*SUBSTRUCTURE GENERATE

Optional parameters

DISPLAY ELSET

Set this parameter equal to the name of the element set that contains all the elements you want to use to define the coarse substructure display representation for visualization in the substructure usage analysis.

This element set can include any 2-node elements (truss, beam, connector, etc.) and 3- or 4-node elements with two-dimensional geometry (surface, membrane, shell).

EIGENPROBLEM

Set this parameter equal to YES (default) if the substructure eigenproblem needs to be solved during substructure generation in Abaqus. Substructure eigenvectors can be used to define substructure modal damping for a given substructure.

Set this parameter equal to NO if the eigensolution is not required.

ELSET

If element output recovery is needed, including all element nodes in the selective recovery node set generally is insufficient since an element can have Abaqus internal nodes.

Set this parameter equal to the name of the element set that contains all the elements in the regions of the substructure where you want to recover results.

FRICTION DAMPING

Set FRICTION DAMPING=NO (default) to ignore friction-induced viscous damping effects.

Set FRICTION DAMPING=YES to include friction-induced viscous damping effects.

GRAVITY LOAD

Set GRAVITY LOAD=YES to calculate the substructure's gravity load vectors. The default is GRAVITY LOAD=NO.

LIBRARY

Set this parameter equal to the prefix in the generated substructure name. The prefix and the identifier (specified using the TYPE parameter) constitute a substructure name that must be unique. The default prefix is jobname.

The LIBRARY and NAME parameters are mutually exclusive. Using the NAME parameter is the preferred method.

MASS MATRIX

Set MASS MATRIX=YES to calculate the substructure's reduced mass matrix. The default is MASS MATRIX=NO.

MODEL DATA

Set MODEL DATA=ODB (default) to generate the substructure model data file, which contains the finite element model data required for visualization of results recovered within the substructure.

Set MODEL DATA=NONE to suppress generation of the substructure model data file.

MONITOR NSET

Set this parameter equal to the name of the node set that contains the nodes whose solution you want to monitor in the substructure usage analysis.

Monitor nodes are created automatically in the usage-level model, and history output requests are applied to these nodes in the usage-level analysis procedures (where applicable).

NAME

Set this parameter equal to the substructure name for which the substructure data are written. See Input Syntax Rules for the syntax of such names. The default substructure name is jobname_Zn, where n is the current step number of the job.

The NAME parameter and the LIBRARY and TYPE parameters are mutually exclusive. Using the NAME parameter is the preferred method.

NSET

Set this parameter equal to the name of the node set that contains the nodes of the substructure where you want to recover results. This node set must contain all nodes for which node output can be requested in a substructure usage analysis.

If the NSET parameter is omitted but the ELSET parameter is used, the recovery matrix corresponding to all the element nodes in the specified element set is generated. If both the NSET and ELSET parameters are used, the recovery matrix for the union of the node set and the set of all the element nodes for all the elements in the element set is generated. If both the NSET and ELSET parameters are omitted, the recovery matrix for all eliminated nodes is generated (default case).

OVERWRITE

Include this parameter to overwrite existing files in the substructure database with the same name. The default is no overwrite.

PROPERTY EVALUATION

Set this parameter equal to the frequency at which to evaluate frequency-dependent properties for viscoelasticity, springs, and dashpots during the substructure generation. If this parameter is omitted, Abaqus/Standard evaluates the stiffness associated with frequency-dependent springs and dashpots at zero frequency and does not consider the stiffness contributions from frequency-domain viscoelasticity in the SUBSTRUCTURE GENERATE step.

RECOVERY MATRIX

Set RECOVERY MATRIX=NO to specify that output of element or nodal information is not available within this substructure. The default is RECOVERY MATRIX=YES, indicating that recovery of eliminated variables is possible for most analysis procedures.

If RECOVERY MATRIX=NO, the NSET and ELSET parameters are ignored.

RESIDUAL MODES

Include this parameter to add the following to the substructure basis:

• The load modes corresponding to the substructure load cases specified in the substructure generation analysis
• The residual modes computed in the static perturbation analyses between the most recent eigenfrequency extraction analysis and the current substructure generation analysis

If no eigenfrequency extraction analysis is specified before the substructure generation analysis, Abaqus/Standard adds the residual modes computed from all the static perturbation analyses specified before the substructure generation analysis, as well as the load modes corresponding to the substructure load cases, to the substructure basis.

STIFFNESS MATRIX

For acoustic-structural substructures, this parameter is valid only for substructures generated using coupled modes.

If this parameter is omitted, a symmetric instance of the substructure's reduced stiffness matrix is generated when Abaqus/Standard uses the symmetric solver for the current analysis step. An unsymmetric instance of the substructure's reduced stiffness matrix is generated when Abaqus/Standard uses the unsymmetric solver for the current analysis step. For more information, see Matrix Storage and Solution Scheme in Abaqus/Standard.

Set STIFFNESS MATRIX=SYMMETRIC to generate a symmetric instance of the reduced stiffness matrix regardless of whether Abaqus/Standard uses the symmetric or unsymmetric solver.

Set STIFFNESS MATRIX=UNSYMMETRIC to generate an unsymmetric instance of the reduced stiffness matrix regardless of whether Abaqus/Standard uses the symmetric or unsymmetric solver.

Set STIFFNESS MATRIX=BOTH to generate both a symmetric and an unsymmetric instance of the reduced stiffness matrix regardless of whether Abaqus/Standard uses the symmetric or unsymmetric solver.

STRUCTURAL DAMPING MATRIX

Set STRUCTURAL DAMPING MATRIX=YES to calculate the substructure's reduced structural damping matrix. A symmetric instance of the reduced structural damping matrix is generated when Abaqus/Standard uses the symmetric solver. An unsymmetric instance of the reduced structural damping matrix is generated when Abaqus/Standard uses the unsymmetric solver. For more information, see Matrix Storage and Solution Scheme in Abaqus/Standard.

The default is STRUCTURAL DAMPING MATRIX=NO.

Set STRUCTURAL DAMPING MATRIX=SYMMETRIC to generate a symmetric instance of the reduced structural damping matrix regardless of whether Abaqus/Standard uses the symmetric or unsymmetric solver. For acoustic-structural substructures, this parameter value is valid only for substructures generated using coupled modes.

Set STRUCTURAL DAMPING MATRIX=UNSYMMETRIC to generate an unsymmetric instance of the reduced structural damping matrix regardless of whether Abaqus/Standard uses the symmetric or unsymmetric solver. For acoustic-structural substructures, this parameter value is valid only for substructures generated using coupled modes.

Set STRUCTURAL DAMPING MATRIX=BOTH to generate both a symmetric and an unsymmetric instance of the reduced structural damping matrix regardless of whether Abaqus/Standard uses the symmetric or unsymmetric solver. For acoustic-structural substructures, this parameter value is valid only for substructures generated using coupled modes.

TYPE

Set this parameter equal to the identifier in the generated substructure name. The identifier and the prefix (specified using the LIBRARY parameter) constitute a substructure name that must be unique. The identifier must be Z followed by a number that cannot exceed 9999. The default identifier is Zn, where n is the current step number of the job.

The TYPE and NAME parameters are mutually exclusive. Using the NAME parameter is the preferred method.

VISCOUS DAMPING MATRIX

Set VISCOUS DAMPING MATRIX=YES to calculate the substructure's reduced viscous damping matrix. A symmetric instance of the reduced viscous damping matrix is generated when Abaqus/Standard uses the symmetric solver. An unsymmetric instance of the reduced viscous damping matrix is generated when Abaqus/Standard uses the unsymmetric solver. For more information, see Matrix Storage and Solution Scheme in Abaqus/Standard.

The default is VISCOUS DAMPING MATRIX=NO.

Set VISCOUS DAMPING MATRIX=SYMMETRIC to generate a symmetric instance of the reduced viscous damping matrix regardless of whether Abaqus/Standard uses the symmetric or unsymmetric solver. For acoustic-structural substructures, this parameter value is valid only for substructures generated using coupled modes.

Set VISCOUS DAMPING MATRIX=UNSYMMETRIC to generate an unsymmetric instance of the reduced viscous damping matrix regardless of whether Abaqus/Standard uses the symmetric or unsymmetric solver. For acoustic-structural substructures, this parameter value is valid only for substructures generated using coupled modes.

Set VISCOUS DAMPING MATRIX=BOTH to generate both a symmetric and an unsymmetric instance of the reduced viscous damping matrix regardless of whether Abaqus/Standard uses the symmetric or unsymmetric solver. For acoustic-structural substructures, this parameter value is valid only for substructures generated using coupled modes.