Abaqus Analysis User's Manual  


10.3.1 Generating global matrices

Product: Abaqus/Standard  

References

Overview

Matrix generation:

Generating global matrices

A linearized finite element model can be summarized in terms of matrices representing the stiffness, mass, damping, and loads in the model. Using these matrices, you can exchange model data between other users, vendors, or software packages without exchanging mesh or material data. Matrix representations of a model prevent the transfer of proprietary information and minimize the need for data manipulation.

The matrix generation procedure is a linear perturbation step (see “General and linear perturbation procedures,” Section 6.1.2) that accounts for all current boundary conditions, loads, and material response in a model. You can also specify new boundary conditions, loads, and predefined fields within the matrix generation step.

Specifying the matrix type

You can generate matrices representing the following model features:

  • stiffness,

  • mass,

  • viscous damping,

  • structural damping, and

  • loads.

The load matrix contains integrated nodal load vectors (right-hand sides) for the load cases defined in the matrix generation step. Load cases can be made up of any combination of loadings—distributed loads, concentrated nodal loads, thermal expansion, and load cases defined for any substructures that may be used as part of the model.

Input File Usage:          Use the following option to generate the stiffness matrix:
*MATRIX GENERATE, STIFFNESS

Use the following option to generate the mass matrix:

*MATRIX GENERATE, MASS

Use the following option to generate the viscous damping matrix:

*MATRIX GENERATE, VISCOUS DAMPING

Use the following option to generate the structural damping matrix:

*MATRIX GENERATE, STRUCTURAL DAMPING

Use the following option to generate the load matrix:

*MATRIX GENERATE, LOAD

Evaluating frequency-dependent material properties

When frequency-dependent material properties are specified in the model definition, Abaqus/Standard offers the option of choosing the frequency at which these properties are evaluated for use in global matrix generation. If you do not choose the frequency, Abaqus/Standard evaluates the matrices at zero frequency and does not consider the contributions from frequency-domain viscoelasticity.

Input File Usage:          
*MATRIX GENERATE, PROPERTY EVALUATION=frequency

Initial conditions

Matrix generation is a linear perturbation procedure. Therefore, the initial state for the matrix generation step is the state of the model at the end of the last general analysis step. The generated matrix includes initial stress and load stiffness effects due to preloads and initial conditions if nonlinear geometric effects are included in the analysis.

Boundary conditions

Boundary conditions can be defined or modified in a matrix generation step. For more information on defining boundary conditions, see “Boundary conditions,” Section 30.3.1. Any boundary conditions that are defined in a matrix generation step will not be used in subsequent general analysis steps (unless they are respecified).

Loads

All types of loads can be applied in the load cases for a matrix generation step. For more information on applying loads, see “Applying loads: overview,” Section 30.4.1. Any loads that are defined in a matrix generation step will not be used in subsequent general analysis steps (unless they are respecified).

Predefined fields

All types of predefined fields can be specified in a matrix generation procedure. For more information on specifying predefined fields, see “Predefined fields,” Section 30.6.1. Any predefined fields that are defined in a matrix generation step will not be used in subsequent general analysis steps (unless they are respecified).

Material options

All types of materials that are available in Abaqus/Standard can be used in a matrix generation procedure.

Elements

All of the elements that are available in Abaqus/Standard can be used in a matrix generation procedure. The elements are listed in Part VI, “Elements.”

Output

Generated matrices are output to a text file. The text file uses the following naming convention:

Job_MatrixStep.mtx
where Job is the name of the input file or analysis job, Matrix is a four-letter identifier indicating the matrix type (as outlined in Table 10.3.1–1), and Step is the step number in which the matrix is generated.

Table 10.3.1–1 Identifiers used in the generated matrix file name.

IdentifierMatrix Type
STIFStiffness matrix
MASSMass matrix
DMPVViscous damping matrix
DMPSStructural damping matrix
LOADLoad matrix
For example, if a stiffness matrix generation procedure is performed in the third step of an analysis job named VehicleFrame, the matrix is output to a file named VehicleFrame_STIF3.mtx.

The assembled sparse matrix operator data are written to the text file as a series of comma-separated lists. Each row in the file represents a single matrix entry; a row is written as a comma-separated list with the following elements:

  1. Row node label

  2. Degree of freedom for row node

  3. Column node label

  4. Degree of freedom for column node

  5. Matrix entry

For load matrices, which represent right-hand side vector data, each row in the text file is written with the following elements:

  1. Node label

  2. Right-hand side vector entry

If the matrix generation step has multiple load cases, the load matrices for each load case are separated by the following line in the text file:
** Loadcase
where Loadcase is the load case number.

Input file template

*HEADING
 …
**
*STEP
Options to define the preloading history for the model.
*END STEP
**
*STEP
*MATRIX GENERATE, STIFFNESS, MASS, LOAD
*BOUNDARY
Options to define the boundary conditions for the matrix generation step.
**
*LOAD CASE, NAME=LC1
Options to define the loading for the first load case.
*END LOAD CASE
**
*LOAD CASE, NAME=LC2
Options to define the loading for the second load case.
*END LOAD CASE
Any number of load cases can be defined.
*END STEP