forces emanating from beam and shell elements) also lead to an unsymmetric dynamic tangent stiffness matrix. By default, these matrices are symmetrized in order to reduce storage costs and enable the usage of a symmetric equation solver (see STATICS), which also reduces CPU costs. Hence, this sub-command keyword can be used to prevent this default symmetrization (characters). In this case, an unsymmetric equation solver must be specified in STATICS in case the tangent or dynamic tangent stiffness matrix becomes unsymmetric.
`REBUILD int_1` [`int_2`]	This sub-command keyword (characters) followed by two integers manages two different intervals for deciding when to rebuild the tangent "stiffness" matrix during the solution of a nonlinear problem by the chosen `METHOD`. The integer `int_1` specifies the iteration interval within a time-step of a dynamic analysis, or a load-step of a static or quasistatic analysis where `DLAMBDA` is used to apply the external load incrementally. For example, `int_1` = `1` specifies rebuilding the tangent stiffness matrix at every iteration, and `int_1` = `2` specifies rebuilding it at every second iteration. The default value for `int_1` is 1. Usage of the integer `int_2` is optional, and its default value is 1. Otherwise, `int_2` specifies the time-step or load-step interval. For example, `int_2` = `1` specifies every time-step or load-step, and `int_1` = `2` specifies every other time-step or load-step. The default value of `int_2` is also 1. Hence, setting `int_1` = `1` and `int_2` = `1` specifies rebuilding the tangent stiffness matrix at every nonlinear iteration of every time-step or load-step. Setting `int_1` = `2` and `int_2` = `3` specifies rebuilding the tangent stiffness matrix at every second iteration of every third time-step or load-step. The characters "`MAX`" can be used to set either or both of `int_1` and `int_2` to a very large interval to limit or effectively deactivate rebuilding the tangent stiffness matrix, respectively. An interesting intermediate case is given by the combination `int_1` = "`MAX`" and `int_2` = `1` which specifies rebuilding the tangent stiffness matrix only at the start of every time-step or load-step.
`LINESEARCH ALPROC` [`maxitr $\text{[math]}$ $\text{[math]}$ flag`]	This sub-command keyword (characters) is applicable only if `Newton` is specified as the nonlinear solution `METHOD`. It requests equipping Newton's method with a line search strategy and specifies the parameters of this strategy. In this case, it is recommended to rebuild the tangent stiffness matrix at each Newton iteration (see `REBUILD` above). Given a nonlinear problem of the form $\text{[math]}$ where $\text{[math]}$ and $\text{[math]}$ denote the nonlinear residual and solution of interest, respectively, Newton's method solves this problem by computing the iterates $\text{[math]}$ where the increment $\text{[math]}$ is the solution of the linearized problem $\text{[math]}$ and $\text{[math]}$ denotes the Jacobian (or tangent stiffness) of $\text{[math]}$ with respect to $\text{[math]}$ . For highly nonlinear problems, combining Newton's method with a line search strategy can prove to be a more appropriate solution method as this combination searches for the solution of the above nonlinear problem in the form of less agressive iterates as follows $\text{[math]}$ where $\text{[math]}$ is a step-length computed by AERO-S using either a `backtracking` or a `bisection` procedure (see `ALPROC` below). Note that equipping Newton's method with a line search strategy typically increases the number of iterations required for convergence. However, for many problems, Newton's method may simply fail to converge without a line search strategy.
`ALPROC`	Sub-command keyword to specify a procedure for computing the step-length parameter $\text{[math]}$ of the line search strategy (characters). Two options are currently available:
`backtracking`	For a given pair of $\text{[math]}$ and $\text{[math]}$ , the main idea in this case is to minimize the "merit" function $\text{[math]}$ by searching iteratively for the value of $\text{[math]}$ which satisfies the first Wolfe condition — aka the "sufficient decrease condition" $\text{[math]}$ where $\text{[math]}$ is the gradient of $\text{[math]}$ with respect to $\text{[math]}$ and satisfies $\text{[math]}$ and $\text{[math]}$ is a user-specified "sufficient decrease factor" chosen as $\text{[math]}$ (see $\text{[math]}$ below). If the tangent stiffness $\text{[math]}$ is rebuilt at every iteration $\text{[math]}$ (see `REBUILD` above), the above sufficient decrease condition can also be written as $\text{[math]}$ Hence, the value of $\text{[math]}$ that satisfies this condition is computed iteratively as follows. The first trial value of $\text{[math]}$ is set to the maximum value of 1.0. Then, while the above sufficient decrease condition is not satisfied, the current value of $\text{[math]}$ is reduced by the user-specified "contraction factor" $\text{[math]}$ (see $\text{[math]}$ below) — that is, $\text{[math]}$ — until the sufficient decrease condition is satisfied.
`bisection`	In this case, the merit function employed, when applicable, is the scalar-valued potential function whose gradient is the nonlinear residual $\text{[math]}$ defined above (see `backtracking`) — that is, $\text{[math]}$ . This function is minimized by applying the well-known bisection root-finding algorithm to search iteratively for the value of $\text{[math]}$ which satisfies the second strong Wolfe condition — aka the "curvature condition" (or "sufficient slope decrease condition") $\text{[math]}$ where $\text{[math]}$ is a user-specified "sufficient slope decrease factor" that is usually chosen to be much larger than $\text{[math]}$ (see $\text{[math]}$ below).
`maxitr`	Specifies the maximum number of line search or bisection iterations — that is, the maximum number of iterations for finding the optimal step-length. The default value of this parameter is 10.
$\text{[math]}$	If `ALPROC` is set to `backtracking`, this parameter specifies the value of the sufficient decrease factor $\text{[math]}$ (real). In this case, the chosen value must satisfy $\text{[math]}$ and the default value is 1.0e-4. On the other hand, if `ALPROC` is set to `bisection`, this parameter specifies the value of the sufficient slope decrease factor $\text{[math]}$ (real). In this case, the defaut value of this parameter is 0.1.
$\text{[math]}$	This parameter is relevant only when `ALPROC` is set to `backtracking`. It specifies the value of the contraction factor $\text{[math]}$ (real). The chosen value must satisfy $\text{[math]}$ . The default value of this parameter is 0.8.
`flag`	Setting this output flag to `YES` requests outputting to the screen some relevant information at each line search iteration. Setting it to `NO` (default setting) turns off this output.
`PENALTY int_1 real_1 real_2`	This sub-command keyword (characters) followed by one integer and two real numbers specifies the parameters of the penalty or augmented Lagrangian method for enforcing CONSTRAINTS in a nonlinear analysis. The integer `int_1` specifies the maximum number of outer iterations on the penalty parameter in the case of the penalty method, or on the Lagrange multipliers (and optionally the penalty parameter) in the case of the augmented Lagrangian method; its default value is 1. The first real number, `real_1`, specifies the absolute tolerance for assessing the convergence of the outer iteration loop based on the infinite norm of the constraint violations; its default value is $\text{[math]}$ . The second real number, `real_2`, specifies the factor by which the penalty parameter in either method is increased at every outer iteration; its default value is 10.

96 NONLINEAR SUPERPOSITION OF RIGID AND DEFORMATION MODES

Note that the global, reduced-order mass and stiffness matrices

\text{[math]}

and

\text{[math]}

, as well as some quantities involved in the evaluation of the two vectors of generalized forces

\text{[math]}

and

\text{[math]}

, are invariant in a given simulation. Hence, AERO-S always pre-computes these quantities offline before applying online the structural dynamic ROM outlined above to the modal analysis of a structural system. This offline/online staging of the computations accelerates a modal analysis based on the computational technology underlying the FLOATINGFRAME command.

It follows that a structural dynamic analysis based on the structural dynamic ROM described above requires including in the same AERO-S ASCII Input Command Data file:

Note 2: After reading the partial ROB

\text{[math]}

inputted via the READMODE command, AERO-S tests whether any of its columns is a rigid body mode and ignores any such modes.

RMIV $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
RMPT $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
SCAL flagSCAL

`RMIV`	Sub-command keyword (characters) for specifying the initial values of the generalized velocity dofs associated with the rigid body modes. Note that the initial values of the generalized velocity dofs associated with the structural deformation modes should be assigned in IVELOCITIES using the `MODAL` sub-command keyword.
$\text{[math]}$	Initial value of the generalized velocity dof associated with the rigid body $\text{[math]}$ -translation mode (real). The default value is $\text{[math]}$ .
$\text{[math]}$	Initial value of the generalized velocity dof associated with the rigid body $\text{[math]}$ -translation mode (real). The default value is $\text{[math]}$ .
$\text{[math]}$	Initial value of the generalized velocity dof associated with the rigid body $\text{[math]}$ -translation mode (real). The default value is $\text{[math]}$ .
$\text{[math]}$	Initial value of the generalized velocity dof associated with the rigid body $\text{[math]}$ -rotation mode (real). The default value is $\text{[math]}$ .
$\text{[math]}$	Initial value of the generalized velocity dof associated with the rigid body $\text{[math]}$ -rotation mode (real). The default value is $\text{[math]}$ .
$\text{[math]}$	Initial value of the generalized velocity dof associated with the rigid body $\text{[math]}$ -rotation mode (real). The default value is $\text{[math]}$ .
`RMPT`	Sub-command keyword (characters) for specifying a prescribed, planar, circular trajectory at a constant angular velocity, for the center of gravity of the structural system.
$\text{[math]}$	$\text{[math]}$ -coordinate of the fixed center of the prescribed planar, circular trajectory (real).
$\text{[math]}$	$\text{[math]}$ -coordinate of the fixed center of the prescribed planar, circular trajectory (real).
$\text{[math]}$	$\text{[math]}$ -coordinate of the fixed center of the prescribed planar, circular trajectory (real).
$\text{[math]}$	$\text{[math]}$ -component of the unit axis of rotation of the prescribed, planar, circular trajectory (real).
$\text{[math]}$	$\text{[math]}$ -component of the unit axis of rotation of the prescribed, planar, circular trajectory (real).
$\text{[math]}$	$\text{[math]}$ -component of the unit axis of rotation of the prescribed, planar, circular trajectory (real).
$\text{[math]}$	Constant angluar velocity of the prescribed planar, circular trajectory (real).
`SCAL`	Sub-command keyword (characters) for specifying whether or not to scale the structural deformation modes stored in $\text{[math]}$ by the square root of the total structural mass.
`flagSCAL`	`On`/`Off` flag (characters). The default value is `Off`. Note that if the command `FLOATINGFRAME` is used to construct and output the structural dynamic ROM described above, mass scaling must be disabled for compatibility reasons.
`On`	In this case, the structural deformation modes are scaled by the square root of the total mass of the structural system.
`Off`	In this case, the structural deformation modes are not scaled by the square root of the total mass of the structural system.

97 OUTPUT OF RESULTS (OUTPUT completely spelled out)

The OUTPUT command statement is used to signal that the following lines of data correspond to specifying which results are to be outputted. For vector results such as displacement fields, this command forces AERO-S to output only the three translational components.

The shared memory version of AERO-S generates ASCII output files. Most of these are in a format that is suitable for postprocessing by the XPost software, but some are in a format that is suitable for postprocessing by gnuplot. The distributed memory version of AERO-S generates binary output files except for the case of selective nodal output which it generates in ASCII format. The SOWER software can be used to convert the binary output files into ASCII output files, in a format suitable for postprocessing by XPost. All “nodal” output files are generated in the gnuplot format. Examples using the various OUTPUT commands can be found in FEM.d/fem_examples/Output.d/.

Note 2: The strain and stress outputs are not available for the bar and beam elements, except for STRAINXX and STRESSXX

RESULT [FORMAT] PATHANDFILENAME INCREMENT [

NODE_NUM
BER

] [OPTION] [...] [OPTION]

RESULT [FORMAT] PATHANDFILENAME INCREMENT [N NODE_NUMBER] [OPTION] [...] [OPTION]

RESULT [FORMAT] PATHANDFILENAME INCREMENT [NG GROUP_NUMBER] [OPTION] [...] [OPTION]

`KEYLETTER`	Optional keyletter specifying how to handle gaps in the numbering of nodes as far as output is concerned.
`e`	In this case, the output is expanded — that is, padded with zero(es) at each line corresponding to a gap in the numbering of the nodes. This is the default case. If XPost is to be used for visualizing the results, the geometry of the AERO-S computational model should be converted in this case to the XPost format using the option `-t` or `-m` to perform the same node padding (see INTRODUCTION).
`c`	In this case, no padding is performed, and the output file is ordered according to the ascending order of the freely numbered nodes. If XPost is to be used for visualizing the results, the geometry of the AERO-S computational model should be converted in this case to the XPost format using the option `-T` or `-M` to avoid any node padding (see INTRODUCTION). In summary, the user should note that AERO-S accepts gaps in the number of elements and nodes (free numbering) and performs all computations by accounting for such gaps efficiently. The visualizer XPost can also handle freely numbered nodes and elements; however, for speed purposes, XPost interprets a result as a node-gap-free result. For this reason, if a AERO-S computational model contains gaps in the numbering of the nodes, using XPost for visualizing the computed results requires performing one of the following: Setting `KEYLETTER` to `e` and converting the geometry of the AERO-S computational model to the XPost format using the option `-t` or `-m` (see INTRODUCTION) — in which case the output files will be larger than needed. Setting `KEYLETTER` to `c` and converting the geometry of the AERO-S computational model to the XPost format using the option `-T` or `-M` (see INTRODUCTION) — in which case the output files will not be larger than needed but a different node numbering (more specifically, a compressed version) will be used in the XPost model.
`RESULT`	The following results can be outputted (typically in an ASCII file, unless otherwise noted):
`GDISPLAC`	Nodal displacements. Note that: In the context of the OUTPUT6 command, this result can be used to collect displacement snapshots during a structural dynamic analysis, for example, for the purpose of constructing a Reduced-Order Basis (ROB) for (linear or nonlinear) model reduction (for collecting displacement snapshots for the purpose of constructing a ROB for nonlinear model reduction, see also below the description of the output result `STATEVCT`). Because this result is stored by default in an ASCII input file, it is recommended to output it in this case using a higher precision by setting the optional field `FORMAT` (see below) appropriately, for example, to 21 15. In the context of an online Reduced-Order Model (ROM) simulation and as long as the option `NODE_NUMBER` is not used, this result corresponds to the generalized coordinates of the displacement field. In this case, these generalized coordinates can be transformed into nodal displacements using the RODC command and the keyword `SROM` of the DYNAMICS command. If however in the same context the option `NODE_NUMBER` is used, this result corresponds to the reconstructed high-dimensional displacement at the node specified using `NODE_NUMBER`.
`DISPLACX`	Nodal displacements in the $\text{[math]}$ direction.
`DISPLACY`	Nodal displacements in the $\text{[math]}$ direction.
`DISPLACZ`	Nodal displacements in the $\text{[math]}$ direction.
`ROTATIOX`	Nodal rotations in the $\text{[math]}$ direction.
`ROTATIOY`	Nodal rotations in the $\text{[math]}$ direction.
`ROTATIOZ`	Nodal rotations in the $\text{[math]}$ direction.
`ROVECTOR`	$\text{[math]}$ , $\text{[math]}$ , and $\text{[math]}$ components of the rotation vector.
`ANGVELOC`	$\text{[math]}$ , $\text{[math]}$ , and $\text{[math]}$ components of the angular velocity vector.
`ANGACCEL`	$\text{[math]}$ , $\text{[math]}$ , and $\text{[math]}$ components of the angular acceleration vector.
`DISPLMOD`	Euclidean norms of the nodal displacements.
`ROTATMOD`	Euclidean norms of the nodal rotations.
`GDISPMOD`	Euclidean norms of the generalized nodal displacements.
`GVELOCIT`	Nodal velocities. In the context of an online Reduced-Order Model (ROM) simulation and as long as the option `NODE_NUMBER` is not used, this result corresponds to the generalized coordinates of the velocity field. In this case, these generalized coordinates can be transformed into nodal velocities using the RODC command and the keyword `SROM` of the DYNAMICS command. If however in the same context the option `NODE_NUMBER` is used, this result corresponds to the reconstructed high-dimensional velocity at the node specified using `NODE_NUMBER`.
`GACCELER`	Nodal accelerations. In the context of an online Reduced-Order Model (ROM) simulation and as long as the option `NODE_NUMBER` is not used, this result corresponds to the generalized coordinates of the acceleration field. In this case, these generalized coordinates can be transformed into nodal accelerations using the RODC command and the keyword `SROM` of the DYNAMICS command. If however in the same context the option `NODE_NUMBER` is used, this result corresponds to the reconstructed high-dimensional acceleration at the node specified using `NODE_NUMBER`.
`ROMATRIX`	Rotation matrix representation of nodal rotations (9 components).
`QUATERNI`	Positive unit quaternion representation of nodal rotations (4 components).
`DSVARVCT`	Dual state variables (Lagrange multipliers associated with constraints) collected for nonlinear model reduction of contact problems.
`GTEMPERA`	Nodal temperatures.
`GTEMPVEL`	Nodal first time-derivatives of the temperature.
`GEIGENPA`	Eigenvalues and Eigenvectors. If singular modes are found during an eigen analysis, they are saved in the file FNAME associated with `GEIGENPA` before the non-singular eigen results.
`GEIGSLSH`	Sloshing Eigenvalues and Eigenvectors (displacement potential). If a singular mode is found during the analysis, it is saved in the file FNAME associated with `GEIGSLSH` before the non-singular eigen results.
`SLSHDISP`	True fluid nodal displacements associated with the computed sloshing modes.
`SLSHDSPX`	$\text{[math]}$ component of the true fluid nodal displacements associated with the computed sloshing modes.
`SLSHDSPY`	$\text{[math]}$ component of the true fluid nodal displacements associated with the computed sloshing modes.
`SLSHDSPZ`	$\text{[math]}$ component of the true fluid nodal displacements associated with the computed sloshing modes.
`STRAINXX`	$\text{[math]}$ component of the (total) strain tensor.
`STRAINYY`	$\text{[math]}$ component of the (total) strain tensor.
`STRAINZZ`	$\text{[math]}$ component of the (total) strain tensor.
`STRAINXY`	$\text{[math]}$ component of the (total) strain tensor.
`STRAINYZ`	$\text{[math]}$ component of the (total) strain tensor.
`STRAINZX`	$\text{[math]}$ component of the (total) strain tensor.
`STRAINVM`	von Mises strain.
`EFFPSTRN`	Effective plastic strain.
`STRAINP1`	First principal strain.
`STRAINP2`	Second principal strain.
`STRAINP3`	Third principal strain.
`PLSTRNXX`	$\text{[math]}$ component of the plastic strain tensor.
`PLSTRNYY`	$\text{[math]}$ component of the plastic strain tensor.
`PLSTRNZZ`	$\text{[math]}$ component of the plastic strain tensor.
`PLSTRNXY`	$\text{[math]}$ component of the plastic strain tensor.
`PLSTRNYZ`	$\text{[math]}$ component of the plastic strain tensor.
`PLSTRNZX`	$\text{[math]}$ component of the plastic strain tensor.
`EP1DIREC`	Direction of first principal strain.
`EP2DIREC`	Direction of second principal strain.
`EP3DIREC`	Direction of third principal strain.
`STRESSXX`	$\text{[math]}$ component of the second-Piola stress tensor.
`STRESSYY`	$\text{[math]}$ component of the second-Piola stress tensor.
`STRESSZZ`	$\text{[math]}$ component of the second Piola stress tensor.
`STRESSXY`	$\text{[math]}$ component of the second Piola stress tensor.
`STRESSYZ`	$\text{[math]}$ component of the second Piola stress tensor.
`STRESSZX`	$\text{[math]}$ component of the second Piola stress tensor.
`STRESSVM`	(Second Piola) von Mises stress.
`STRESSP1`	(Second Piola) first principal stress.
`STRESSP2`	(Second Piola) second principal stress.
`STRESSP3`	(Second Piola) third principal stress.
`SP1DIREC`	Direction of first principal stress.
`SP2DIREC`	Direction of second principal stress.
`SP3DIREC`	Direction of third principal stress.
`BKSTRSXX`	$\text{[math]}$ component of the back stress tensor.
`BKSTRSYY`	$\text{[math]}$ component of the back stress tensor.
`BKSTRSZZ`	$\text{[math]}$ component of the back stress tensor.
`BKSTRSXY`	$\text{[math]}$ component of the back stress tensor.
`BKSTRSYZ`	$\text{[math]}$ component of the back stress tensor.
`BKSTRSZX`	$\text{[math]}$ component of the back stress tensor.
`ELEMDELE`	List of elements deleted from the finite element model by the element deletion method, and time at which they were deleted. This output file can be used for post-processing using xp2exo/ParaView.
`DAMAGESC`	Scalar damage parameter which is equal to 1 when an element is completely damaged and therefore deleted from the finite element model by the element deletion method, and to 0 when the element is not damaged.
`HEATFLXX`	Temperature flux along the $\text{[math]}$ direction.
`HEATFLXY`	Temperature flux along the $\text{[math]}$ direction.
`HEATFLXZ`	Temperature flux along the $\text{[math]}$ direction.
`GRDTEMPX`	Temperature gradient along the $\text{[math]}$ direction.
`GRDTEMPY`	Temperature gradient along the $\text{[math]}$ direction.
`GRDTEMPZ`	Temperature gradient along the $\text{[math]}$ direction.
`INXFORCE`	Internal forces along the element $\text{[math]}$ -axis. This output result is supported only for bar and beam elements.
`INYFORCE`	Internal forces along the element $\text{[math]}$ -axis. This output result is supported only for bar and beam elements.
`INZFORCE`	Internal forces along the element $\text{[math]}$ -axis. This output result is supported only for bar and beam elements.
`AXMOMENT`	Internal moments along the element $\text{[math]}$ -axis. This output result is supported only for beam elements.
`AYMOMENT`	Internal moments along the element $\text{[math]}$ -axis. This output result is supported only for beam elements.
`AZMOMENT`	Internal moments along the element $\text{[math]}$ -axis. This output result is supported only for beam elements.
`ENERGIES`	External, Aeroelastic, Elastic, Kinetic, Dissipative, and Numerical Production energies. The Numerical Production energy corresponds to the energy conservation error for a conservative system. When positive, it suggests a numerically unstable scheme. When negative, it suggests the presence of numerical damping in the scheme. Using the standard notation and that of the `DYNAMICS` section, these energies are computed as follows (note that in the formulae given below, summation is performed over the outputted time-steps):

	$\text{[math]}$	$\text{[math]}$
	$\text{[math]}$	$\text{[math]}$
	$\text{[math]}$	$\text{[math]}$ $\text{[math]}$
	$\text{[math]}$	$\text{[math]}$
	$\text{[math]}$	$\text{[math]}$ $\text{[math]}$
	$\text{[math]}$	Kinetic - Previous_Kinetic + Elastic - Previous_Elastic + Increment_Dissipative_Between_Previous_and_Current - Increment_Exterior_Between_Previous_and_Current

`DISSIPAT`	Dissipative energy corresponding to $\text{[math]}$ in the output of `ENERGIES` (see above). When the computational model contains both material dissipation and structural damping (e.g. Rayleigh damping), the output `ENERGIES` includes a report on their combination. This output result reports on material dissipation separately.
`AEROFORX`	Aeroelastic nodal forces along the $\text{[math]}$ direction at $\text{[math]}$ , after application of the boundary conditions (see DYNAMICS).
`AEROFORY`	Aeroelastic nodal forces along the $\text{[math]}$ direction at $\text{[math]}$ , after application of the boundary conditions (see DYNAMICS).
`AEROFORZ`	Aeroelastic nodal forces along the $\text{[math]}$ direction at $\text{[math]}$ , after application of the boundary conditions (see DYNAMICS).
`AEROMOMX`	Aeroelastic nodal moments along the $\text{[math]}$ direction at $\text{[math]}$ , after application of the boundary conditions (see DYNAMICS).
`AEROMOMY`	Aeroelastic nodal moments along the $\text{[math]}$ direction at $\text{[math]}$ , after application of the boundary conditions (see DYNAMICS).
`AEROMOMZ`	Aeroelastic nodal moments along the $\text{[math]}$ direction at $\text{[math]}$ , after application of the boundary conditions (see DYNAMICS).
`RAEROFOR`	Aeroelastic resultant forces along the $\text{[math]}$ , $\text{[math]}$ , and $\text{[math]}$ directions (integrated over the wet surface of the structure) at $\text{[math]}$ , before application of the boundary conditions (see DYNAMICS).
`RAEROTFL`	Fluid heat fluxes transferred to the structure at $\text{[math]}$ .
`GHELMHOL`	Real or complex acoustic pressure scattered field computed by an acoustic analysis in the frequency domain. The real part is always output first, then, if it is non uniformly zero, the imaginary part is output as a separate frame but in the same output file.
`GACOUPRE`	Nodal values of the acoustic pressure computed by an acoustic analysis in the time domain.
`GACOUVEL`	Nodal values of the first time-derivative of the acoustic pressure computed by an acoustic analysis in the time domain.
`GACOUACC`	Nodal values of the second time-derivative of the acoustic pressure computed by an acoustic analysis in the time domain.
`KIRCHHOFF`	Acoustic pressure field at locations specified using the KIRLOC command and evaluated using the Kirchhoff integral. This result can be outputted only if the surface of the scatterer is defined using the command HSCB. The corresponding output file contains on each line five words of the form: X-ORDINATE_I Y-ORDINATE_I Z-ORDINATE_I REAL(U_I) IMAG(U_I). X, Y, and Z-ORDINATE_I are the X, Y, and Z coordinates of the I-th point specified using the command KIRLOC. REAL(U_I) and IMAG(U_I) are the real and imaginary parts of the acoustic pressure field computed at the I-th specified point using the Kirchhoff integral method.
`FARFIELD`	Farfield pattern of the acoustic pressure field. This field can be output only if the HSCB command is also specified. In this case, the output file contains on each line four words of the form “ $\text{[math]}$ , $\text{[math]}$ , real-part(ffp), imaginary-part(ffp)”. The first two quantities are the spherical angles (expressed in radians) that determine the direction $\text{[math]}$ . The number of output lines depends on the parameter `INCREMENT` (see below).
`GENCOORD`	Projections of a transient solution onto a modal or other basis specified via the MODE command. This field can be outputted only during a linear dynamic analysis without mesh decomposition, and if the MODE command is also specified in the ASCII Input Command Data file.
`MODERROR`	Relative truncation error using the two-norm of the representation of a transient solution by its projection onto a modal or other basis specified via the MODE command. This field can be outputted only during a linear dynamic analysis without a mesh decomposition, and if the MODE command is also specified.
`MODALDSP` or `SROMDISP`	Modal displacement coefficients or generalized displacements, when dynamics computations are done in a modal or other Reduced-Order Basis (ROB). This result can be outputted only during a linear dynamic analysis.
`MODALEXF` or `SROMEXTF`	Modal external forces coefficients or generalized external forces, when structural dynamics computations are done in a modal basis. This result can be outputted only during a linear dynamic analysis.
`CONPRESS`	Contact pressure forces (Lagrange multipliers in the normal directions).
`CONFACE`	Denotes the status of interactions at a node. A value of 0.5 indicates the node is not in contact. A value of 1, 2, or 3 denotes the number of interactions at that node.
`NORMAL_FORCE_MAG`	Normal force magnitude at a node. If multiple constraints exist at a node, the value is for the last constraint.
`NORMAL_TRACTION_MAG`	Normal traction magnitude at a node. If multiple constraints exist at a node, the value is for the last constraint.
`TANGENTIAL_FORCE_MAG`	Tangential force magnitude at a node. If multiple constraints exist at a node, the value is for the last constraint.
`TANGENTIAL_TRACTION_MAG`	Tangential traction magnitude at a node. If multiple constraints exist at a node, the value is for the last constraint.
`CDIRNORX`	x component of the normal direction for the constraint at a node. If multiple constraints exist at a node, the value is for the last constraint.
`CDIRNORY`	y component of the normal direction for the constraint at a node. If multiple constraints exist at a node, the value is for the last constraint.
`CDIRNORZ`	z component of the normal direction for the constraint at a node. If multiple constraints exist at a node, the value is for the last constraint.
`CDIRTANX`	x component of the tangential direction for the constraint at a node. If multiple constraints exist at a node, the value is for the last constraint.
`CDIRTANY`	y component of the tangential direction for the constraint at a node. If multiple constraints exist at a node, the value is for the last constraint.
`CDIRTANZ`	z component of the tangential direction for the constraint at a node. If multiple constraints exist at a node, the value is for the last constraint.
`SLIP_MAG`	Incremental slip at a node. If multiple constraints exist at a node, the value is for the last constraint.
`NODAL_DISSIPATION`	Frictional energy dissipated at a node.
`CONTACT_AREA`	Contact area for a node.
`GAP_CUR`	Normal gap for the current time. If multiple constraints exist at a node, the value is for the last constraint.
`GAP_OLD`	Normal gap from the previous time. If multiple constraints exist at a node, the value is for the last constraint.
`REACTION`	Reaction forces and moments along all three orthogonal directions.
`HEATREAC`	Thermal reaction sources.
`VMSTTHIC`	Nodal sensitivities of the von Mises stress with respect to all thickness variables specified in SENSITIVITY (column by column).
`WEIGTHIC`	Sensitivities of the total weight of the structural model with respect to all thickness variables specified in SENSITIVITY (row by row).
`VMSTSHAP`	Nodal sensitivities of the von Mises stress with respect to all shape (design) variables (column by column).
`VMSTMACH`	For an aeroelastic computation, nodal sensitivities of the von Mises stress with respect to the Mach number.
`VMSTALPH`	For an aeroelastic computation, nodal sensitivities of the von Mises stress with respect to the sideslip angle of attack.
`WEIGSHAP`	Sensitivities of the total weight of the structural model with respect to all shape variables (row by row).
`STATEVCT`	Snapshots of the state vector (displacements) stored in a binary file. They can be used, for example, for constructing a ROB for the purpose of (linear or nonlinear) model reduction. Currently, this result can be outputted only during a nonlinear structural dynamic analysis. During a linear structural dynamic analysis, displacement snapshots can be collected in the result `GDISPLAC` using the OUTPUT6 command. Because in this case the displacement snapshots are stored in an ASCII file, it is recommended to output them using a higher precision by setting the optional field `FORMAT` appropriately, for example, to 21 15.
`NODALCOO`	Nodal coordinates of the finite element mesh stored in a binary file. They can be used, for example, for constructing one or multiple (hyper) reduced meshes using the `NDSCFG` sub-command keyword of the RMSHC command.
`VELOCVCT`	Snapshots of the velcity vector (velocities). Currently, this result can be outputted only during a nonlinear structural dynamics analysis.
`ACCELVCT`	Snapshots of the vector of accelerations. Currently, this result can be outputted only during a nonlinear structural dynamics analysis.
`FRCNGVCT`	Snapshots of the vector of external forces. Currently, this result can be outputted only during a nonlinear structural dynamics analysis.
`ROMRESID`	Residual associated with a ROM-based approximate solution defined by a Reduced-Order Basis (ROB) inputted using the READMODE command and (time-dependent) generalized coordinates inputted using the RODC command. Currently, this result can be outputted only during a nonlinear structural dynamics analysis.
`ROMEXTFO`	Contribution of the (possibly configuration-dependent) external forces to the residual associated with a ROM-based approximate solution defined by a Reduced-Order Basis (ROB) inputted using the READMODE command and (time-dependent) generalized coordinates inputted using the RODC command. Currently, this result can be outputted only during a nonlinear structural dynamics analysis.
`ROBDATAF`	Prefix of the two binary files containing both instances of the Reduced-Order Basis (ROB) generated by the ROBC command (see in ROBC the `MNORMA` sub-command keyword). If this ROB is a primal ROB, its orthonormalized instance is outputted in the file `<PATHANDFILENAME.orthonormalized>`, and its mass-orthonormalized counterpart is outputted in the file `<PATHANDFILENAME.massorthonormalized>`. To this effect, note that when inputting this ROB in READMODE using the first format of this command, the extension "`.massnormalized`" can be omitted from `<pathandfilename>` as it will be internally added by AERO-S. On the other hand, when inputting this ROB in READMODE using the second format of this command, `<pathandfilename_i>` must be set to the name of the file containing the mass-orthonormalized version of this ROB unless `rob_type_i` is set to `inorm`. If this ROB is a dual ROB, and there can be more than one basis computed (see `numrob` in ROBC), each ROB is outputted in a separate file labeled `<PATHANDFILENAME>.int`, where `int` is the integer indicating the dimension of the ROB (recall that when multiple ROBs are computed, they have monotonically increasing/decreasing dimensions).
`SAMPLMSH`	This result consists of three files or sets of files: A file named `<PATHANDFILENAME>`, containing the attributes of the original mesh and therefore all sampling weights needed for performing a hyper reduction, if computed using the RMSHC command. Specifically, it is outputted as an inclusive list of element attributes and their corresponding hyper reduction coefficients (or weights) (see ATTRIBUTES). In the case of local ROBs, one such file is outputted for each local basis and the extension `.cluster<local_basis_id>` is appended to the filename `<PATHANDFILENAME>`. Another file named `<PATHANDFILENAME>.elementmesh.inc` containing the reduced mesh as well as that part of the high-dimensional model needed for constructing the corresponding hyper reduced projection-based reduced-order model – that is: The reduced mesh and its weights. The attributes and material properties of the elements of the reduced mesh. Initial reduced-order displacement and/or velocity conditions or hyper reduced counterparts, if the corresponding command(s) is/are included in the same input file containing RMSHC and the latter command is properly configured. The constant reduced-order mass matrix, when the ROB is not mass-orthonormalized (see READMODE); and the flag `flag_cmf` was set to `Off` in the command RMSHC that generated the content of the file `<PATHANDFILENAME>.elementmesh.inc`. Reduced-order external, constant (non-follower) forces, if the corresponding command(s) is/are included in the same input file containing RMSHC. Reduced-order linear multipoint constraints (see LMPC), if the corresponding command is included in the same input file containing RMSHC. In the case of local ROBs, the above information is outputted for each (training) local ROB in the same output file `<PATHANDFILENAME>.elementmesh.inc`. Note: When considering an online computation using a hyperreduced ROM, the user should include in the corresponding ASCII Input Command Data file the aforementioned file `<PATHANDFILENAME>.elementmesh.inc` using an `INCLUDE` statement (see INTRODUCTION). And a third file containing the trace on the reduced mesh of its training ROB: this file is named `<PATHANDFILENAME>.elementmesh.inc.compressed.basis.massorthonormalized`, if the training ROB is mass-orthonormalized; otherwise, it is named `<PATHANDFILENAME>.elementmesh.inc.compressed.basis`. In the case of local ROBs, one such file is outputted for each local basis and the extension `<local_basis_id>` is inserted in the filename `<PATHANDFILENAME>.elementmesh.inc.compressed.basis.massorthonormalized` after the word `basis`, or appended to the filename `<PATHANDFILENAME>.elementmesh.inc.compressed.basis`. The format of each of the above files is designed to allow their inclusion in AERO-S's input file using `INCLUDE` (see INTRODUCTION).
`MODALMAS` or `SROMMASS`	ASCII file containing the reduced-order mass matrix associated with a structural dynamic ROM. In the case of a nonlinear structural dynamic ROM constructed in a floating reference frame attached to the center of gravity of the structural system (see FLOATINGFRAME), this reduced-order mass matrix corresponds to the matrix block $\text{[math]}$ . If the Reduced-Order Basis (ROB) underlying the linear structural ROM is of the type `inorm` or `nnorm`, this file is outputted in the following format * Mr: Full reduced mass matrix inorm (or nnorm) n n Mr11 Mr12 ... Mr1n Mr21 Mr22 ... Mr2n . . . Mrn1 Mrn2 ... Mrnn where n denotes the size of the linear or nonlinear structural dynamics ROM. If the ROB underlying the linear structural ROM is of the type `mnorm` (or `eigen`), this file is outputted in the following format * Mr: Diagonal reduced mass matrix mnorm (or eigen) n Mr11 Mr22 ... Mrnn where n denotes the size of the linear or nonlinear structural dynamics ROM.
`MODALDMP` or `SROMDAMP`	ASCII file containing the reduced-order damping matrix associated with a linear structural ROM. This file is outputted in the format described below. * Dr: Reduced damping matrix n n Dr11 Dr12 ... Dr1n Dr21 Dr22 ... Dr2n . . . Drn1 Drn2 ... Drnn where n denotes the size of the linear structural dynamics ROM. This file is outputted if: The ROB underlying the linear structural ROM is of the type `eigen` (see READMODE), and damping in the underlying HDM is modeled in DYNAMICS as modal damping (`MODDAMP`) or Rayleigh damping (`RAYDAMP`). The ROB underlying the linear structural ROM is of the type `mnorm`, `inorm`, or `nnorm` (see READMODE), and damping in the underlying HDM is modeled in DYNAMICS as Rayleigh damping (`RAYDAMP`).
`MODALSTF` or `SROMSTIF`	ASCII file containing the reduced-order stiffness matrix associated with a structural ROM. In the case of a nonlinear structural dynamic ROM constructed in a floating reference frame attached to the center of gravity of the structural system (see FLOATINGFRAME), this reduced-order mass matrix corresponds to the matrix block $\text{[math]}$ . If the Reduced-Order Basis (ROB) underlying the linear structural ROM is of the type `inorm`, `mnorm`, or `nnorm`, this file is outputted in the following format * Kr: Full reduced stiffness matrix inorm (mnorm or nnorm) n n Kr11 Kr12 ... Kr1n Kr21 Kr22 ... Kr2n . . . Krn1 Krn2 ... Krnn where n denotes the size of the linear structural ROM. If the ROB underlying the linear structural ROM is of the type `eigen`, this file is outputted in the following format * Kr: Diagonal reduced stiffness matrix eigen n Kr11 Kr22 ... Krnn where n denotes the size of the linear structural dynamics ROM.
`SROMMATR`	ASCII file containing the reduced-order mass, damping, and stiffness matrices associated with a (linear) structural dynamics ROM. This file is essentially the union of all 3 files associated with the results `MODALMAS` or `SROMMASS`, `MODALDMP` or `SROMDAMP`, and `MODALSTF` or `SROMSTIF`.
`MODALACT` or `SROMACTU`	ASCII file containing the reduced-order displacement, velocity, and acceleration control matrices associated with a linear structural dynamics ROM and three gain variables (displacement, velocity, and acceleration) of an output feedback control law defined using the user-defined subroutine "control.C", ACTUATORS, and SENSORS. This file is outputted in the format described below. * Dr: Full reduced-order displacement control matrix rob_type n n - n: size of the linear structural dynamics ROM Dr11 Dr12 ... Dr1n Dr21 Dr22 ... Dr2n . . . Drn1 Drn2 ... Drnn * Vr: Full reduced-order velocity control matrix rob_type n n - n: size of the linear structural dynamics ROM Vr11 Vr12 ... Vr1n Vr21 Vr22 ... Vr2n . . . Vrn1 Vrn2 ... Vrnn * Mr: Full reduced-order acceleration control matrix rob_type n n - n: size of the linear structural dynamics ROM Ar11 Ar12 ... Ar1n Ar21 Ar22 ... Ar2n . . . Arn1 Arn2 ... Arnn
`MODALFLF`	This output result is relevant only when the simulation is performed using a nonlinear structural dynamic ROM constructed in a floating reference frame attached to the center of gravity of the structural system (see FLOATINGFRAME). In this case, this is the ASCII file containing the projection-based, reduced-order coupling tensors required to evaluate the generalized gyroscopic damping forces associated with the nonlinear structural dynamic ROM. It is outputted in the following format * B_p[0][0]: Full reduced-order fourth-order tensor 3 3 B_p[0][0]11 B_p[0][0]12 B_p[0][0]13 B_p[0][0]21 B_p[0][0]22 B_p[0][0]23 B_p[0][0]31 B_p[0][0]32 B_p[0][0]33 repeat for B_p[0][1], ..., B_p[0][n-1], B_p[1][0], ..., B_p[1][n-1], ..., B_p[n-1][n-1] * B_t[0]: Full reduced-order third-order tensor n 3 B_t[0]11 B_t[0]12 B_t[0]13 B_t[0]21 B_t[0]22 B_t[0]23 ... B_t[0]n1 B_t[0]n2 B_t[0]n3 repeat for B_t[1], ..., B_t[n-1] * B_h[0]: Full reduced-order third-order tensor 3 3 B_h[0]11 B_h[0]12 B_h[0]13 B_h[0]21 B_h[0]22 B_h[0]23 B_h[0]31 B_h[0]32 B_h[0]33 repeat for B_h[1], ..., B_h[n-1] where $\text{[math]}$ denotes the number of flexible modes of the structural dynamic system.
`FORMAT`	This optional field can be used to override the default format for outputting a numerical value by one which consists of 2 integer numbers F and P separated by a blank (integers). F specifies the field width — that is, the total number of digits to be printed including the decimal point, the "E" of the exponent and the sign of the exponent, but excluding the sign of the output value. P is the number of digits after the decimal and before the exponent. For example, 8 2 results in printing the output value 1523 as 0.15E+03.
`FNAME`	User specified filename associated with result (characters).
`INCREMENT`	Output increment for transient and eigenvalue results (integer). For a `FARFIELD` output result, this field specifies, in the three-dimensional case, the number of longitudinal directions where the farfield is to be evaluated. In this case, (`INCREMENT`/2)+1) latitudinal directions are also considered and therefore the farfield is evaluated at ((`INCREMENT`/2)+1))*`INCREMENT` points uniformly distributed in spherical coordinates. In two-dimensions, the farfield is evaluated at `INCREMENT` points that are evenly distributed on a circle. For transient and quasi-static analyses, the final time-instance is always outputted for the requested fields — except for the aeroelastic forces and moments — independently of the value of `INCREMENT`.
`N`	Sub-command keyword (character) signaling that the next entry is a node identifying number.
`NODE_NUMBER`	When this optional field is used, with or without the sub-command keyword `N`, only the computed results associated with the node NODE_NUMBER are outputted in the same format as otherwise, except that the header of the XPost file is omitted for easier use of a visualization software such as gnuplot (integer).
`NG`	Sub-command keyword (characters) signaling that the next entry is a group identifying number (see GROUPS).
`GROUP_NUMBER`	When this optional field is used together with the sub-command keyword `NG`, only the computed results associated with the nodes belonging to the group of nodes `GROUP_NUMBER` (see GROUPS) are outputted in the following format which is suitable for a visualization software such as gnuplot (integer). FLOAT-1 NODE_NUMBER-1 X Y Z RESULT-1 RESULT-2 ... RESULT-n NODE_NUMBER-2 X Y Z RESULT-1 RESULT-2 ... RESULT-n ... FLOAT-2 NODE_NUMBER-1 X Y Z RESULT-1 RESULT-2 ... RESULT-n NODE_NUMBER-2 X Y Z RESULT-1 RESULT-2 ... RESULT-n ... where FLOAT-i is an $\text{[math]}$ -th time-instance in the case of a dynamic analysis or a circular frequency value (number of cycles per second) in the case of a frequency sweep analysis (see IMPEDANCE), NODE_NUMBER-j is the $\text{[math]}$ -th node number of group `GROUP_NUMBER`, X, Y and Z are the $\text{[math]}$ , $\text{[math]}$ , and $\text{[math]}$ coordinates of NODE_NUMBER-j, and RESULT-1 RESULT-2 ... RESULT-n are all the computed results pertaining to NODE_NUMBER-j and the chosen instance of `RESULT`.
`OPTION`	Any of the following optional fields can be specified after the previous optional and/or non-optional entries documented above:
`NDTYPE` [`NUM_OUT_RLZ`]	`NDTYPE` is an optional parameter that can take one of the following values: `MEAN`, `STDV`, or `PDF`. It should be used only when an intrusive or non intrusive non deterministic analysis is performed. When `MEAN` is selected and a non intrusive non deterministic analysis is performed, the mean value of the `RESULT` is outputted using the number of realizations `NUM_RLZ` specified in the `NONINPC` command. When `STDV` is chosen and a non intrusive non deterministic analysis is performed, the standard deviation of the `RESULT` is outputted using the number of realizations `NUM_RLZ` specified in the `NONINPC` command. When `PDF` is specified, the probability density function is outputted using a number of realizations equal to the integer set in the suboptional field `NUM_OUT_RLZ` (integer). First, the shape functions are evaluated at `NUM_OUT_RLZ` realizations of the random system. Then, `NUM_OUT_RLZ` realizations of the non deterministic `RESULT` are reconstructed from these evaluations using $\text{[math]}$ in the case of a displacement or $\text{[math]}$ in the case of a stress field $\text{[math]}$ and written in the output file (note that the case of a von Mises stress is treated slightly differently because it is a nonlinear function of the stress tensor components). A histogram can be constructed from these results.
`AVG_OPTION`	If the output of a stress field, strain field, or the damage parameter field `DAMAGESC` is requested, the user can set this optional parameter to one of the following values: `NODALFULL`, `NODALPARTIAL`, `NODALPARTIALGROUP`, `ELEMENTAL`, or `GAUSS` (characters), to specify a type of stress/strain/damage averaging. If `NODALFULL` is specified, the target field is averaged at each node using all elements attached to this node. In this case, the contributions of the beam and bar elements are first transformed to the global frame. If `NODALPARTIAL` is specified, the averaging is performed using only the elements that are neither of a bar or a beam type. If `NODALPARTIALGROUP` is specified and the keyword `NG` is used to activate output for a group of nodes, the averaging is performed using only those elements whose nodes belong to the specified group. If `ELEMENTAL` is specified, the field is outputted without any averaging at each node of each element. Note however that currently, the option `ELEMENTAL` is not supported when a FETI solver is invoked. If `GAUSS` is specified, the target field is outputted without any averaging at each Gauss point of each element. This latter option is currently supported however only for nonlinear analysis using three-dimensional solid elements (type 17, 23, 24, 25, 72, 91, 92 and 94) for which constitutive laws are specified using MATLAW.
`STR_TYPE_OPTION`	This optional field is applicable only for linear analyses. It can have any of the following settings: `THERMAL`, `MECHANICAL`, or `THERMOMECHANICAL` (default setting). In the first case, the computed and outputted stresses are the thermal stresses defined as $\text{[math]}$ , where $\text{[math]}$ is the pertaining constitutive matrix, $\text{[math]}$ is the thermal expansion coefficient specified in MATERIAL, $\text{[math]}$ is the temperature (absolute), and $\text{[math]}$ is the ambient (reference) temperature (absolute) also specified in MATERIAL. In the second case, the computed and outputted stresses are the mechanical stresses defined as $\text{[math]}$ , where $\text{[math]}$ is the strain tensor. In the last case, which is the default setting, the computed and outputted stresses are the thermomechanical stresses defined as $\text{[math]}$ .
`STR_SHELL_OPTION`	This optional field is applicable only when the output of a stress/strain field of a shell element is requested. It can take any of the following values `UPPER, MEDIAN, LOWER` (characters). If `UPPER` is specified, the stresses are computed on the upper surface of the element. If `MEDIAN` is specified (default value), they are computed on the median surface of the element. If `LOWER` is specified, they are computed on the lower surface of the element.
`STR_BEAM_OPTION`	This optional field is applicable only when the output of `STRAINXX` or `STRESSXX` of a beam element is requested. It specifies two real numbers (real). The first (second) real number represents the positive or negative `y` (`z`) coordinate in percentage of the maximum positive (top fiber) or negative (bottom fiber) `y` (`z`) coordinate of the beam cross section, in the local frame attached to the beam, of the fiber at which $\text{[math]}$ or $\text{[math]}$ is requested. The default value for both real numbers is zero.
`COMPLEX_OUTPUT_OPTION` [`NSTEPS`]	These optional and suboptional fields are applicable only when the output is complex-valued. `COMPLEX_OUTPUT_OPTION` can take any of the following values `REALIMAG, MODPHASE, ANIM` (characters). When set to `REALIMAG`, the real parts of the complex-valued output are printed first and the imaginary parts are printed next. When set to `MODPHASE`, the moduli $\text{[math]}$ of the output values are first printed and then the phases $\text{[math]}$ are printed. When set to `ANIM`, the values of $\text{[math]}$ are printed first, followed by the values of $\text{[math]}$ , etc, concluding with the values of $\text{[math]}$ , where $\text{[math]}$ is defined as $\text{[math]}$ and $\text{[math]}$ is specified in the suboptional field `NSTEPS` (integer).
`FRM_OPTION`	This optional parameter can be used to request outputting directional results (such as, for example, the $\text{[math]}$ , $\text{[math]}$ and $\text{[math]}$ components of a computed displacement field, or the $\text{[math]}$ component of a computed stress field) in the nodal reference frames defined at the nodes of the finite element model, in the global reference frame, or in the material reference frame. In the first case, this parameter should be set to `NODFRA`. In the second case, its should be set to `GLOFRA`. In the third case, it should be set to `MATFRA`. Its default value is `GLOFRA`. For this reason, when outputting a directional result to be reused with the READMODE command, this parameter should be set to `NODFRA`.
`ORTHONORM_OPTION`	This optional field is applicable only when the result to be outputted is `GEIGENPA`. It specifies whether to output the computed mass-orthonormalized eigenvectors or associated orthonormalized vectors (characters). Hence, it can take one of the two following values:
`mnorm`	In this case, which is the default case, the computed mass-orthonormalized eigenvectors are outputted.
`inorm`	In this case, (identity-) orthonormalized vectors that span the same subspace as the mass-orthonormalized eigenvectors are outputted.
`ROTVEC_OPTION`	This optional parameter can be used to select the specific type of rotation vector output for `GDISPLAC` (only under OUTPUT6), `ROTATIOX`, `ROTATIOY`, `ROTATIOZ`, `ROTATMOD`, and `GDISPMOD`. It can can take values `Euler` (default value), `Complement`, `Linear`, `ReducedEulerRodrigues`, `CayleyGibbsRodrigues`, `WienerMilenkovic`, or `BauchauTrainelli`. The default `Euler` rotation vector, also known as the axis-angle representation, is a vectorial parameterization of the rotation group whose magnitude is the (scalar) rotation angle $\text{[math]}$ and rotation axis is the unit 3-vector $\text{[math]}$ — that is, $\text{[math]}$ . This is not to be confused with non-vectorial Euler angles for the parameterization of rotation. The complement rotation vector is specifically the complement of the Euler rotation vector and corresponds to a rotation angle of ( $\text{[math]}$ ) about the axis $\text{[math]}$ . For details about the other options, refer to The vectorial parameterization of rotation, by Bauchau and Trainelli, in Nonlinear Dynamics, 32, No 1, pp. 71–92, 2003. Regardless of the value of `ROTVEC_OPTION`, the rotation vector is a representation of the "total rotation" — that is, it is measured with respect to the reference orientation (which corresponds in AERO-S to the case where the rotation matrix is the identity matrix).
`ORTHONORM_OPTION`	This optional field is applicable only when the result to be outputted is `GEIGENPA`. It specifies whether to output the computed mass-orthonormalized eigenvectors or associated orthonormalized vectors (characters). Hence, it can take one of the two following values:
`mnorm`	In this case, which is the default case, the computed mass-orthonormalized eigenvectors are outputted.
`inorm`	In this case, (identity-) orthonormalized vectors that span the same subspace as the mass-orthonormalized eigenvectors are outputted.
`RESCALING` `FLAG`	Optional sub-command keyword followed by an `On` or `Off` flag which can be used to define whether or not to rescale the rotation vector – which is a one-to-many mapping from the rotation matrix. It applies to `GDISPLAC`, `GVELOCIT`, and `GACCELER` under OUTPUT6, and to `ROTATIOX`, `ROTATIOY`, `ROTATIOZ`, `ROTATMOD`, and `GDISPMOD`. The default value of `FLAG` is `On`. The specific interpretation of this option depends on the setting of `ROTVEC_OPTION`. For example, in the case of an Euler rotation vector, setting `FLAG` to `On` means that the outputted rotation vector is that with a rotation angle $\text{[math]}$ . When the rotation vector is rescaled, its components become discontinuous at the point of rescaling. Otherwise, its components may be discontinuous at certain singularity points ( $\text{[math]}$ in the case of the Euler rotation vector).
`ANGULAR_OPTION`	This optional parameter can be used to choose a definition of the angular velocity or acceleration for `GVELOCIT` or `GACCELER` under OUTPUT6. It can take the following values: `Convected` (default), `Spatial`, and `Total`. The `Convected` definition refers to a moving frame that is computed by AERO-S and attached to each node. The definition `Spatial` refers to the fixed reference frame, and the definition `Total` refers to the time derivatives of the (Euler) rotation vector. In the case of `Total`, the `RESCALING` option may also be used to specify whether the angular velocity (acceleration) is the first (second) time derivative of the rescaled or non-rescaled Euler rotation vector. Note that angular velocities and accelerations inputted using `IVEL` or USDD should be `Convected`.

98 OUTPUT OF RESULTS 6 COLUMNS (OUTPUT6 completely spelled out)

The OUTPUT6 command has the same options and format of the OUTPUT command. Its outcome differs from that of OUTPUT only when vector results such as generalized displacements fields are to be outputted. In that case, the OUTPUT6 command forces AERO-S to output all six components of the generalized displacement field in a format slightly different from that of the file created by OUTPUT, in that the node number is included at the beginning of each line.

99 PARALLEL-IN-TIME ALGORITHM (PITA)

The PITA command statement is used to request the parallelization in time of the time-integration algorithm specified under the DYNAMIC command. This option is supported only when executing the distributed version of the AERO-S executable. The simultaneous presence of the command statement NONLINEAR in the input file automatically triggers the nonlinear version of the PITA algorithm. By default, the initialization of the time-slices is performed by running the chosen time-integrator on the coarse time-grid. Alternatively, the IDISP6PITA (see IDISP6PITA) and IVEL6PITA (see IVEL6PITA) commands can be used to specify the seed displacements and velocities. The imput format is given below.

Note 2: The foundations of the PITA methodology are described in: J. Cortial, Time-Parallel Methods for Accelerating the Solution of Structural Dynamics Problem, PhD Thesis, Stanford University, 2011.

`J_RATIO`	Ratio between the time-steps on the fine and coarse time-grids. Also, number of time-steps in each time-slice (integer).
`MAX_ITER`	Maximum number of outer PITA iterations (integer).
`MAX_SLICES_ON_CPU`	Maximum number of time-slices assigned to a processor (integer). If the number of time-slices is larger than the number of available CPUs, the supernumerary time-slices are ignored. For optimal performance, there should be as many available CPUs as time-slices. The default value is 1.
`PITA_OPTIONS`	None, one or several of the following optional statements
`TIMEREVERSIBLE`	Instructs AERO-S to exploit the time-reversibility of the problem. In this case, each time-slice is divided into 2 halves, one treated by usual forward-in-time integration, and the other by backward-in-time integration. For optimal performance, 2 CPUs should be assigned to each time-slice.
`ORTHOPROJTOL` `orthoprojtol`	Sets the relative tolerance used to construct the orthogonal projectors for the correction step. The default value is $\text{[math]}$ .
`READINITSEED`	Instructs AERO-S to use the initial seed information provided via the commands IDISP6PITA and IVEL6PITA. If additional seed values are required, they are obtained in this case via time-integration on the coarse time-grid.
`REMOTECOARSE`	Instructs AERO-S to perform the coarse time-grid integration on a dedicated CPU, which will not be available during the parallel integration on the fine-time grid (linear case only). For optimal performance in the linear case, it is recommended to use this option and provide one additional CPU. This command is ignored when only one CPU is available.
`NOFORCE`	Informs AERO-S about the absence of any external force so that a special version of the PITA can be executed for optimal performance (linear case only).
`JUMPCVG` `jumpcvg`	Instructs AERO-S to enable the jump-reduction-based convergence criterion with the specified tolerance `jumpcvg` (linear case only). The default value is `J_RATIO` $\text{[math]}$ .
`GLOBALBASES` `integer`	Determines the scheme to use for updating the global bases using the following convention: 1 = all seed vectors, 2 = all seed and propagated vectors (nonlinear case only). The default value is 1.
`LOCALBASES`	Instructs AERO-S to use the local basis updating scheme instead of the global one (nonlinear case only). This option may improve performance but at the expense of time-accuracy. It is not implemented (and therefore ignored) for time-reversible simulations.
`JUMPOUTPUT`	Instructs AERO-S to output the magnitudes of the jumps.

100 PRELOAD

The PRELOAD command statement can be used to specify a preload for a truss or a membrane element. For a truss element, the preload is an axial force that affects its stiffness matrix. For a membrane element, the preload is a three-dimensional generalized force (or force per unit directional length) that also affects its element stiffness matrix. In both cases, the default value(s) of the the preload is (are) zero. It is assumed that the nodal coordinates of the model specified under NODES include the deformations due to preload.

Preload affects all of linear, nonlinear, static, transient, and eigen analyses. For a truss element, the outputted internal axial force includes the amount of preload. For a membrane element, the outputted stresses also include the amount of preload.

STARTING_ELEMENT# THRU ENDING_ELEMENT# PRELOAD_VALUE1 PRELOAD_VALUE2 PRELOAD_VALUE3

`ELEMENT#`	Element number where a preload is to be specified (integer).
`PRELOAD_VALUE1`	For a truss element, value of the axial preloading force. For a membrane element, value of the preload generalized force (force per unit length) in the global $\text{[math]}$ direction (float).
`PRELOAD_VALUE2`	For a membrane element, value of the preload generalized force (force per unit length) in the global $\text{[math]}$ direction (float).
`PRELOAD_VALUE3`	For a membrane element, value of the preload generalized force (force per unit length) in the global $\text{[math]}$ direction (float).
`STARTING_ELEMENT#`	First element of a sequence of elements where a specified preload value or set of values apply (integer).
`THRU`	Keyword indicating that the following entry is the last element of a sequence of elements (characters).
`ENDING_ELEMENT#`	Last element of a sequence of elements where a preload value or set of values apply (integer).

101 PRESSURE

Command Statement: PRESSURE [LOADSET_ID]

The PRESSURE command can be used to specify a piece-wise uniform pressure field, and/or a pressure field resulting from an air blast in the free field and whose parameters are specified under the CONWEP command. The specified pressure field can be applied to beam elements, membrane elements, shell elements, and surface elements defined in SURFACETOPO. For a beam element (type 6 or 7), the pressure is actually a load per unit length applied in the Y-direction of the element frame specified in the EFRAMES command or implied by the third node technique for beam elements (see TOPOLOGY).

For a membrane element (type 128, or 129), a shell element (type 8, 88, 15, 1515, 16, 20, 2020, 73, or 76), or a surface element defined in SURFACETOPO for the sole purpose of defining a surface computation that may be independent from any specific element type, the pressure field is applied normal to the surface of the element using the usual convention of a positive outward normal — that is, if the three nodes of a shell element are denoted by a, b, and c and numbered in this order, the normal is computed as

\text{[math]}

. Furthermore, a positive value of PRESSURE_VALUE implies a force in the direction of the normal.

In a nonlinear analysis, the generated pressure forces are of the follower type for shell elements and surface elements defined in SURFACETOPO.

`LOADSET_ID`	Optional non-negative integer which identifies explicitly the "load" set to which the source term generated by this command belongs to (integer). The default value is 0. Hence, the `PRESSURE` command can be repeated as many times as desired within the same input file using each time a different value for `LOADSET_ID` and different data. The LOADCASE command can refer to `LOADSET_ID` to define one or multiple "load" cases for static analysis (see the STATICS command and the explanation of its sub-command keyword `CASES`), and/or the "load" case for dynamic analysis.
`ELEMENT#`	Element number where a pressure field is to be specified (integer).
`PRESSURE_VALUE#`	Value of the piece-wise uniform pressure field (or load per unit length for a beam element) in that element (float). If `CONWEPSWITCH` is set to `On`, this pressure value is added to the blast pressure generated by the `CONWEP` software module.
`CONWEPSWITCH`	On/Off switch for the pressure load due to an air blast in the free field whose parameters are set in the CONWEP command (characters). If this switch is set to On, the pressure field computed by the software module `CONWEP` is added to that specified in `PRESSURE_VALUE`. Otherwise, only the pressure value specifies in `PRESSURE_VALUE` is used to generate the pressure load to be applied on the specified element or set of elements. The default value of this switch is On.
`STARTING_ELEMENT#`	First element of a sequence of elements where the piece-wise uniform pressure field has the same value (integer).
`ENDING_ELEMENT#`	Last element of a sequence of elements where the piece-wise uniform pressure field has the same value (integer).
`SURFACE`	Keyword indicating that a surface defined in SURFACETOPO is to be identified next by its integer identification number (characters).
`SURFACE#`	Integer identification of the surface defined in SURFACETOPO where the uniform pressure value `PRESSURE_VALUE` is to be applied (integer).

102 PRINTMAT

The PRINTMAT command statement can be used to request outputting to ASCII files the global stiffness and mass matrices in matrix market format. This format is a sparse matrix format that can be read by other programs such as MATLAB.

The numbering of the rows and columns of the printed sparse matrices corresponds to a trivial numbering of all unconstrained degrees of freedom attached to an element of the mesh. It is constructed as follows. First, any constrained and unused degrees of freedom are eliminated. Second, the remaining degrees of freedom are numbered by sorting them in ascending order of their node number. Third, the degrees of freedom with a common node number are further sorted in ascending order according to the degree of freedom index (1: x-displacement, 2: y-displacement, 3: z-displacement; 4: x-rotation, etc). Any other renumbering system specified using the RENUM command is ignored as far as this comand is concerned.

Note 2: If any hyper reduction coefficients are specified in the ATTRIBUTES command, the outputted matrices are the stiffness and mass matrices assembled using the inputted mesh or sampled mesh, weighted by these coefficients.

Note 3: In the presence of this command in the ASCII Input Command Data file, AERO-S will exit after printing the aforementioned matrices and therefore will not perform any specified analysis.

pathandfilenameprefix Specifies a prefix for the output files to contain the global stiffness and mass matrices in matrix market format (character string). The suffixes “.stiffness” and “.mass” will be automatically appended to this prefix by AERO-S.

103 QUASISTATICS ANALYSIS

The QSTATICS command statement is used to signal that the subsequent data lines correspond to the following quasistatics iterative algorithm for solving either Ax=b, where A represents a diagonal block of a coupled linear-linear or linear-nonlinear (multidisciplinary) system and can be singular, or r(x,b)=0, where r represents a row block of a coupled nonlinear-linear or nonlinear-nonlinear (multidisciplinary) system.

For problems of the form Ax=b, the iterative solution algorithm underlying this command can be described as follows

For problems of the form r(x,b)=0, the iterative solution algorithm underlying this command can be described as

For single discipline analysis, the above algorithm is at best (

\text{[math]}

) a direct solution method.

This command is currently relevant for aeroelastic and aerothermal static analyses where the structural or thermal system (respectively) is linear, or aeroelatic static analyses where the structural system is nonlinear. In the first case, A can represent a structural stiffness matrix for aeroelastic analysis, or a conductivity matrix for an aerothermal analysis. In this case, the second and fourth steps of the iterative solution algorithm are enabled only for an aerothermal analysis in which the thermal problem is singular, A represents the matrix of the thermal sub-system, and R represents a basis of its null space. In the second case, r represents the residual of the nonlinear equations governing static equilibrium of the structural system.

This command can also be used to compute a flow-induced load and perform the corresponding static structural analysis. In this case, it must be used together with the staggered solution procedure B0 of the AERO command.

For all purposes outlined above, this command requires the additional usage of the AERO command to specify either the structure matcher file, or the discrete surface to be embedded in the fluid grid, as needed.

MECH $\text{[math]}$ tolqs maxqs delta
HEAT $\text{[math]}$ $\text{[math]}$ tolqs maxqs

$\text{[math]}$	Underrelaxation factor $\text{[math]}$ .
$\text{[math]}$	Underrelaxation factor $\text{[math]}$ .
`tolqs`	Convergence tolerance.
`maxqs`	Maximum number of iterations.
`delta`	Time-step equivalent-value of the increment between any two iterations. This parameter is taken into account only in: (a) the presence of a user-defined “control.C” file (see ACTUATORS, see SENSORS, see USDD, and see USDF), and/or (b) the time-stamp in the output format for quasi-static analysis. It is the equivalent of a time-step and is used to convert the current iteration into current time. The default value is 0. When `delta` is specified to a non-zero value, $\text{[math]}$ is automatically set to $\text{[math]}$ and convergence is not checked because in that case, convergence is reached in one iteration and it is understood that the purpose of the quasistatics analysis is to solve a series of consecutive static problems whose right-hand sides are set by a “control.C” file.

104 RANDOM

The RANDOM command statement is used to signal that some materials have properties with random values. All random material properties are assumed to have a Gaussian probability distribution.

`GROUP#`	Id of the element group for which the random properties are to be specified (integer).
`MATPROP#`	Material property for which the random properties are to be specified (string). Currently, this keyword can take any of the following values: `E` (Young's modulus), `A` (cross section of a bar or beam element), and `kx`, `ky`, and `kz` (linear spring coefficients (see MATERIAL).
`MEAN`	Mean value of the non deterministic `MATPROP` (real). This value overwrites the deterministic value of `MATPROP` specified under the `MATERIAL` command for the elements in the corresponding `GROUP#`.
`STDV`	Standard deviation of the non deterministic `MATPROP` (real).

105 READING REDUCED BASES

Each inputted ROB may be identified by an integer ID number and characterized by a type that covers, among others, different forms of an eigen basis (basis of eigenvectors) or a POD (Proper Orthogonal Decomposition) basis (see ROBC), and a non-negative basis. Such a ROB can be used, for example, to perform reduced-order dynamic computations (see DYNAMICS), or a "Basis Ping-Pong" analysis (see AERO).

Initial conditions for the generalized coordinates associated with a chosen primal ROB can be directly specified using, for example, IDISPLACEMENTS, IVELOCITIES, and/or ITEMPERATURES, as appropriate.

A primal ROB

\text{[math]}

and a dual ROB

\text{[math]}

can also be used to hyper reduce linear and nonlinear problems with equality or inequality constraints (see below for limitations).

Note 2: Currently, the reduction of inequality constraints is supported only for nonlinear implicit dynamic computations such as nonlinear implicit dynamic contact problems, and only for those cases where the constraints are linear and enforced using the Lagrange multipliers method.

Note 3: In such cases, snapshot collection for the construction of a dual basis can be performed only when the constraint method (see CONSTRAINTS) is one of the following methods:

Note 4: Currently, the reduction of equality constraints is supported only when such constraints are enforced using the penalty method.

rob_id1 rob_type1 <pathandfilename1> numvec1 [tolerance1]
.
.
.
rob_idi rob_typei <pathandfilenamei> numveci [tolerancei]
.
.
.
rob_idN rob_typeN <pathandfilenameN> numvecN [toleranceN]

`rob_idi`	Integer number identifying the `i`-th inputted (primal or dual) ROB to support its usage in other commands such as DYNAMICS, IDISPLACEMENTS, IVELOCITIES, and ITEMPERATURES (integer).
`rob_typei`	Type of the `i`-th inputted ROB (characters). It can take one of the following values: `eigen`: in this case, the inputted ROB $\text{[math]}$ must satisfy — within the specified absolute tolerance `tolerance` — both properties $\text{[math]}$ and $\text{[math]}$ , where $\text{[math]}$ and $\text{[math]}$ are the mass and stiffness matrices associated with the finite element model inputted in this ASCII Input Command Data file, $\text{[math]}$ is the diagonal matrix of the squares of its natural circular frequencies, and $\text{[math]}$ is the identity matrix. `mnorm`: in this case, the inputted ROB $\text{[math]}$ must satisfy — within the specified absolute tolerance `tolerance` — the property $\text{[math]}$ . `inorm`: in this case, the inputted ROB $\text{[math]}$ must satisfy — within the specified absolute tolerance `tolerance` — the property $\text{[math]}$ , or may simply have full column rank and not satisfy any orthonormality property. `nnorm`: in this case, the inputted ROB does not have to satisfy any orthogonality property but its columns must be linearly independent. `noneg`: in this case, the inputted ROB $\text{[math]}$ must satisfy the property that none of its entries is negative.
`<pathandfilenamei>`	Name of the `i`-th file (including path, if needed) containing a primal or dual ROB to be read (characters). The type (ASCII/binary) and format of this file follow the same rules as those governing the type and format of `<pathandfilename>` (see above). If the ROB to be read is a primal ROB, this name must have the extension ".massorthonormalized", unless `rob_type_i` is set to `inorm`.
`numveci`	Specifies the size of the `i`-th inputted primal or dual ROB (integer). This parameter is governed by the same rules as those governing `numvec`.
`tolerancei`	Tolerance to be used by AERO-S to verify that the `i`-th inputted primal ROB satisfies the mathematical property associated with its type (real). For example if the ROB $\text{[math]}$ is declared to be mass-orthonormalized, AERO-S performs the following verification $\text{[math]}$ If the ROB $\text{[math]}$ is declared to be of the type `nnorm`, AERO-S performs the Singular Value Decomposition (SVD) of $\text{[math]}$ and verifies that each of its singular values $\text{[math]}$ satisfies $\text{[math]}$ AERO-S performs this verification if and only if this parameter is set to a non zero value, and the requested analysis is a linear structural dynamic analysis using a ROM constructed with the sub-command `MODAL` or `SROM` of DYNAMICS. If this parameter is skipped or assigned a zero value, AERO-S skips this verification. One good reason for skipping this verification is if the computational model does not include a mass or stiffness matrix, as possible in the case of a modal analysis using a ROB of the type `eigen`.

106 RECONSTRUCTING THE SOLUTION FROM THE REDUCED COORDINATES

The RODC command can be used to perform either or both of the following tasks:

The reconstructed high-dimensional solution and its time-derivatives can be outputted in ASCII files using the standard GDISPLAC, GVELOCIT, and GACCELER result keywords of the OUTPUT and/or OUTPUT6 commands.

Note 1: The proper execution of this command requires the presence in the same ASCII Input Command Data file of the DYNAMICS command and its SROM sub-command keyword because this is where the ROB is specified.

Note 2: AERO-S determines the type of data — that is, displacement, velocity, or acceleration — contained in an ASCII input file specified using the sub-command keyword CONFIL from the order in which this file is specified. Specifically, the displacement generalized coordinates file should always be inputted first, followed by the associated velocity and acceleration generalized coordinates files, in this order.

Note 3: Inputting the velocity and acceleration generalized coordinates is optional. However, if the corresponding files are specified through additional entries of CONFIL, freq should be the same for all instances of this sub-command keyword.

Note 4: This command can be executed in parallel by partitioning the mesh associated with the underlying finite element model of interest using the DECOMPOSE command — or the corresponding command line to request mesh partitioning or provide aeros a previously computed mesh partition (see DECOMPOSE).

CONFIL <pathandfilenameS> freq
CONFIL <pathandfilenameV> freq
CONFIL <pathandfilenameA> freq

`CONFIL`	Sub-command keyword for specifying the name of the ASCII file containing the low-dimensional solution (generalized coordinates) of a nonlinear, reduced-order problem constructed by the projection of its high-dimensional counterpart on a ROB. Typically, this file is outputted in a previous AERO-S simulation using the result keyword `GDISPLAC` of OUTPUT or OUTPUT6.
`<pathandfilenameS>`	Path and name of the ASCII file containing the low-dimensional solution (generalized coordinates) of a nonlinear, reduced-order problem constructed by projecting its high-dimensional counterpart of interest on a ROB (characters). Typically, this file is outputted in a previous AERO-S simulation using the result keyword `GDISPLAC` of OUTPUT or OUTPUT6.
`freq`	Frequency at which the reconstruct the dynamic solution (integer). Its default value is 1.
`<pathandfilenameV>`	Path and name of the ASCII file containing the first time-derivative of the low-dimensional solution (generalized coordinates) of a nonlinear, reduced-order problem constructed by projecting its high-dimensional counterpart of interest on a ROB (characters). Typically, this file is outputted in a previous AERO-S simulation using the result keyword `GVELOCIT` of OUTPUT or OUTPUT6.
`<pathandfilenameA>`	Path and name of the ASCII file containing the second time-derivative of the low-dimensional solution (generalized coordinates) of a nonlinear, reduced-order problem constructed by projecting its high-dimensional counterpart of interest on a ROB (characters). Typically, this file is outputted in a previous AERO-S simulation using the result keyword `GACCELER` of OUTPUT or OUTPUT6.

107 RENUMBERING

The RENUMBERING command statement is used to specify the type of node renumbering to be performed on the mesh for either or both of the skyline and sparse solvers. The input format is given below.

TYPE For FEM, the “rcm” and “sloan” schemes are available for the skyline solvers, and the “esmond” (minimal degree ordering) and “metis” (recursive spectral bisection ordering) are available for the (esmond) sparse solver. When a FETI solver is used, two renumbering schemes can be specified if a skyline as well as a sparse solver are to be used by this FETI solver. In this case, the two renumbering schemes can be specified in any order, each on a separate line (string).

108 RESTART

The RESTART command is used to request saving computational data in a RESTART file in order to enable later the restart of a dynamics simulation, and/or initializing a dynamics computation using computational results previously saved in a RESTART file (restart data). The processes of creating and reading from a RESTART file are specified on separate lines using different syntaxes.

`INCREMENT`	An integer number that specifies at every how many time-integration steps the “rcfem.restart” file will be updated. For an updating restart, this number specifies at every how many iterations the file “restart.upd” will be updated.
`PATHANDFILENAME1 INCREMENT`	This command, which can be combined with the following one, instructs AERO-S to save/overwrite the restart data into the specified file `PATHANDFILENAME1` (string) every `INCREMENT` (integer) time-steps. An example using `RESTART` can be found in FEM.d/fem_examples/Restart.d/
`PATHANDFILENAME2 EXTENSION`	This command, which can be combined with the previous one, instructs AERO-S to read the restart data from the specified file `PATHANDFILENAME2` (string) and append the extension `EXTENSION` (string) (e.g. “.2”) to all output filenames specified under the command `OUTPUT`. An example using `RESTART` can be found in FEM.d/fem_examples/Restart.d/
`FLAG_RST`	This optional parameter can be used to specify whether a hot or cold restart is to be performed (characters). A hot restart (which is the default type) is activated by setting `FLAG_RST` to "old" (case-sensitive and must include the quotation marks): it specifies that the restart is to continue a previously performed simulation. A cold restart is activated by setting `FLAG_RST` to "new" (case-sensitive and must include the quotation marks): it specifies that the restart is to perform a new simulation using as initial condition the state stored in the restart file created by a previous simulation. Cold restart of AERO-S is required when performing a coupled fluid-structure simulation using the tandem AERO-F-AERO-S and AERO-F is also restarting in cold mode – that is, not continuing a previous simulation – (for example, if AERO-F is starting an unsteady flow simulation in which the initial condition is specified to be the outcome of a previous steady-state flow computation).

109 RIGID BODY (AND OTHER ZERO ENERGY) MODES

The TRBM command is used to specify a tolerance for monitoring small pivots during the factorization of a matrix. “Small” pivots are deemed to be zero pivots. Therefore, they are associated with rigid body modes (or zero energy modes in general). When this command is specified in the AERO-S input file and the sparse, skyline, blockskyline, or mumps pivot solver is specified under the STATICS command, the generalized inverse of the stiffness, conductivity, mass (when an initial acceleration is to be computed to satisfy the governing equation (see DYNAMICS)), or other relevant matrix is computed in factored form by eliminating the equation associated with a deemed zero pivot and setting the corresponding unknown to zero. This command can be used together with the GRBM command (see below).

Note 2: This command can be used together with the GRBM command. If both of the GRBM and TRBM commands are specified in the same AERO-S input file, then:

VALUE Tolerance for monitoring the zero pivots of a matrix during its factorization. The default value is 1.0e-16 except for the MUMPS solver for which the default is $\text{[math]}$ , where $\text{[math]}$ is the machine precision (real).

110 RIGID BODY MODES FILTER

This command is suitable for structural, aeroelastic, and aerothermoelastic simulations involving an unrestrained (or partially restrained) structural system, when any of the following reasons applies:

In either context outlined above, if this command is specified in the ASCII Input Command Data file, AERO-S automatically determines the rigid body modes of the modeled system using the GRBM method, constructs a projector

\text{[math]}

, where

\text{[math]}

is the identity matrix,

\text{[math]}

is a specified symmetric positive definite matrix (see below), and

\text{[math]}

is the matrix storing the computed rigid body modes, and uses this projector as described below.

`LEVEL`	Omitting the specification of this integer is equivalent to specifying the value of 1.
1	This is the default value. In this case, AERO-S uses the projector as described above.
2	This value is applicable only for linear quasistatic and dynamic analyses. In this case, AERO-S also applies the projector $\text{[math]}$ at each iteration or time-step to the computed displacement and velocity fields in order to explicitly $\text{[math]}$ -orthogonalize them against the specified subset of rigid body modes. This is a safety measure that can be useful, for example, when ill-conditioning prevents the default case from functioning properly.
`QMATRIX`	This integer information is relevant for a linear static or quasistatic analysis only. It allows the user to choose between two different settings for the matrix $\text{[math]}$ . Omitting this information is equivalent to choosing the value of 0.
0	This is the default value. In this case, $\text{[math]}$ is set to the mass matrix.
1	In this case, $\text{[math]}$ is set to the identity matrix.
`TOLERANCE`	Optional tolerance for the case where `QMATRIX` is set to 0 (mass matrix $\text{[math]}$ ) (real). This tolerance is used by AERO-S to identify zero pivots during the factorization of the matrix $\text{[math]}$ , when $\text{[math]}$ is singular due to modeling assumptions. Its default value is 0 (which means that by default, AERO-S assumes that $\text{[math]}$ is invertible).
`LISRBM`	Sub-command keyword to specify a list of rigid body modes to be filtered out (characters). It is relevant only in the case of a dynamic analysis. The list consists of integers ranging between 1 and the number of rigid body modes $\text{[math]}$ computed by the GRBM method and stored in $\text{[math]}$ , each identifying a rigid body mode by its column number in the matrix $\text{[math]}$ . To this effect, the reader is reminded that $\text{[math]}$ stores first the translational rigid body modes in the $\text{[math]}$ , $\text{[math]}$ and $\text{[math]}$ directions, then the rotational ones in the $\text{[math]}$ , $\text{[math]}$ , and $\text{[math]}$ directions. The integer identifiers can be listed in any order. A specified identifier that is greater than $\text{[math]}$ is simply ignored.
`id1` (... `id6`)	ID number ranging between 1 and the number $\text{[math]}$ of rigid body modes computed by the GRBM method and stored in the matrix of rigid body modes $\text{[math]}$ . This integer identifies the column number of $\text{[math]}$ where a rigid body mode to be filtered out from the computed solution is stored: if it is greater than $\text{[math]}$ , it is ignored.

111 RUBBER DAMPING PROPERTIES TABLE

The command RUBDAFT should be used to describe the variations of Young's modulus

\text{[math]}

, its loss factor

\text{[math]}

, the shear modulus

\text{[math]}

, and its loss factor

\text{[math]}

with the frequency

\text{[math]}

(see the sub-command keyword RUBDAMP in MATERIAL) anytime anyone of these four parameters is frequency dependent. These evolutions can be specified here in one or multiple tables defined for one or multiple materials by quintuplets of

\text{[math]}

\text{[math]}

\text{[math]}

\text{[math]}

, and

\text{[math]}

. In each table, linear interpolation is used for the "in between" points, and constant extrapolation (using the parameter values at the closest frequency) is adopted for the "outside" points. When multiple tables are defined, they are inputted one after the other, and each is identified by an id number as described below.

TABLE table_id
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ $\text{[math]}$
. . . . .
. . . . .
. . . . .
$\text{[math]}$ $\text{[math]}$ $\text{[math]}$ $\text{[math]}$ $\text{[math]}$

`TABLE`	Sub-command keyword (characters) for defining a table describing the variation of Young's modulus $\text{[math]}$ , its loss factor $\text{[math]}$ , the shear modulus $\text{[math]}$ , and its loss factor $\text{[math]}$ with the frequency $\text{[math]}$ in the form of quintuplets $\text{[math]}$ .
`table_id`	Id number for the defined table (integer).
$\text{[math]}$	A sampled frequency value (real).
$\text{[math]}$	Value of Young's modulus at the frequency $\text{[math]}$ (real).
$\text{[math]}$	Value of Young's modulus loss factor at the frequency $\text{[math]}$ (real).
$\text{[math]}$	Value of the shear modulus at the frequency $\text{[math]}$ (real).
$\text{[math]}$	Value of the shear modulus loss factor at the frequency $\text{[math]}$ (real).

112 SAVING EIGENMODES OR PROJECTING ONTO A BASIS

Note 2: The EIGENMODES file is written using the “internal” numbering of AERO-S for the degrees of freedom. This internal numbering depends on the equation solver and renumbering scheme that were specified under the STATICS and RENUMBERING commands, respectively, when the eigen solutions were computed. Hence, when reusing the EIGENMODES file for computing the projections of the transient solution of a problem onto the vectors contained in this file, the same equation solver and renumbering scheme must be specified under the STATICS and RENUMBERING commands, respectively.

rob_id Integer number identifying the basis inputted via READMODE (integer). See above for a detailed description of the use of this parameter.

113 SENSITIVITY ANALYSIS (SENSITIVITY completely spelled out)

The SENSITIVITY command statement is used to request the formulation and solution of a structural or aeroelastic sensitivity analysis problem. It can also be used to request that AERO-S participates in the gradient-based solution of a structural or aeroelastic optimization problem by providing the needed sensitivities.

THGRLI int1 int2 ... intN
READSE pathandfilename
TOLSEN tolsen

`THGRLI`
`int1` `int2` `...` `intN`	Sequence of integers inputted on the same line with blank spaces in between that specifies the list of element GROUPS whose thicknesses are to be declared as sensitivity parameters.
`READSE`	This subcommand is relevant only when performing a sensitivity analysis with respect to shape variables.
`pathandfilename`	Name of the ASCII file containing shape sensitivities to be read (characters). Specifically, this file contains $\text{[math]}$ , the derivatives of the structural mesh position $\text{[math]}$ with respect to a number of shape design variables $\text{[math]}$ . The file starts with an XPost-like header (see below), followed by the total number of nodes in the structural model. Then, the information $\text{[math]}$ is specified in this file for each shape design parameter $\text{[math]}$ , one parameter at a time, in block form. First, the index $\text{[math]}$ of $\text{[math]}$ is specified on a separate line starting from $\text{[math]}$ (zero). Then, all nodes of the finite element model are considered in the same ordering as that adopted in the command NODES. On each line corresponding to node $\text{[math]}$ , the derivatives $\text{[math]}$ , $\text{[math]}$ , and $\text{[math]}$ (where $\text{[math]}$ , $\text{[math]}$ , and $\text{[math]}$ denote the coordinates of the node $\text{[math]}$ ) are provided. An example of this ASCII file is given below. `Vector <file name> under load for StructureNodes <vector size = total number of nodes in the finite element structural model> 0^M . . . . . . . . . dx_i/ds_0 dy_i/ds_0 dz_i/ds_0 . . . . . . . . . 1 . . . . . . . . . dx_i/ds_1 dy_i/ds_1 dz_i/ds_1 . . . . . . . . . 2 . . . . . . . . . dx_i/ds_2 dy_i/ds_2 dz_i/ds_2 . . . . . . . . .`
`TOLSEN`
`tolsen`	Convergence tolerance used only when the `SENSITIVITY` command is used to request that AERO-S participates in the gradient-based solution of an aeroelastic optimization problem. The default value is 1.0e-5.

114 SENSORS *S*

The SENSORS command statement is used to specify to AERO-S the degrees of freedom to be observed and whose structural state is to be passed to the user defined control subroutine “control.C” (see ACTUATORS). An example input file using the SENSORS command can be found in FEM.d/fem_examples/Control.d

`NODE#`	Node number where the sensor is to be placed (integer).
`DOF#`	Degree of freedom local number where the sensor is to be placed (integer).

115 SLOSHING PROBLEMS

The command SLOSH is used to specify the computation of the sloshing modes of an incompressible and inviscid fluid whose free surface is orthogonal to a specified gravity field. The computational approach assumes linear kinematics and is based on a fluid displacement potential. In three dimensions, it does not involve any fluid material property. In two dimensions, it requires inputting the thickness of the considered slice of the problem. In both cases, the SLOSH analysis associated with this command requires identifying a free surface using free-surface elements (element type 312 in three dimensions and element type 302 in two dimensions, see TOPOLOGY) but does not require any other boundary condition.

Hence, this command should be used in conjunction with the commands EIGEN and STATICS in order to solve the arising eigenvalue problem.

slgrav Magnitude (scalar) of the gravitational acceleration whose direction must be orthogonal to the free surface of the problem. AERO-S uses this specified value to convert the sloshing eigenvalues to sloshing frequencies (number of cycles per second) for output (real).

116 SLOSHING ZERO ENERGY MODE

This command is effective only for a sloshing eigen computation involving a zero energy mode. It is used to request the computation of the constant potential mode using a physics-based algorithm (rather than the tolerance-based algorithm associated with the TRBM command). It should be used in conjunction with the SLOSH and related commands.

117 SOURCE TIME TABLE-HEAT CONDUCTION

The HFTT command statement must be used to specify the time-dependent amplification of the boundary fluxes. For FEM, pairs of time and amplification values are input. Linear interpolation is also used for “in between” points.

`TABLE_ID`	Optional non-negative integer which uniquely identifies a source-time table so that it can be associated with a "load" set to define the "load" case for a dynamic analysis using the LOADCASE command. The default value is 0. Hence, the `HFTT` command can be repeated as many times as desired within the same input file using each time a different value for `TABLE_ID` and different data.
`TIME_1`	A specified time point (float).
`AMP_1`	A specified amplification value at time point `TIME_1` (float). This amplification factor is automatically set to zero for all times prior to the earliest specified time point and all times later than the latest specified time point.

118 SPECIFIC HEAT COEFFICIENT-TEMPERATURE TABLE

The SCTT command can be used to describe, for a given material, the evolution of the specific heat coefficient with temperature. This evolution can be specified here in a curve (or one-dimensional table) defined by pairs of specific heat coefficient and temperature values. Linear interpolation is used for "in between" points, and the extrema values are adopted for "outside" points. Several curves can be specified, one after the other. Each curve is identified by an ID number as described below.

Note 1: Currently, this command is supported only by the 4-noded tetrahedral termal element (type 50).

`CURVE`	Sub-command keyword (characters) that signals the definition of a specific heat coefficient-temperature curve (or one-dimensional table).
`curve_id`	ID number for the following curve (or one-dimensional table) (integer).
`T_i`	A specified temperature value (real).
`YM_i`	A specified specific heat coefficient value at temperature `T_i` (real).

119 STATICS

The STATICS command statement can be used mainly for three independent purposes: (a) select a static analysis, (b) and/or select an equation solver needed for a static analysis or any other type of analysis specified in an additional command such as DYNAMICS, EIGEN, or other, (c) and/or set parameters that are relevant to many other analyses besides static analysis, such as, for example, a load case among those defined in the command LOADCASE.

For linear static analysis, this command can also be used for requesting the interpretation of concentrated follower (see FORCES) and pressure-induced (see PRESSURE and CONWEP) forces and moments as configuration-dependent external forces and moments and applying to them a piecewise constant treatment, thereby leading to a quasi-static analysis.

`spooles`	Can be executed in parallel on a shared memory system using OpenMP, in both contexts of a single domain and a coarse solver for a FETI-type method.
`skyline`	Can be executed in parallel on a shared memory system using OpenMP, in both contexts of a single domain and a coarse solver for a FETI-type method.
`blockskyline`	Can be executed in parallel on a shared memory system using OpenMP, in both contexts of a single domain and a coarse solver for a FETI-type method.

mumps Can be executed in parallel on a distributed system using MPI, in all contexts of a single domain, a coarse solver for a FETI-type method, and multiple subdomains.

All FETI-type solvers Can be executed in parallel on a shared memory system using OpenMP, a distributed memory system using MPI, and a hybrid system using OpenMP on its shared memory subsystem and MPI across its subsystems. In the case of a distributed or hybrid memory system, and except when mumps is chosen as the coarse problem solver, the coarse problem is duplicated on each MPI process: for this reason, if mumps is not chosen as the coarse problem solver, a single MPI process should be created in general within each computational node in order to minimize the memory penalty associated with this parallel implementation of a FETI-type solver. In the specific case of a hybrid system, if mumps is not chosen as the coarse problem solver, the coarse problem is solved in parallel using the OpenMP threads forked within an MPI process: for this reason, if mumps is not chosen as the coarse problem solver, the maximum speedup factor that can be expected from the parallel solution of the coarse problem is in this case equal to the number of OpenMP threads forked within each MPI process, and a single MPI process should be created within each computational node in order to be able to assign all computational units within this node to the effective parallel solution of the coarse problem. On the other hand, if mumps is chosen as the coarse problem solver, whether the computations are performed on a parallel distributed or hybrid memory system, the coarse problem is solved using all MPI processes without storage duplication. However, by default, the coarse problem is stored on a single MPI process, which is memory inefficient: to distribute this problem across all MPI processes, the user should set ICNTL(18) = 3 (see mumps_icntl below).

METHOD
PARAMETERS
PIECEWISE real_1 real_2
CASES case_id_1 case_id_2 ... case_id_n

`METHOD`	Keyword (characters) specifying one of the solvers named below.
`solverhandle solver_id`	For any of the equation solvers listed below, if configured in the command SOLVERCNTL using for `SOLVER_ID` the same integer specified here in `solver_id` — that is, if this solver and its parameters and identification are specified in SOLVERCNTL (characters, integer). Note that while any of the equation solvers listed below can be configured in SOLVERCNTL, a multi-level FETI-DP solver must be configured in SOLVERCNTL and specified here as a `solverhandle solver_id`.
`direct`	For a skyline direct solver (characters). This is also the default solver (except when the `INPC` command is used) and is available for frequency-domain acoustic (Helmholtz) problems.
`skyline`	For a skyline direct solver (characters). This is also the default solver and is available for frequency-domain acoustic (Helmholtz) problems.a
`blockskyline`	For a skyline symmetric positive direct solver with loop unrolling for optimal performance (characters).
`sparse`	For Esmond's sparse direct solver (characters). This solver is also available for frequency-domain acoustic (Helmholtz) problems.
`sgisparse` (completely spelled out)	For SGI's sparse direct solver (characters). Runs only on SGI machines.
`spooles` (completely spelled out)	For the SPOOLES sparse symmetric positive definite direct solver (characters). Cannot be used for: (a) a singular system, and (b) a system with less than 24 equations and unknowns.
`spooles pivot` (completely spelled out)	For the SPOOLES sparse general symmetric direct solver with the pivoting option turned on (characters).
`mumps` (completely spelled out)	For the MUMPS sparse symmetric positive definite or semi-definite direct solver (characters). This equation solver is not supported by the data organization of BINARY.
`mumps pivot` (completely spelled out)	For the MUMPS sparse general symmetric direct solver with the pivoting option turned on (characters). This equation solver is not supported by the data organization of BINARY.
`mumps unsymmetric` (completely spelled out)	For the MUMPS unsymmetric sparse direct solver (characters). This equation solver is not supported by the data organization of BINARY.
`superlu` (completely spelled out)	For the SUPERLU unsymmetric sparse direct solver (characters).
`sgisky` (completely spelled out)	For SGI's skyline direct solver (characters). Runs only on SGI machines.
`frontal` (completely spelled out)	For a frontal direct solver (characters).
`eisgal`	For EISGAL, the dense, linear equation solver of the `Eigen3` library. It is applicable to arbitrary dense systems of equations arising from a projection-based Reduced-Order Model (ROM). It is also the default equation solver for such computational models.
`dbsgal`	For DBSGAL, the dense, symmetric, linear equation solver of the `LAPACK` library. It is applicable to symmetric, dense systems of equations arising from a projection-based Reduced-Order Model (ROM).
`pcg`	For a preconditioned conjugate gradient solver (characters).
`bcg`	For a bi-conjugate gradient solver (characters).
`cr`	For a conjugate residual solver (characters).
`gmres`	For a generalized minimum residual solver (characters). Applicable to symmetric and unsymmetric systems.
`FETI`	For a one-level FETI solver (default) (characters).
`FETI 1`	For a FETI-1 (one-level FETI method) solver (characters).
`FETI 2 OLD`	For a FETI-2 solver using a “full” coarse problem implementation (characters).
`FETI 2 NEW`	For a FETI-2 solver using a “sparse” coarse problem implementation (characters).
`FETI DP`	For a FETI-DP (FETI dual-primal method) solver (characters).
`FETI DPH`	For a FETI-DPH (FETI dual-primal method with augmentation basis) solver (characters). This solver is to be used only with the `IMPEDANCE` command. Depending on whether the system to be solved is damped or not, or contains a complex boundary condition or multipoint constraint or not, this solver performs in the real or complex domain.
`PARAMETERS`	(keywords or keywords and values) for pcg/bcg/cr/gmres solvers, in any order.
`precno`	Specifies the preconditioner (characters).
0	Unpreconditioned (integer). This is the default value.
1	Diagonal scaling (integer). This option should not be used when solving an indefinite system arising in conjunction with the usage of the LMPC or TIEDSURFACES command, or whenever a structural model includes rigid and/or joint elements (see TOPOLOGY), because in all these cases, the system matrix will contain zero diagonal entries.
2	Incomplete block diagonal scaling (integer). This option is available only for a system of equations resulting from the intrusive version of the Polynomial Chaos method. In this case, the subsystems of equations associated with the diagonal blocks can be solved either using the `sparse` solver (default), or the `FETI DP` method with its acceleration for multiple right sides. If the `FETI DP` method is chosen as a block diagonal solver, then its keyword and the keywords associated with its options should be specified after all other parameters of the main (outer) solver have been specified.
`tolpcg`	Error tolerance for the convergence of the pcg solver (real). The default value is 1e-8.
`tolbcg`	Error tolerance for the convergence of the bcg solver (real). The default value is 1e-8.
`tolcr`	Error tolerance for the convergence of the cr solver (real). The default value is 1e-8.
`tolgmres`	Error tolerance for the convergence of the gmres solver (real). The default value is 1e-8.
`maxitr`	Maximum number of iterations to be performed (integer). The default value is 1000.
`PARAMETERS`	(keywords or keywords and values) for spooles solver, in any order.
`spooles_renum`	Specifies the renumbering (integer, default value is 0).
0	Best of nested dissection and multisection.
1	Multiple minimum degree.
2	Multisection.
3	Nested dissection.
`spooles_scale`	Specifies the scaling (integer, default value is 0).
0	No scaling.
1	Symmetric scaling.
`spooles_tau`	Upper bound on the magnitude of the largest element in L or U when pivoting enabled (real $\text{[math]}$ ). If this number is too small the results will be wrong. The default value of 100 is generally safe if scaling is used (see spooles_scale).
`spooles_msglvl`	Message output level (integer $\text{[math]}$ 0, default value is 0).
`spooles_maxdomainsize`	$\text{[math]}$ /spooles_maxdomainsize is the maximum subgraph size used by SPOOLES orderings, where $\text{[math]}$ is the number of equations in the system to be solved. This parameter is used to control the incomplete nested dissection process. Any subgraph whose weight is less than maxdomainsize is not split further (integer $\text{[math]}$ 0, default value is 24).
`spooles_maxzeros`	$\text{[math]}$ *spooles_maxzeros is the maximum number of zeros allowed in a supernode/front (real > 0 and $\text{[math]}$ 1.0, default value is 0.04).
`spooles_maxsize`	Maximum number of internal columns in supernode/front (integer > 0, default value is 64).
`PARAMETERS`	Keywords and values for the solver `mumps`, in any order. Note that: When specific values are assigned to the `mumps` parameters discussed below under this command (`STATICS`) – to override their default values – AERO-S interprets these parameters as those of a global equation solver: hence, AERO-S ignores them if `mumps` is not specified as the global equation solver. If `mumps` is to be used as the coarse solver of a FETI-type method and specific values are to be assigned to the parameters discussed below, `COARSE_SOLVER` (see below) should be defined as a `solverhandle` identified by `solver_id` and the solver `mumps` and its parameters discussed below should be specified using SOLVERCNTL (see above).
`MUMPS_ICNTL index integer_value`	Sub-command keyword and corresponding pair of integers which can be used to set the integer-valued `mumps` parameters stored in its ICNTL array, as follows: `MUMPS_ICNTL index integer_value` (for ICNTL[`index`] = `integer_value`, see the MUMPS documentation for further details). This keyword and corresponding pair of integers can be repeated as often as desired to set different parameters of the array ICNTL. For example, setting ICNTL[18] = 3 requests that the sparse matrix governing the system of equations to be solved be distributed across all MPI processes, while the default setting ICNTL[18] = 0 has this matrix stored entirely on a single MPI process.
`MUMPS_CNTL index real_value`	Sub-command keyword and corresponding pair of integer index and real value which can be used to set the real-valued `mumps` parameters stored in its CNTL array, as follows: `MUMPS_CNTL index integer_value` (for CNTL[`index`] = `real_value`, see the MUMPS documentation for further details). This keyword and corresponding pair of integer index and real value can be repeated as often as desired to set different parameters of the array CNTL.
`MUMPS_MINEQ integer_value`	This parameter is relevant only when the solver `mumps` is run in distributed mode. It specifies the minimum number of equations to be allocated to each `mumps` MPI process (integer), which itself determines how many of the `mumps` MPI processes requested within the mpirun command are to be effectively allocated to `mumps`: this number is equal to the floor of the ratio of the size of the system of equations to be solved by `mumps` and `integer_value`. Hence, this parameter is particularly important for parallel speedup when `mumps` is used within a FETI-DP solver.
`PARAMETERS`	(keywords or keywords and values) for FETI, FETI-DP, FETI-DPH solvers, in any order).
`spacedim`	This parameter is needed only for the FETI-DPH method with augmentation. It should be set to 2 for two-dimensional problems, and to 3 for three-dimensional ones (integer).
`sparse`	Specifies Esmond's sparse direct method as the local (subdomain and Dirichlet preconditioner) solver (characters). The default is a skyline solver which can also be invoked by specifying `skyline` instead of `sparse` on this line. Note also that there is another mechanism for specifying this option (see below).
`local_solver`
`solverhandle solver_id`	This choice can represent any of the equation solvers listed below, if configured in the command SOLVERCNTL using for `SOLVER_ID` the same integer specified here in `solver_id` — that is, if this solver and its parameters and identification are specified in SOLVERCNTL (characters, integer).
`skyline`	Selects the skyline direct method as the local solver (subdomain and Dirichlet preconditioner problems) (characters). This is also the default choice.
`sparse`	Selects Esmond's sparse direct method as the local solver (characters).
`spooles`	Selects the SPOOLES sparse direct method as the local solver (characters).
`spooles pivot`	Selects the SPOOLES sparse direct method as the local solver with pivoting option turned on (characters).
`mumps`	Selects the MUMPS sparse direct method as the local solver (characters).
`mumps pivot`	Selects the MUMPS sparse direct method as the local solver with pivoting option turned on (characters).
`coarse_solver`
`solverhandle solver_id`	This choice can represent any of the equation solvers listed below, if configured in the command SOLVERCNTL using for `SOLVER_ID` the same integer specified here in `solver_id` — that is, if this solver and its parameters and identification are specified in SOLVERCNTL (characters, integer). It can also represent any FETI-DP solver, including a multi-level FETI-DP solver.
`blockskyline`	Selects the block-skyline direct method as the coarse solver. This is also the default choice (characters).
`skyline`	Selects the skyline direct method as the coarse solver (characters).
`sparse`	Selects Esmond's (sequential) sparse direct method as the coarse solver (characters).
`spooles`	Selects the SPOOLES sparse direct method as the coarse solver (characters).
`spooles pivot`	Selects the SPOOLES sparse direct method as the coarse solver with pivoting option turned on (characters).
`mumps`	Selects the MUMPS sparse direct method as the coarse solver (characters).
`mumps pivot`	Selects the MUMPS sparse direct method as the coarse solver with pivoting option turned on (characters).
`precno`	Specifies the local preconditioner (integer or characters).
`0 or noprec`	Unpreconditioned (integer). This is the default value.
`1 or lumped`	Lumped preconditioner (integer).
`2 or dirichlet`	Dirichlet preconditioner (integer). This is also the default preconditioner.
`projector`
1	Identity based projector (integer). This is also the default projector.
2	Preconditioner based projector (integer). Uses the selected preconditioner for building the so-called Q matrix.
4	Superlumped projector (integer).
`scaling`
`1 or stiffness`	Stiffness based scaling (integer).
`2 or topology`	Topology (subdomain connectivity) based scaling (integer). This is the default scaling procedure.
`version`
1	The FETI (also known as FETI-1) method (integer).
2	The two-level FETI (also known as FETI-2) method (integer).
`nocoarse`	This option is only for dynamics. When specified, the FETI algorithm is executed without any “coarse grid”.
`corners`	This keyword is useful only for the FETI-2, FETI-DP, and FETI-DPH methods. It specifies the treatments of the corners and corner dofs for the construction by these iterative methods of their respective coarse problems. For the FETI-2 method, the user can define both the corner and corner dof selection algorithms. For the FETI-DP and FETI-DPH methods, the corners are automatically chosen by AERO-S but the user can still control the number of dofs at these corners.
`cp3`	In that case, a corner is defined by FETI-2 as a crosspoint, and only the three active translational dof attached at each corner node are included in the construction of the FETI-2 or FETI-DP and FETI-DPH coarse problems. This is the default value for nodes with 3 dofs. Here, a crosspoint is defined as a point that belongs to more than four subdomains.
`cp6`	In that case, a corner is defined by FETI-2 as a crosspoint, and all six active dof attached at each corner node are included in the construction of the FETI-2 or FETI-DP and FETI-DPH coarse problems. This is the default value for nodes with 6 dofs. Here, a crosspoint is defined as a point that belongs to more than two subdomains.
`be3`	In that case, a corner is defined by FETI-2 as the beginning or end of and edge, and only the three active translational dof attached at each corner node are included in the construction of the FETI-2 or FETI-DP and FETI-DPH coarse problems. Note that a crosspoint is also the beginning or end of an edge.
`be6`	In that case, a corner is defined by FETI-2 either as the beginning or end of and edge, and all six active dof attached at each corner node are included in the construction of the FETI-2 or FETI-DP and FETI-DPH coarse problems. Note that a crosspoint is also the beginning or end of an edge.
`fsi_corners`	This keyword is useful only for the FETI-DPH method when applied to the solution of a fluid-structure interaction problem (see FSINTERFACE and HWIB) in the frequency domain. It manages the selection of additional, non_essential corner nodes except for numerical scalability. Note that if the decomposition is performed using DECOMPOSE and a separate run of AERO-S, the setting of this parameter must be the same when later running AERO-S using the generated mesh partition to solve a fluid-structure interaction problem using FETI-DPH.
`0`	In that case, no node of the fluid/structure interface is chosen as a corner node.
`1`	In that case, every fluid node at the intersection of a subdomain boundary interface and the fluid/structure interface is chosen as an additional corner node.
`2`	In that case, every node — whether it is a structure or fluid node — on the intersection of a subdomain boundary interace and the fluid/structure interface is chosen as an additional corner node.
`augment`	This keyword is useful only for the FETI-DP and/or FETI-DPH methods. It specifies the augmentation of the “coarse grid” by various methods defined by the following commands.
`EdgeGs trans/all`	In that case, the “coarse grid” is augmented using extra equations generated by the rigid body modes (rbms) of the subdomain interfaces, and organized edge-by-edge. Here an edge refers to an interface between two subdomains and not to the usual geometric edge. The “trans/all” option denotes the equation type where “trans” refers to the translational rbms, and “all” refers to both the translational and rotational rbms applied per edge.
`Gs trans/all`	In that case, the “coarse grid” is augmented using extra equations generated by the traces of the subdomain rigid body modes (rbms) on the subdomain interface boundaries, and organized subdomain-by-subdomain. The “trans/all” option denotes the equation type where “trans” refers to the translational rbms, and “all” refers to both the translational and rotational rbms.
`WeightedEdgeGs trans/all`	In that case, the “coarse grid” is augmented using extra equations generated by the weighted rigid body modes (rbms) of the subdomain interfaces, and organized edge-by-edge. Here an edge refers to an interface between two subdomains and not to the usual geometric edge. The “trans/all” option denotes the equation type where “trans” refers to the translational rbms, and “all” refers to both the translational and rotational rbms applied per edge. The weights are similar to those used for scaling the residuals. Hence, they are based on stiffness considerations if the `scaling` option is set to `stiffness`, or on topological considerations if the `scaling` option is set to `topology`.
`primal`	This choice is relevant for the one-level (standard) FETI-DP method, when either `Gs trans/all` or `WeightedEdgeGs trans/all` augmentation option is selected. It is also required in the context of an $\text{[math]}$ -level FETI-DP method, for the FETI-DP solvers applied to levels 1 to $\text{[math]}$ . In this case, the rigid body modes are used to define primal unknowns on the "coarse grid" problems instead of additional constraints.
`EdgeWs [type] numdir`	This option is exclusive to the FETI-DPH solver and can be combined with the option `EdgeGs`. It augments the corner-based coarse problem of the FETI-DPH algorithm with extra equations generated by the free-space solutions of the frequency-domain acoustic or elastodynamic (or modelled dynamic shell) equation — these are real cosine and sine waves of arbitrary directions — and organized edge-by-edge. Here an edge refers to an interface between two subdomains and not to the usual geometric edge. There are as many free-space solutions to be considered as there are wave directions to be considered. Setting the optional parameter `type` to `solid`, `shell`, `fluid`, or `any`, depending on the type of the elements used in the mesh delivers the best performance. If the mesh contains several types of elements, the option `any` is recommended (default value). The parameter `numdir` specifies the number of desired directions and therefore controls the total number of such wavy augmentation modes (integer). Its default value is 0. The exact number of augmentation modes per interface edge is equal to $\text{[math]}$ `numdir` for two- and three-dimensional frequency-domain acoustic problems, $\text{[math]}$ `numdir` for two-dimensional elastodynamic (or modelled dynamic shell) problems, and $\text{[math]}$ `numdir` for three-dimensional elastodynamic (or modelled dynamic shell) problems. In the latter case, the factor 6 comes from the fact that for each direction, there are 2 shear waves and 1 pressure wave, and each of these three waves has a cosine mode as well as a sine mode. The implemented directions are chosen according to the following scheme. In two dimensions, a sector is discretized into `n` sectors, with `n` an even integer. A direction is defined by connecting the center of the circle to a point on the circle delimiting a sector. Since both the cosine and sine modes are included, only one direction for each pair of opposite directions needs be retained, which results in a total of `n`/2 directions. Hence, `n` is chosen to be 2*`numdir`. In three dimensions, a cube is discretized into $\text{[math]}$ points. A direction is defined by connecting the center of the cube to a point lying on a face of the cube. Since both the cosine and sine modes are included, only one direction for each pair of opposite directions needs be retained, which results in a total of $\text{[math]}$ directions. Hence, `n` is chosen so that $\text{[math]}$ is as close as possible to `numdir`, with $\text{[math]}$ `numdir`.
`interf_solver`	This option is currently available only for the FETI-DP and FETI-DPH solvers. It specifies the Krylov method to be used with these algorithms for solving the interface problem (characters).
`cg`	Turns on the CG algorithm as an interface problem solver. This is the default value of `interf_solver`.
`cgal`	Turns on Dostal's Augmented Lagrangian CG algorithm with adaptive precision control as an interface problem solver.
`gmres`	Turns on the GMRES algorithm as an interface problem solver.
`agmres`	Turns on the GMRES algorithm with a deflation-based accelerator for systems with multiple left and/or right sides (characters). In this case, a non zero deflation subspace size must also be specified using the sub-command keyword `deflation_size`: otherwise, `agmres` will revert to `gmres`. Note that by default, the acceleration of the solution of systems with multiple left sides (or nearby systems) using this configuration of the GMRES algorithm is disabled because unless the left side matrices have some special structure (that is not currently exploited), it requires a substantial overhead. However, this acceleration can be enabled using the sub-command keyword `mlhs`.
`deflation_size`	Specifies the size of the deflation subspace when `AGMRES` is specified as the Krylov-based interface solver for the FETI-DP or FETI-DPH iterative domain decomposition method (integer). The default value for this size is 0. Hence, activating the deflation-based acceleration component of the GMRES solver for systems with multiple left and/or right sides requires setting the deflation size to a strictly positive integer value.
`deflation_type`	Specifies how to construct the deflation subspace of the iterative solver `agmres` (integer). The default value is 0.
`0`	Specifies that the deflation subspace is to be constructed using eigenvectors associated with the smallest eigenvalues XXX of what?? XXX.
`1`	Specifies that the deflation subspace is to be constructed using eigenvectors associated with the largest eigenvalues XXX of what?? XXX.
`mlhs`	Specifies whether to turn on or off the deflation-based accelerator for systems with multiple left sides when `agmres` is specified as the Krylov-based interface solver for the FETI-DP or FETI-DPH iterative domain decomposition method. The default value is 0.
`1`	Turns on the deflation-based accelerator.
`0`	Turns off the deflation-based accelerator.
`gcr`	Turns on the GCR algorithm as an interface problem solver.
`orthotol`	This option is currently available only for the FETI-DPH solver. It specifies the tolerance to be used for filtering out “small” vectors during the local Gram-Schmidt-like orthogonalization of the augmentation vectors. The default value is 1.0e-02.
`mpc_type`	This keyword is useful only for the FETI-DP and FETI-DPH methods. It specifies the algorithm to be used for handling potential multipoint constraints (MPCs) (characters). The default is `primal` when the number of MPCs is less or equal to 1000, and `dual` otherwise.
`dual`	In this case, the MPCs are enforced by Lagrange multipliers and are satisfied only at convergence (characters).
`primal`	In this case, the MPCs are put in the coarse problem and are satisfied at every iteration (characters).
`mpc_precn`	This keyword is useful only for the FETI-DP and FETI-DPH methods, in the presence of MPCs, and when `mpc\_type` is set to `dual` (characters). The default is `tblock` when running a single thread process, and `full` otherwise.
`full`	In this case, the $\text{[math]}$ matrix, where `C` denotes the constraint matrix, is treated as a single block matrix (characters).
`tblock`	In this case, the potential algebraic block-structure of the $\text{[math]}$ matrix, is exploited (characters).
`sblock`	In this case, the subdomain-structure of the $\text{[math]}$ matrix, is exploited (characters).
`mblock`	In this case, the mortar-interface-structure of the $\text{[math]}$ matrix, is exploited (characters).
`diag`	In this case, the $\text{[math]}$ matrix is approximated by its diagonal (characters).
`mpc_scaling`
`1 or stiffness`	Stiffness based scaling (integer).
`2 or topology`	Topology (subdomain connectivity) based scaling (integer). This is the default scaling procedure.
`cct_solver`
`solverhandle solver_id`	This choice can represent any of the equation solvers listed below, if configured in the command SOLVERCNTL using for `SOLVER_ID` the same integer specified here in `solver_id` — that is, if this solver and its parameters and identification are specified in SOLVERCNTL (characters, integer).
`skyline`	Selects the skyline direct method as the coarse solver. This is the default choice (characters).
`sparse`	Selects Esmond's (sequential) sparse direct method as the coarse solver (characters).
`cct_tol`	Specifies the tolerance to be used for detecting singularities in the solution of the $\text{[math]}$ problems of the FETI-DP and FETI-DPH methods in the presence of MPCs (real). The default is 1.0E-12.
`kryprec`	This option is only for nonlinear problems. It turns on the Krylov preconditioner enrichment for the solution of nearby problems in a Newton method (characters).
1	Turns on the Krylov preconditioner and gives to the `maxorth` parameter (see below) the scope of the entire nonlinear analysis.
2	Turns on the Krylov preconditioner and gives to the `maxorth` parameter (see below) the scope of a load-step in a nonlinear analysis.
`global_cor_rbm_tol`	Specifies the tolerance to be used for detecting singularities in the solution of the corner-based coarse problems of the FETI-DP and FETI-DPH methods (real). The default is 1.0E-6.
`global_rbm_tol`	Specifies the tolerance to be used for detecting the global rigid body modes when using a FETI method (real). The default is 1.0E-6.
`maxorth`	Specifies the maximum total number of reorthogonalization vectors used for accelerating a FETI algorithm and/or enriching its chosen preconditioner during a simulation (integer). For linear problems or while the tangent operator of a nonlinear problem is frozen, the acceleration is performed using a multiple right side technique based on reorthogonalization, but only if `interf-solver` (see below) is set to `CG` or `GCR`. For nonlinear problems, the acceleration is performed using a multiple left side technique based on the enrichment of the preconditioner, but only if: (a) `interf_solv` (see below) is set to `CG`, and (b) kryprec (see above) is activated. If the kryprec option is not activated, `maxorth` is to be understood as the maximum total number of reorthogonalization vectors per Newton iteration, as these vectors are flushed when the tangent operator is rebuilt. For nonlinear problems where the tangent operator is periodically frozen, if the `kryprec` option is used, priority in the accumulation of vectors is given to enriching the preconditioner. The default value is `maxitr` (see below). To turn-off this reorthogonalization option, set `maxorth` to 1.
`tolfeti`	Error tolerance for the convergence of the feti solver (real). The default value is 1.0e-06.
`maxitr`	Maximum number of iterations to be performed (integer). The default value is 1000.
`PIECEWISE real_1 real_2`	This sub-command keyword (characters) followed by two real numbers is applicable to linear static and dynamic analyses. It requests the interpretation of concentrated follower (see FORCES), pressure-induced (see PRESSURE and CONWEP), temperature-induced (see TEMPERATURES and THERMOE), and freeplay-induced (see MATERIAL) forces and moments, and moments due to gravity (see GRAVITY) and discrete masses (see DIMASS) as configuration-dependent external forces and moments, and enables their piecewise constant treatment. In this treatment, the application of the aforementioned external loading is divided into steps and is performed at the beginning of each step using the updated deformed configuration. To this effect, and in the case of a static analysis: the first entered real number, `real_1`, specifies the load fraction increment to apply at each step; and the second real number, `real_2`, specifies the total load factor to apply to all inputted external loads. For example, consider the input "PIECEWISE 0.25 1.0". The second entry "1.0" requests keeping all external loads inputted using various commands of AERO-S unchanged, and the first entry "0.25" requests their application to the system of interest in 4 steps — that is, the application at each step of 25% only of these external loads. On the other hand, inputting "PIECEWISE 0.25 2.0" requests multiplying first all external loads resulting from various external load input commands by the factor 2, then applying at each step a load increment equal to 0.25 times of the original external loads. This implies splitting the application of the magnified external loads in 8 steps and applying at each step an external load increment equal to 12.5% of the magnified external load. For a dynamic analysis, this sub-command is automatically activated for the freeplay-induced (see MATERIAL) forces and moments.
`CASES`	This optional sub-command keyword (characters) can be used to select a "load" case among those defined in the LOADCASE command. In this capacity, it is relevant to all analyses. However for linear static analysis and single-frequency frequency response analysis, it can also be used to select multiple "load" cases among those defined in the LOADCASE command. Selecting no "load" case is equivalent to selecting the load case 0 which by default contains the "load" set 0 and any "load" generated by a command which does not support the "load" set construct (`LOADSET_ID`) (see the FORCES, PRESSURE, HNEU, FLUX, and/or CONVECTION command).
`case_id_j`	Non-negative integer identifying uniquely a $\text{[math]}$ -th "load" case that is defined in the LOADCASE command. Specifying more than one case identifier on the same line results in a multiple "load" case analysis.

120 STRESS-STRAIN ONE-DIMENSIONAL TABLE

The SS1DT command can be used to describe the evolution of stress with strain, for a given material. This evolution can be specified here via a curve (or one-dimensional table) defined by pairs of strain and stress values. Linear interpolation is used for "in between" points, and the extrema values are adopted for "outside" points. Several curves can be specified, one after the other. Each curve is identified by an ID number as described below.

`CURVE`	Sub-command keyword (characters) signaling the definition of a stress-strain curve (or table).
`curve_id`	“Id number” for the following curve (or one-dimensional table) (integer).
`strain_i`	A specified strain value (real).
`stress_i`	A specified stress value at strain `strain_i` (real).

121 STRESS-STRAIN TWO-DIMENSIONAL TABLE

The SS2DT command can be used to describe the evolution of stress with biaxial strain, for a given material. This evolution can be specified here in a surface (or two-dimensional table) defined by triplets of two strain values and and one stress value. Linear interpolation is used for "in between" points, and the extrema values are adopted for "outside" points. Several surfaces can be specified, one after the other. Each surface is identified by an ID number as described below.

SURFACE surface_id [ENGINEERING eng_flag]
strain22_1 ... strain22_m
strain11_1 stress_11 ... stress_1m
. .
. .
. .
strain11_n stress_n1 ... stress_nm

`SURFACE`	Sub-command keyword (characters) signaling the definition of a stress-biaxial-strain surface (or table).
`surface_id`	“Id number” for the following surface (or two-dimensional table) (integer).
`ENGINEERING`	Optional sub-command keyword signaling the input of a flag that specifies the interpretation of the inputted stress and strain data (characters).
`eng_flag`	A flag specifying the interpretation of the inputted stress and strain data (characters). The value `On` indicates that the stress and strain data are to be interpreted as engineering quantities. The value `Off` indicates that the stress and strain data are to be interpreted as the second-Piola Kirchhoff stress and Green-Lagrange strain, respectively. The default value is `On`.
`strain11_i`	A specified strain11 value (real).
`strain22_j`	A specified strain22 value (real).
`stress_ij`	A specified stress value at strains `strain11_i` and `strain22_j` (real).

122 STRUCTURAL DAMPING LOSS FACTOR TABLE

The command SDETAFT can be used to describe for a given material, the variation of the Young modulus loss factor

\text{[math]}

(see the sub-command keyword STRDAMP in MATERIAL) with the frequency

\text{[math]}

. This evolution can be specified here in one or multiple curves (or tables) each defined by pairs of Young modulus loss factor and frequency values. On each curve, linear interpolation is used for the "in between" points, and constant extrapolation (using the loss factor value at the closest frequency) is adopted for the "outside" points. When multiple curves are defined, they are inputted one after the other, and each is identified by an id number as described below.

CURVE curve_id
$\text{[math]}$ $\text{[math]}$
. .
. .
. .
$\text{[math]}$ $\text{[math]}$

`CURVE`	Sub-command keyword (characters) for defining a curve (or table) describing the variation of the Young modulus loss factor $\text{[math]}$ with the frequency $\text{[math]}$ in the form of pairs $\text{[math]}$ .
`curve_id`	"Id number" for the defined curve (integer).
$\text{[math]}$	A sampled frequency value (real).
$\text{[math]}$	Value of the Young modulus loss factor at the frequency $\text{[math]}$ (real).

123 SURFACE TOPOLOGY

The SURFACETOPO command statement can be used to define a discrete surface on a body by describing its faceted connectivity. Each facet may, but does not necessarily have to, be an element defined in the command TOPOLOGY. Such a surface can be paired with another similar surface using another command statement in order to define a surface-to-surface interaction (see TIEDSURFACES, CONTACTSURFACES, FSINTERFACE, AERO). It can also be referred to by another command statement to define a surface boundary condition (see PRESSURE, FORCES, DISPLACEMENTS, FLUX and TEMPERATURES) or a group of nodes (see GROUPS).

Each surface is inputted using two sections. The first one identifies the surface to be defined and assigns to it, if needed, a thickness. This section is followed by a second section which contains the description of all faces constituting the surface. Each face is specified on a separate line. The set of two sections can be repeated as many times as there are surfaces to be defined.

`ID_NUMBER`	Surface id number (integer).
`SURFACE_THICKNESS`	Optional keyword indicating that the surface identified by `ID_NUMBER` defines the midplane of a physical surface (string). The importance of this parameter is underlined by the following note and consequences. For contact detection and enforcement, a surface is treated as 2-sided (or “shell” surface) when both of the following conditions are met: (a) the simulation is explicit dynamics with `flagTDENFORCE` set to `On` in DYNAMICS (or omitted since this is the default setting), and (b) a non-zero value is specified here for this surface thickness parameter. In all other cases, the contact detection and enforcement is 1-sided. For a 1-sided surface, the directions of the normals to the faces of the surface are important. Contact interactions between two 1-sided surfaces, or self-contact involving one 1-sided surface, can only be detected between two faces with normals in opposite directions. Furthermore, if an interaction is detected, the directions of the normals establish whether the configuration involves penetration or separation. For a 2-sided surface, the directions of the normals of the faces of the surface are not important. Contact interactions between two 2-sided surfaces, or self-contact involving one 2-sided surface, can be detected between two faces regardless of the directions of the normals. For contact between one 2-sided surface and one 1-sided surface, only the normal direction of the 1-sided surface is important. If an interaction is detected, the direction of the normal of the 1-sided surface establishes whether the configuration involves penetration or separation.
`t`	Real or virtual thickness of the surface used for detecting and enforcing contact conditions on both of its sides (real). The default value is 0.

`FACE#`	Face id number whose type and connectivity are to be specified (integer).
`FACETYPE`
1	4-node quadrilateral.
2	8-node quadrilateral.
3	3-node triangle.
4	6-node triangle.
5	9-node quadrilateral.
6	12-node quadrilateral.
7	10-node triangle.

124 THERMAL EXPANSION TEMPERATURE TABLE

The TETT command statement can be used to describe the evolution of the coefficient of thermal expansion with temperature, for a given material. This evolution can be specified here in a curve (or table) defined by pairs of temperature and coefficient of thermal expansion values. Linear interpolation is used for “in between” points, and the extrema values are adopted for “outside” points. Several curves can be specified, one after the other. Each curve is identified by an “id number” as described below.

`CURVE`
`curve_id`	“Id number” for the following curve (or table) (integer).
`T_1`	A specified temperature value (float).
`TE_1`	A specified coefficient of thermal expansion value at temperature `T_1` (float).

125 THERMOELASTICITY

The THERMOE command statement is used to indicate that AERO-S is to interact with itself to perform a transient thermoelastic (thermostructure-structure vibration) one-way coupled simulation.

126 TIED SURFACES

The TIEDSURFACES command can be used to tie — that is, enforce perfect contact between — pairs of surfaces defined using the command SURFACETOPO. Surface interactions are detected using the search module of the library ACME. For explicit computations, the discrete kinematic constraint equations are defined and enforced as specified in the sub-command keyword TDENFORCE and its associated flag flagTDENFORCE of the DYNAMICS object. For implicit computations, the discrete kinematic constraint equations are formulated using AERO-S's mortar method and enforced using the method specified in CONSTRAINTS or in CONSTRAINT_METHOD below with the following limitation: in this case, the enforcement method can be only one of the following three methods: the penalty method, the Lagrange multiplier method, or the augmented Lagrange multiplier method.

Note 1: The enforcement of tied surface constraints by the Lagrange multiplier method in all but explicit dynamic analyses is supported only by the FETI-DP family of solvers, the GMRES solver, and the SPOOLES and MUMPS direct sparse solvers with pivoting enabled (see STATICS).

or, for static, frequency response, eigenvalue, implicit dynamic, and explicit dynamic computations with the flag flagTDENFORCE set to Off (see DYNAMICS)

SURF_PAIR_ID# MASTER SLAVE MORTAR_TYPE NORMAL_TOL TANGENTIAL_TOL CONSTRAINT_METHOD

or, for explicit dynamic computations with the flag flagTDENFORCE set to On (see DYNAMICS)

SURF_PAIR_ID# MASTER SLAVE KPART_TYPE NORMAL_TOL TANGENTIAL_TOL NUM_ITER CONVERG_TOL CONSTRAINT_METHOD

`SURF_PAIR_ID#`	Id number of the surface pair to be described (integer).
`MASTER`	Identification of the master (mortar method) surface (see SURFACETOPO) (integer).
`SLAVE`	Identification of the slave (mortar method) surface (see SURFACETOPO) (integer).
`CONSTRAINT_METHOD`	Method for enforcing the associated constraints (characters). The default method is set in CONSTRAINTS and used whenever this entry is omitted.
`multipliers`	The Lagrange multiplier method.
`elimination`	The elimination method (see CONSTRAINTS for changing the default values of its parameters).
`penalty` `beta`	The penalty method. The parameter `beta` should be a large positive number, typically of the order of $\text{[math]}$ (no default value is provided).
`augmented` `beta`	The augmented Lagrangian method. The parameter `beta` should be a large positive number, typically of the order of $\text{[math]}$ (no default value is provided).
`MORTAR_TYPE`	Mortar type: 0 = standard, 1 = dual, default value is 0 (integer).
`NORMAL_TOL`	Normal search tolerance used by ACME to identify interactions, default value is 0.1 (float) (see Figs. 1.2 and 1.3 in Section 1.3 of ACME's User Reference Manual).
`TANGENTIAL_TOL`	Tangential search tolerance used by ACME to identify interactions, default value is 0.001 (float) (see Figs. 1.2 and 1.3 in Section 1.3 of ACME's User Reference Manual).
`KPART_TYPE`	Kinematic partitioning type: 0 = fixed, 1 = automatic, default value is 0 (integer).
`NUM_ITER`	Maximum number of predictor-corrector iterations to be performed at each time step. The default value is 5 (integer).
`CONVERG_TOL`	Convergence tolerance of the predictor-corrector iteration loop. The default value is 1.0e-10 (float).

127 USER DEFINED FORCES *S*

The main purpose of the USDF command is to specify nodal forces and/or moments of the follower or axial type for a structural model via a user-defined subroutine. In this case, the user should: (1) write his/her own algorithm for specifying the nodal forces and/or moments within a subroutine named control.C (see APPENDIX 10), (2) compile this subroutine and link it using the makefile provided for this command, and (3) use LOAD to activate it.

By default, all user-defined forces and moments are interpreted as being of the axial type — that is, as being defined in the fixed nodal degree of freedom reference frames (see NODES and NFRAMES). However, if a node has rotational degrees of freedom, the user can specify that the forces and/or moments prescribed at this node are of the follower type — that is, they act in a direction that remains constant in the local frame attached to the node where they are applied. This local frame coincides with the nodal degree of freedom reference frame (see NODES and NFRAMES) in the undeformed configuration. In the deformed configuration, the orientation of this local frame is defined by the rotation of the node to which it is attached. In other words, the specified nodal force or moment "follows" in this case the rotation of the node to which it is applied.

User-defined nodal forces and/or moments are not assembled neither at the element level nor at the subdomain level. They can be combined with those specified under the FORCES and GRAVITY commands, but will not be amplified by the MFTT or HFTT tables. In case of a conflict between this command and the FORCES and GRAVITY commands, the specified nodal forces are simply added. A more detailed description of the control.C subroutine is given in the form of a template in APPENDIX 10.

`NODE#`	Node number where the force/moment is specified (integer).
`DOF#`	Degree of freedom local number where the force/moment is specified (integer).
`TYPE`	For structural models, all user-defined nodal sources (forces and/or moments in the case of a structural model) are by default of the axial type. However, if this parameter is set to `FOLLOWER` and the node `NODE#` has rotational degrees of freedom, the user-defined source (force or moment in the case of a structural model) at this node and the degree of freedom `DOF#` is considered to be of the follower type (characters).

128 USER DEFINED PRESCRIBED DISPLACEMENTS *S*

The purpose of the USDD command is to specify time-variant prescribed displacements for any node and its associated dofs using a user-defined subroutine. In this case, the user should: 1) write his/her own algorithm for specifying the prescribed displacement field within a subroutine named “control.C”, 2) compile this subroutine and link it with AERO-S using the makefile that is provided for this purpose, and 3) use the LOAD command (see LOAD) to activate it. An example input file using the USDD command can be found in FEM.d/fem_examples/USDD.d/.

This command can be used simultaneously with the time-invariant command DISPLACEMENTS for prescribing displacements at a node. In the event of a conflict between the DISPLACEMENTS and USDD commands, USDD prevails. A more detailed description of the “control.C” subroutine is given in its template located in the Control.d directory of AERO-S.

`NODE#`	Node number where the displacement is specified (integer).
`DOF#`	Degree of freedom local number where the displacement is specified (integer).

129 WEIGHTS

The WEIGHTS command statement can be used to modify some or all of the weights attributed by default to an element type (see TOPOLOGY). These weights are exploited by the mesh partitioning algorithm (see DECOMPOSE) to achieve load balance when generating the subdomains.

`ELEMENT_TYPE#`	This is the element type id number as in the `TOPOLOGY` command (integer).
`DESIRED_WEIGHT`	This is the desired weight to be attributed to this element type (integer).

1	M: 3d truss (bar) with 3 dof/node (W = 1).
2	M: 2d 4-node quadrilateral with 2 dof/node (W = 2).
3	H: 3d 4-node quadrilateral with 1 dof/node (W = 2).
4	M: 2d 3-node triangle with 2 dof/node (W = 2).
6	M: 3d Bernoulli beam with 6 dof/node (W = 1).
7	M: 3d Timoshenko beam with 6 dof/node (W = 1).
8	M: 3d 3-AQR shell with 6 dof/node (W = 3).
88	M: 3d 4-node shell with 6 dof/node (splits into 2 elements of type 8) (W = 4).
9	H: 3d 2-node line with 1 dof/node (W = 1).
10	H: 2d 4-node quadrilateral with 1 dof/node ( W = 2).
11	M: 3d 1-node torsional spring with 3 dof/node (W = 1).
12	M: 3d 1-node translational spring with 3 dof/node (W = 1).
15	M: 3d 3-node triangular AQR shell with 6 dof/node and composite as well as nonlinear material capability (W = 3).
1515	M: 3d 4-node quadrilateral AQR shell with 6 dof/node and composite as well as nonlinear material capability (W = 4).
16	M: 3d Belytschko-Tsay shell with 6 dof/node (W = 4).
17	M: 3d 8-node brick with 3 dof/node (W = 3).
18	M: 3d 4-node shear panel with 3 dof/node (W = 1).
19	M: 3d 3-node membrane with 6 dof/node (W = 3).
	(only in-plane and drilling stiffnesses) (W = 1).
20	M: 3d 3-node composite or orthotropic shell with 6 dof/node (W = 3).
2020	M: 3d 4-node composite or orthotropic shell with 6 dof/node (splits into 2 elements of type 20) (W = 4).
21	M: 3d translational spring-link with 3 dof/node (W = 1).
22	M: 3d torsion spring-link with 3 dof/node (W = 1).
23	M: 3d 4-node tetrahedron with 3 dof/node (W = 3).
24	M: 3d 6-node pentahedron with 3 dof/node (W = 3).
25	M: 3d 10-node tetrahedron with 3 dof/node (W = 4).
30	A: 2d 4-node quadrilateral with 1 dof/node (W = 1).
31	A: 2d 4-node quadrilateral GLS element with 1 dof/node (W = 1).
32*	A: 2d 8-node quadrilateral with 1 dof/node (W = 3).
33*	A: 2d 4-node quad bubblE element with 1 dof/node (W = 1).
34*	A: 2d 4-node quad two-level bubble element with 1 dof/node (W = 1).
35	A: 2d 3-node triangle with 1 dof/node (W = 1).
36	A: 2d 3-node triangular GLS element with 1 dof/node (W = 1).
38*	A: 2d 6-node triangle with 1 dof/node (W = 3).
40	A: 3d 4-node tetrahedron with 1 dof/node (W = 2).
41	A: 3d 4-node tetrahedral GLS element with 1 dof/node (W = 2).
42	A: 3d 10-node tetrahedron with 1 dof/node (W = 3).
44	A: 3d 8-node brick GLS element with 1 dof/node (W = 3).
45*	A: 3d 8-node brick with 1 dof/node (W = 3).
46	H: 3d 3-node triangular heat element (W = 2).
4646	H: 3d 4-node triangular heat element (splits into 2 elements of type 46) (W = 3).
47	H: 3d 2-node line with 1 dof/node for boundary convection (W = 1).
48	H: 3d 4-node quadrilateral with 1 dof/node for boundary convection (W = 2).
49	H: 3d 3-node triangle with 1 dof/node for boundary convection (W = 2).
50	H: 3d 4-node tetrahedron with 1 dof/node (W = 3).
51	H: 3d 8-node brick with 1 dof/node (W = 4).
52*	M: 3d 6-node triangular shell (W = 1).
53	H: 2d 3-node triangular heat element (W = 2).
56	H: 3d 2-node heat radiation element (W = 1).
57	H: 3d 3-node triangular heat radiation element (W = 2).
58	H: 3d 4-node quadrilateral heat radiation element (W = 2).
59	A: 2d 6-node axisymmetric triangle with 1 dof/node (W = 3).
60	A: 2d 4-node axisymmetric quadrilateral with 1 dof/node (W = 2).
61	A: 2d 3-node axisymmetric triangle with 1 dof/node (W = 1).
62	A: 2d 8-node axisymmetric quadrilateral with 1 dof/node (W = 3).
65	M: 3d 2-node rigid truss (bar) (W = 1).
66	M: 3d 2-node rigid beam (W = 1).
67	M: 3d rigid link (translational and rotational) (W = 1).
68	M: 3d rigid translational link (W = 1).
69	M: 3d rigid rotational link (W = 1).
70	M: 3d rigid plane or solid element with 3 dof/node (3-node to 20-node element) (W = 3).
71	M: 3d rigid plane or solid element with 3 dof/node and anywhere from 3 to 20 nodes per element (W = 1).
72	M: 3d 20-node brick (W = 4).
73	M: 3d 3-node rigid shell (W = 3).
74	M: 3d rigid plane or solid element with 6 dof/node (3-node to 32-node element) (W = 1).
76	M: 3d 4-node rigid shell (W = 4).
78	M: 3d 1-node point-to-line constraint element with 3 dof/node (W = 1).
79	M: 3d 1-node point-to-plane constraint element with 3 dof/node (W = 1).
81	H: 2d 4-node contact resistance thermal element with 1 dof/node that can be inserted between two thermal elements of type = 10 (W = 2).
82	H: 3d 8-node contact resistance thermal element with 1 dof/node that can be inserted between two thermal elements of type = 51 (W = 4).
83	H: 3d 6-node contact resistance thermal element with 1 dof/node that can be inserted between two thermal elements of type = 50 with 4 nodes each (W = 4).
84	H: 2d 3-node triangular bulk fluid (thermal) element with 1 dof/node. The first node appearing in the connectivity list of this element must be inside the bulk fluid and the other two nodes must be located at the interface boundary between the bulk fluid and the surrounding material. The temperature at the first node is by definition the average temperature of the bulk fluid (W = 2).
85	H: 3d 4-node bulk fluid (thermal) tetrahedron with 1 dof/node. The first node appearing in the connectivity list of this element must be inside the bulk fluid and the other three nodes must be located at the interface boundary between the bulk fluid and the surrounding material. The temperature at the first node is by definition the average temperature of the bulk fluid (W = 3).
86	H: 3d 5-node pyramidal bulk fluid (thermal) element with 1 dof/node. The first node appearing in the connectivity list of this element must be inside the bulk fluid and the other four nodes must be located at the interface boundary between the bulk fluid and the surrounding material. The temperature at the first node is by definition the average temperature of the bulk fluid (W = 4).
87	M: 3d 4-node membrane with 6 dof/node (W = 4).
90	A: 3d 6-node wedge with 1 dof/node (W = 3).
91	M: 3d 32-node serendipity brick with 3 dof/node (W = 6).
92	M: 3d 26-node serendipity wedge with 3 dof/node (W = 5).
93	A: 3d 32-node serendipity brick with 1 dof/node (W = 5).
94	A: 3d 26-node serendipity wedge with 1 dof/node (W = 4).
95	A: 3d 8-node, or 27-node, or 64-node, or 125-node hexahedron with 1 dof/node (W = 3, 4, 5, 6).
96	A: 3d 4-node, or 10-node, or 20-node, or 35-node tetrahedron with 1 dof/node (W = 1, 2, 3, 4).
97	M: 3d 15-node serendipity wedge with 3 dof/node (W = 4).
98	A: 2d 4-node, or 9-node, or 16-node, or 25-node quadrilateral with 1 dof/node (W = 2, 3, 4, 5).
99	A: 2d 3-node, or 6-node, or 10-node triangle with 1 dof/node (W = 2, 3, 4).
100	M: 2d 4-node, or 9-node, or 16-node, or 25-node quadrilateral with 3 dof/node (W = 2, 3, 4, 5).
101	M: 2d 3-node, or 6-node, or 10-node triangule with 3 dof/node (W = 2, 3, 4).
102	M: 3d 8-node, or 27-node, or 64-node, or 125-node hexahedron with 3 dof/node (W = 2, 3, 4, 5).
103	M: 3d 4-node, or 10-node, or 20-node, or 35-node hexahedron with 3 dof/node (W = 1, 2, 3, 4).
105	A: 3d 8-node, or 27-node, or 64-node, or 125-node spectral hexahedron with 1 dof/node (W = 2, 3, 4, 5).
106	M: 3d 2-node rigid beam of arbitrary length, including zero length (W = 1).
108	A: 2d 4-node, or 9-node, or 16-node, or 25-node spectral quadrilateral with 1 dof/node (W = 2, 3, 4, 5).
109	H: 3d 8-node, or 27-node, or 64-node, or 125-node hexahedron with 1 dof/node (W = 2, 3, 4, 5).
111	M: 3d fabric truss with 3 dof/node (W = 1).
118	M: 3d 2-node planar joint with 6 dof/node (W = 1).
120	M: 3d 2-node spherical joint with 3 dof/node (W = 1).
121	M: 3d 2-node translational joint with 3 rotational dof/node (W = 1).
122	M: 3d 2-node universal joint with 6 dof/node (W = 1).
123	M: 3d 2-node revolute joint with 6 dof/node (W = 1).
124	M: 3d 2-node cylindrical joint with 6 dof/node (W = 1).
125	M: 3d 2-node prismatic joint with 6 dof/node (W = 1).
126	M: 3d 2-node joint-with-driver with 6 dof/node (W = 1).
127	M: 3d 2-node pin-in-slot joint with 6 dof/node (W = 1).
128	M: 3d 4-node plane stress/plane strain quadrilateral with 3 dof/node (W = 1).
129	M: 3d 3-node plane stress/plane strain triangle with 3 dof/node (W = 1).
131	M: 3d 1-node discrete mass and inertia element with 6 dof/node (W = 1).
132	M: 3d 2-node massless rigid beam of non zero length (W = 1).
133	M: 3d 2-node massless rigid beam of arbitrary length, including zero length (W = 1).
134	M: 3d 2-node prismatic joint-with-driver and 6 dof/node (W = 1).
150	M: 3d 4-node rigid tetrahedron with 3 dof/node (W = 3).
151	M: 3d 6-node rigid pentahedron with 3 dof/node (W = 4).
177	M: 3d 2-node point-to-moving-point constraint element with 3 dof/node (W = 1).
178	M: 3d 3-node point-to-moving-line constraint element with 3 dof/node (W = 1).
179	M: 3d 4-node point-to-moving-plane constraint element with 3 dof/node (W = 1).
180	M: 3d 8-node Q1-P0 hexahedron with 3 dof/node and nonlinear material capability (W = 3).
181	M: 3d 20-node Q2-P0 hexahedron with 3 dof/node and nonlinear material capability (W = 4).
182	M: 3d 20-node Q2-P1 hexahedron with 3 dof/node and nonlinear material capability (W = 4).
183	M: 3d 4-node P1-P0 tetrahedron with 3 dof/node and nonlinear material capability (W = 3).
200	M: 3d 2-node uniaxial translational spring with 3 dof/node for linear or nonlinear analyses (W = 1).
201	M: 3d 2-node uniaxial translational spring with 6 dof/node for linear or nonlinear analyses (W = 3).
202	M: 3d 2-node uniaxial torsional spring with 3 rotational dof/node for linear or nonlinear analyses (W = 3).
203	M: 3d 2-node uniaxial tension-only translational spring with 3 dof/node and an optional freeplay model, for linear or nonlinear analyses (W = 1).
204	M: 3d 2-node uniaxial tension-only or compression-only translational spring with 6 dof/node and a freeplay model, for linear or nonlinear analyses (W = 1).
205	M: 3d 2-node uniaxial tension-only or compression-only torsional spring with 3 rotational dof/node and a freeplay model, for linear or nonlinear analyses (W = 1).
220	M: 3d 2-node spherical joint spring combination with 6 dof/node (W = 1).
221	M: 3d 2-node translational joint spring combination element with 6 dof/node (W = 1).
222	M: 3d 2-node universal joint spring combination element with 6 dof/node (W = 1).
223	M: 3d 2-node revolute joint spring combination element with 6 dof/node (W = 1).
224	M: 3d 2-node cylindrical joint spring combination element with 6 dof/node (W = 1).
225	M: 3d 2-node prismatic joint spring combination element with 6 dof/node (W = 1).
226	M: 3d 2-node revolute joint-with-actuator and 6 dof/node (W = 1).
227	M: 3d 2-node pin-in-slot joint spring combination element with 6 dof/node (W = 1).
234	M: 3d 2-node prismatic joint-with-actuator and 6 dof/node (W = 1).
280	M: 3d 8-node Q1-P0 incompressible hexahedron with 3 dof/node and nonlinear material capability (W = 3).
301	F: 2d 4-node sloshing (fluid) quadrilateral with 1 dof/node (W = 1).
302	F: 2d 2-node free-surface (fluid) element with 1 dof/node for two-dimensional sloshing computations using element type = 301 (W = 1).
311	F: 3d 4-node sloshing (fluid) tetrahedron with 1 dof/node (W = 3).
312	F: 3d 3-node free-surface (fluid) triangle with 1 dof/node for three-dimensional sloshing computations using element type = 311 (W = 2).
321	F: 2d 4-node hydroelastic vibration (fluid) quadrilateral with 1 dof/node (W = 2).
323	M: 3d 2-node revolute joint spring combination element with 6 dof/node and a freeplay model (W = 1).
325	M: 3d 2-node prismatic joint spring combination element with 6 dof/node and a freeplay model (W = 1).
331	F: 3d 4-node hydroelastic vibration (fluid) tetrahedron with 1 dof/node (W = 3).
1100	A: 2d 4-node Helmholtz DGM element Q-4-1 (W = 1).
1101	A: 2d 4-node Helmholtz DGM element Q-8-2 (W = 2).
1102	A: 2d 4-node Helmholtz DGM element Q-16-4 (W = 4).
1103	A: 2d 4-node Helmholtz DGM element Q-32-8 (W = 8).
1110	A: 2d 3-node Helmholtz DGM element T-4-1 (W = 1).
1111	A: 2d 3-node Helmholtz DGM element T-8-2 (W = 2).
1120	A: 2d 4-node Helmholtz DEM element Q-4-1 (W = 1).
1121	A: 2d 4-node Helmholtz DEM element Q-8-2 (W = 2).
1122	A: 2d 4-node Helmholtz DEM element Q-16-4 (W = 4).
1123	A: 2d 4-node Helmholtz DEM element Q-32-8 (W = 8).
1130	A: 2d 3-node Helmholtz DEM element T-4-1 (W = 1).
1131	A: 2d 3-node Helmholtz DEM element T-8-2 (W = 2).
1150	A: 3d 8-node Helmholtz DGM element H-6-1 (W = 1).
1151	A: 3d 8-node Helmholtz DGM element H-26-4 (W = 4).
1152	A: 3d 8-node Helmholtz DGM element H-56-8 (W = 8).
1153	A: 3d 8-node Helmholtz DGM element H-98-12 (W = 12).
1160	A: 2d 3-node Helmholtz DGM element T-6-1 (W = 1).
1161	A: 2d 3-node Helmholtz DGM element T-26-4 (W = 4).
1162	A: 2d 3-node Helmholtz DGM element T-56-8 (W = 8).
1170	A: 3d 8-node Helmholtz DEM element H-6-1 (W = 1).
1171	A: 3d 8-node Helmholtz DEM element H-26-4 (W = 4).
1172	A: 3d 8-node Helmholtz DEM element H-56-8 (W = 8).
1173	A: 3d 8-node Helmholtz DEM element H-98-12 (W = 12).
1200	M: 2d 4-node Elastodynamic DGM element Q-4x2-2 (W = 2).
1201	M: 2d 4-node Elastodynamic DGM element Q-16x2-8 (W = 8).
1220	M: 2d 4-node Elastodynamic DEM element Q-4x2-2 (W = 2).
1250	M: 3d 4-node Elastodynamic DGM element H-6x3-3 (W = 3).
1251	M: 3d 4-node Elastodynamic DGM element H-26x3-15 (W = 15).
1252	M: 3d 4-node Elastodynamic DGM element H-50x3-28 (W = 28).

130 YOUNG MODULUS-STRAIN TABLE

The YMST command can be used to describe, for a given material, the evolution of the Young modulus with strain. This evolution can be specified here in a curve (or one-dimensional table) defined by pairs of Young modulus and strain values. Linear interpolation is used for "in between" points, and the extrema values are adopted for "outside" points. Several curves can be specified, one after the other. Each curve is identified by an ID number as described below.

`CURVE`	Sub-command keyword (characters) that signals the definition of a Young modulus-strain curve (or one-dimensional table).
`curve_id`	ID number for the following curve (or one-dimensional table) (integer).
`T_i`	A specified strain value (real).
`YM_i`	A specified Young modulus value at strain `Strain_i` (real).

131 YOUNGS MODULUS-TEMPERATURE TABLE

The YMTT command statement can be used to describe the evolution of Young's modulus with temperature, for a given material. This evolution can be specified here in a curve (or table) defined by pairs of temperature and Young's modulus values. Linear interpolation is used for “in between” points, and the extrema values are adopted for “outside” points. Several curves can be specified, one after the other. Each curve is identified by an “id number” as described below.

`CURVE`
`curve_id`	“Id number” for the following curve (or table) (integer).
`T_1`	A specified temperature value (float).
`YM_1`	A specified Young's modulus value at temperature `T_1` (float).

132 YIELD STRESS-EFFECTIVE PLASTIC STRAIN TABLE

The YSST command statement can be used to describe the evolution of the yield stress with the effective plastic strain, for a given material. This evolution can be specified here in a curve (or table) defined by pairs of effective plastic strain and yield stress values. Linear interpolation is used for "in between" points, and linear extrapolation is used for "outside" points (at the "right"). Several curves can be specified, one after the other. Each curve is identified by an "id number" as described below.

`CURVE`
`curve_id`	"Id number" for the following curve (or table) (integer).
`EPS_i`	A specified effective plastic strain value (float). The first point of the table should be characterized by `EPS_1` = 0.
`YS_i`	A specified yield stress value at the effective plastic strain `EPS_i` (float).

133 YIELD STRESS SCALING FACTOR-EFFECTIVE PLASTIC STRAIN RATE TABLE

The YSSFSRT command statement can be used to describe the evolution of the yield stress scaling factor with the effective plastic strain rate, for a given material. This evolution can be specified here in a curve (or table) defined by pairs of effective plastic strain rate and yield stress scaling factor values. Linear interpolation is used for “in between” points, and linear extrapolation is used for “outside” points (at the “right”). Several curves can be specified, one after the other. Each curve is identified by an “id number” as described below.

`CURVE`
`curve_id`	“Id number” for the following curve (or table) (integer).
`EPSR_1`	A specified effective plastic strain rate value (float). The first point of the table should be characterized by `EPSR_1` = 0 and `YSSF_1` = 1.
`YSSF_1`	A specified yield stress scaling factor value at the effective plastic strain `EPSR_1` (float). The first point of the table should be characterized by `EPSR_1` = 0 and `YSSF_1` = 1.

AERO-S Manual

Version 1.1

Short Contents

Table of Contents

AERO-S

1 INTRODUCTION

2 INSTALLATION

3 ACOUSTIC TIME-DOMAIN ARTIFICIAL BOUNDARY *S*

4 ACOUSTIC TIME-DOMAIN DIRICHLET BOUNDARY CONDITIONS *S*

5 ACOUSTIC TIME-DOMAIN DISTRIBUTED NEUMANN BOUNDARY CONDITION *S*

6 ACOUSTIC TIME-DOMAIN NEUMANN BOUNDARY CONDITIONS *S*

7 ACOUSTIC TIME-DOMAIN ROBIN DISTRIBUTED BOUNDARY CONDITION *S*

8 ACTUATORS *S*

9 AEROELASTICITY

10 AEROHEAT

11 ATTRIBUTES *S*

12 BEAM OFFSET

13 BEAM REFERENCE FRAMES

14 BINARY INPUT / OUTPUT

15 BOUNDARY CONVECTION *S*

16 BOUNDARY DISPLACEMENTS *S*

17 BOUNDARY FLUXES

18 BOUNDARY FORCES *S*

19 BOUNDARY TEMPERATURES *S*

20 BUCKLING

21 CLUSTERING SNAPSHOTS OR CONSTRUCTING A REDUCED BASIS

22 COMMENTS

23 COMPOSITE (OR ORTHOTROPIC SHELL OR ANISOTROPIC SOLID)

24 COMPOSITE (ORTHOTROPIC SHELL OR ANISOTROPIC SOLID) ELEMENT FRAMES

25 CONDITION NUMBER

26 CONSTRAINTS

27 CONSTRUCTING A REDUCED MESH

28 CONTACT SURFACES

29 CONTROL STATEMENT

30 CONWEP

31 DENSITY-TEMPERATURE TABLE

32 DISCRETE NODAL MASS AND INERTIA

33 DYNAMIC ANALYSIS

34 EIGENVALUE PROBLEMS

35 ELEMENT TOPOLOGY *S*

36 ENABLING REDUCTION AND HYPER REDUCTION USING LOCAL REDUCED-ORDER BASES

37 END

38 EQUATION SOLVER CONFIGURATION

39 FIELD WEIGHTS FOR MESH DECOMPOSITION

40 FLUID/STRUCTURE INTERFACE

41 FORCE TIME TABLE-MECHANICS AND ACOUSTICS

42 GEOMETRIC RIGID BODY MODES

43 GEOMETRIC STIFFENING DUE TO PRESTRESS

44 GLOBAL SIMULATION PARAMETERS

45 GRAVITATIONAL ACCELERATION

46 GROUPS

47 HEAT CONDUCTION COEFFICIENT-TEMPERATURE TABLE

48 HEAT ZERO ENERGY MODE

49 HEAT ZERO ENERGY MODES FILTER

50 HELMHOLTZ

51 HELMHOLTZ ANALYSIS (AXISYMMETRIC/PARTIALLY AXISYMMETRIC)

52 HELMHOLTZ ARTIFICIAL ABSORBING BOUNDARY CONDITIONS *S*

53 HELMHOLTZ ARTIFICIAL ABSORBING BOUNDARY CONDITIONS (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) *S*

54 HELMHOLTZ AUXILIARY SURFACE FAR-FIELD PATTERN (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) *S*

55 HELMHOLTZ CONSTRAINED FICTITIOUS NODES (PARTIALLY AXISYMMETRIC) *S*

56 HELMHOLTZ DIRICHLET BOUNDARY CONDITIONS *S*

57 HELMHOLTZ DIRICHLET BOUNDARY CONDITIONS (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) *S*

58 HELMHOLTZ DISTRIBUTED NEUMANN BOUNDARY CONDITION *S*

59 HELMHOLTZ FAR-FIELD PATTERN (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) *S*

60 HELMHOLTZ LINEAR MULTIPOINT CONSTRAINTS

61 HELMHOLTZ LINEAR MULTIPOINT CONSTRAINTS (PARTIALLY AXISYMMETRIC) *S*

62 HELMHOLTZ LOCATIONS WHERE TO COMPUTE THE KIRCHHOFF INTEGRAL

63 HELMHOLTZ NEUMANN BOUNDARY CONDITIONS *S*

64 HELMHOLTZ NEUMANN BOUNDARY CONDITIONS – FICTITIOUS DOMAIN (PARTIALLY AXISYMMETRIC) *S*

65 HELMHOLTZ NEUMANN BOUNDARY CONDITIONS – REAL DOMAIN (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) *S*

66 HELMHOLTZ NODES BELOW AUXILIARY SURFACE (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) *S*

67 HELMHOLTZ SCATTERER BOUNDARY *S*

68 HELMHOLTZ WAVE NUMBER (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) *S*

69 HELMHOLTZ WET INTERFACE BOUNDARY *S*

70 HYDROELASTIC FLUID/STRUCTURE BOUNDARY

71 HYDROELASTIC FREE SURFACE BOUNDARY

72 HYPER REDUCTION OF THE INERTIA FORCES ASSOCIATED WITH A CONSTANT MASS MATRIX

73 IMPEDANCE ANALYSIS

74 INITIAL ACCELERATIONS (Not Supported Yet)

75 INITIAL DISPLACEMENTS *S*

3 ACOUSTIC TIME-DOMAIN ARTIFICIAL BOUNDARY S

4 ACOUSTIC TIME-DOMAIN DIRICHLET BOUNDARY CONDITIONS S

5 ACOUSTIC TIME-DOMAIN DISTRIBUTED NEUMANN BOUNDARY CONDITION S

6 ACOUSTIC TIME-DOMAIN NEUMANN BOUNDARY CONDITIONS S

7 ACOUSTIC TIME-DOMAIN ROBIN DISTRIBUTED BOUNDARY CONDITION S

8 ACTUATORS S

11 ATTRIBUTES S

15 BOUNDARY CONVECTION S

16 BOUNDARY DISPLACEMENTS S

18 BOUNDARY FORCES S

19 BOUNDARY TEMPERATURES S

35 ELEMENT TOPOLOGY S

52 HELMHOLTZ ARTIFICIAL ABSORBING BOUNDARY CONDITIONS S

53 HELMHOLTZ ARTIFICIAL ABSORBING BOUNDARY CONDITIONS (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) S

54 HELMHOLTZ AUXILIARY SURFACE FAR-FIELD PATTERN (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) S

55 HELMHOLTZ CONSTRAINED FICTITIOUS NODES (PARTIALLY AXISYMMETRIC) S

56 HELMHOLTZ DIRICHLET BOUNDARY CONDITIONS S

57 HELMHOLTZ DIRICHLET BOUNDARY CONDITIONS (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) S

58 HELMHOLTZ DISTRIBUTED NEUMANN BOUNDARY CONDITION S

59 HELMHOLTZ FAR-FIELD PATTERN (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) S

61 HELMHOLTZ LINEAR MULTIPOINT CONSTRAINTS (PARTIALLY AXISYMMETRIC) S

63 HELMHOLTZ NEUMANN BOUNDARY CONDITIONS S

64 HELMHOLTZ NEUMANN BOUNDARY CONDITIONS – FICTITIOUS DOMAIN (PARTIALLY AXISYMMETRIC) S

65 HELMHOLTZ NEUMANN BOUNDARY CONDITIONS – REAL DOMAIN (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) S

66 HELMHOLTZ NODES BELOW AUXILIARY SURFACE (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) S

67 HELMHOLTZ SCATTERER BOUNDARY S

68 HELMHOLTZ WAVE NUMBER (AXISYMMETRIC/PARTIALLY AXISYMMETRIC) S

69 HELMHOLTZ WET INTERFACE BOUNDARY S

75 INITIAL DISPLACEMENTS S

76 INITIAL DISPLACEMENT 6 COLUMNS (IDISP6 completely spelled out) S

79 INITIAL TEMPERATURES S

80 INITIAL VELOCITIES S

82 LINEAR MATERIAL PROPERTIES S

93 NODES S

114 SENSORS S

127 USER DEFINED FORCES S

128 USER DEFINED PRESCRIBED DISPLACEMENTS S