can be used to represent stiffness or mass for a part of the model or for the entire model;
is defined by giving it a unique name and by specifying matrix data, which may be scaled;
must be symmetric;
can be given in lower triangular, upper triangular, or square (lower and upper triangular) format;
can be used to provide linear elastic response with large translations but not large rotations;
can be used only with the symmetric equation solver in a static procedure or with either the Lanczos or AMS eigensolver;
can have loads, boundary conditions, and constraints applied directly to any matrix nodal degrees of freedom; and
can be used in submodeling analysis.
Designing complex models like automobiles typically involves subcontracting the work on various parts. When the entire model has to be put together, information about the parts needs to be exchanged between different vendors. In general, this information is exchanged in terms of matrices representing the stiffness, mass, and damping for each part. Mesh and material data are not exchanged, which avoids the transfer of proprietary information and minimizes the need for data manipulation (especially when exchanging data between different software packages). During an analysis these matrices are added to the corresponding global finite element matrices to complete the assembly of the entire model.
ABAQUS/Standard provides the capability to input stiffness or mass matrices directly. You can define as many different stiffness or mass matrices as are necessary to build the model.
You must assign a name to the matrix to include it in a model. The matrix is always treated as symmetric. You can specify a matrix as a lower triangular, upper triangular, or square matrix (containing both lower and upper triangular portions). However, a square matrix is considered symmetric only if the corresponding entries above and below the diagonal have exactly the same values. For example, if and are two of the entries for a square matrix (where i and j are row and column indices for the matrix), must equal for the matrix to be symmetric. ABAQUS/Standard will issue an error message if you specify only or for some entries of a square matrix; that is, the matrix has entries below and above the diagonal but the entries do not match.
|Input File Usage:|
*MATRIX INPUT, NAME=name
You can define a multiplication factor for all matrix entries.
|Input File Usage:|
*MATRIX INPUT, NAME=name, SCALE FACTOR=s
The matrix data can be contained in an alternate file. See Input syntax rules, Section 1.2.1, for the syntax of such file names. Typically, an alternate file is used for large matrices. To ensure acceptable performance, the data lines in the alternate file are read without extensive checking for data format. You should make sure that the data entries are specified in the proper format without any comments or blank lines.
|Input File Usage:|
*MATRIX INPUT, NAME=name, INPUT=input_file_name
You can assemble the stiffness and mass matrices that you have specified into the corresponding global finite element matrices for the model.
|Input File Usage:|
*MATRIX ASSEMBLE, STIFFNESS=sname, MASS=mname
A part represented by user-defined matrices is connected to other parts and finite elements through shared nodes. You must define these nodes directly in the model (see Node definition, Section 2.1.1). In addition, there may be nodes that define the part represented by matrices but that are not shared. You do not need to define nodes that are not shared and have no loads, boundary conditions, or constraints associated with them; these nodes will be defined for you and placed at the origin of the global coordinate system.
|Input File Usage:||Use the following option to define the shared nodes directly:|
Since the matrix data remain unchanged during the analysis, only linear elastic material behavior can be represented and only large translations can be modeled correctly in a geometrically nonlinear analysis. Changes to the matrix due to large rotations or load stiffness are not computed in a geometrically nonlinear analysis.
Only the symmetric equation solver is available for models that include matrices, which limits the matrix interface to handle only symmetric matrices.
User-defined matrices can be used in a natural frequency extraction analysis using the Lanczos or AMS eigensolver. Stiffness and mass matrices can be defined to represent portions of the model. For certain output quantities such as participation factors and inertia properties to be computed properly, the coordinates of the nodes used in the user-defined matrices should be defined.
Kinematic constraints (for example, coupling constraints, linear constraint equations, multi-point constraints, or surface-based tie constraints) can be applied to any nodes in a model containing matrices. However, matrix nodes or nodal degrees of freedom must be the independent nodes or nodal degrees of freedom in the constraint definition.
To apply contact constraints on matrix nodes, a node-based surface must be defined on these nodes and this surface should be used as the slave surface in the contact pair definition.
Nodal transformations defined at nodes that appear in the matrix do not affect the matrix. The matrix entries corresponding to these nodes are assumed to be in the local coordinates defined by the nodal transformations.
Initial conditions can be specified as usual; however, only node-based initial conditions can be applied to nodes that appear in matrices. See Initial conditions, Section 27.2.1.
Boundary conditions can be specified as usual. See Boundary conditions, Section 27.3.1. Matrix nodes can be defined as driven nodes in a submodel analysis (see Submodeling, Section 10.2.1); they cannot be defined as driving nodes in a global model. For shell-to-solid submodeling, matrix nodes that are defined as driven nodes are treated as lying within the center zone no matter how far they are from the shell reference surface.
Concentrated nodal forces can be applied at displacement degrees of freedom (1–6) of any node as usual. Distributed pressure forces can be applied to surface elements defined over matrix nodes (see Surface elements, Section 26.7.1). Body forces cannot be applied to parts of the model represented by matrices. User-defined loads can be applied with the same restrictions as above for distributed pressure forces and body forces.
Predefined fields can be applied at any nodes as usual (see Predefined field variables” in “Predefined fields, Section 27.6.1, and Predefined temperature” in “Predefined fields, Section 27.6.1); however, matrix data are not affected by predefined fields. For example, if temperatures are specified as a predefined field on nodes that appear on a matrix, only the elements that share these nodes with the matrix experience thermal strains if thermal expansion is specified for those elements. The matrix does not experience any thermal strains, but it may experience linear elastic forces due to displacements at shared nodes.
All elements that can be used in static stress analysis are available (see Choosing the appropriate element for an analysis type, Section 21.1.3).
All nodal output variables that apply to static analysis are available (see ABAQUS/Standard output variable identifiers, Section 4.2.1).
The following are known limitations to using matrices:
An analysis that contains matrices cannot be restarted. In addition, matrices cannot be introduced in a restart analysis.
Matrices cannot be used in a model containing parts and assemblies.
Matrices cannot be used in a substructure generation procedure.
Matrices containing acoustic pressure and mechanical degrees of freedom will disable coupled acoustic structural eigenvalue extraction.
*HEADING … *BOUNDARY Data lines to specify zero-valued boundary conditions *MATRIX INPUT, NAME=MAT1, SCALE FACTOR=sval Data lines to specify a matrix *MATRIX INPUT, NAME=MAT2, SCALE FACTOR=sval Data lines to specify a matrix *MATRIX ASSEMBLE, STIFFNESS=MAT1 *MATRIX ASSEMBLE, MASS=MAT2 *STEP(,NLGEOM)(,PERTURBATION) Use the NLGEOM parameter to include nonlinear geometric effects; it will remain active in all subsequent steps. *STATIC *BOUNDARY Data lines to prescribe zero-valued or nonzero boundary conditions *CLOAD and/or *DLOAD Data lines to specify loads *END STEP *STEP *FREQUENCY *END STEP