- 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.
-
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.
-
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.