*MATRIX GENERATE

Generate global or element matrices.

This option is used to generate matrices representing the stiffness, mass, viscous damping, structural damping, or load vectors in a model.

This page discusses:

See Also
In Other Guides
Generating Matrices as a Linear Analysis Step

ProductsAbaqus/Standard

TypeHistory data

LevelStep

At least one of the following parameters is required

STIFFNESS

Include this parameter to generate the stiffness matrix.

MASS

Include this parameter or set MASS=CONSISTENT to generate the consistent mass matrix.

Set MASS=AT USER NODES to generate the consistent mass matrix with the mass only at the user-defined nodes. If a finite element has nonzero mass at Abaqus internal nodes, the mass is transferred to the user-defined nodes using heuristic techniques. Mass is redistributed only for modified triangle and tetrahedral elements; no mass is redistributed from internal to user-defined nodes for frame elements and substructures.

VISCOUS DAMPING

Include this parameter to generate the viscous damping matrix.

STRUCTURAL DAMPING

Include this parameter to generate the structural damping matrix.

LOAD

Include this parameter to generate the load matrix.

The following parameter is required if the model contains solid continuum infinite elements

SOLID INFINITE FORMULATION

Set this parameter equal to STATIC to select the static formulation for solid infinite elements.

Set this parameter equal to DYNAMIC to select the dynamic formulation for solid infinite elements.

Optional parameters

ELEMENT BY ELEMENT

Include this parameter to generate local element matrices. By default, global assembled matrices are generated.

ELSET

Use this parameter to generate matrices for a part of a model. Set this parameter equal to the name of an element set that contains all the elements in the selected part of a model. By default, matrices are generated for the whole model.

FIELD

Set FIELD=ALL (default) to indicate that matrices are generated for the structural and acoustic parts of the model.

Set FIELD=MECHANICAL to indicate that matrices are generated only for the structural part of the model.

Set FIELD=ACOUSTIC to indicate that matrices are generated only for the acoustic part of the model.

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.

INTERFACE NODES

This parameter specifies some of the nodes as “interface nodes.” By specifying interface nodes, you can reduce the number of nodes required for including matrices in the matrix usage analysis. Set this parameter equal to the name of the node set that contains all of the interface nodes in the desired order.

MPC

Set MPC=YES (default) to generate the matrices with applied multipoint constraints. The generated matrices will include entries only for the independent degrees of freedom.

Set MPC=NO to skip applying the multipoint constraints during the matrix generation. The matrices will include entries for all active degrees of freedom in the model.

PROPERTY EVALUATION

Set this parameter equal to the frequency at which to evaluate frequency-dependent properties for viscoelasticity, springs, and dashpots during the matrix 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.

SOURCE

Set SOURCE=ALL (default) to generate matrices including contributions from the finite elements and from the matrix input.

Set SOURCE=ELEMENTS to generate matrices including only contributions from the finite elements.

Set SOURCE=MATRIX INPUT to generate matrices including only contributions from the matrix input. The ELSET and SOURCE=MATRIX INPUT parameters are mutually exclusive.

There are no data lines associated with this option.