Introducing a linear user-defined element (Abaqus/Standard only)
Required parameters
Optional parameters
- FILE
Set this parameter equal to the name of the results file (with no extension) from which the data are to be read. See Input Syntax Rules for the syntax of such file names.
This parameter can be used only if the user-defined element type is linear and its stiffness and/or mass matrices are to be read from the Abaqus/Standard results file of a previous analysis (in which they were written by using the ELEMENT MATRIX OUTPUT or SUBSTRUCTURE MATRIX OUTPUT options). When this parameter is used, all values are taken from the results file. For example, if the stiffness or mass being read from the results file is not symmetric, the UNSYMM parameter will be invoked automatically.
If this parameter is omitted, the data will be read from a standard input file.
- INTEGRATION
This parameter applies only to Abaqus/Standard analyses.
Set this parameter equal to the number of integration points to be used in Gauss integration. This parameter must be used in conjunction with the TENSOR parameter.
- TENSOR
This parameter applies only to Abaqus/Standard analyses.
Include this parameter to specify the element type. This parameter must be used in conjunction with the INTEGRATION parameter.
Set TENSOR=THREED to specify that it is a three-dimensional element in a stress/displacement or heat transfer analysis.
Set TENSOR=TWOD to specify that it is a two-dimensional element in a heat transfer analysis.
Set TENSOR=PSTRAIN to specify that it is a plane strain element in a stress/displacement analysis.
Set TENSOR=PSTRESS to specify that it is a plane stress element in a stress/displacement analysis.
Required parameters if the FILE parameter is included
- OLD ELEMENT
Set this parameter equal to the element number that was assigned to the element whose matrices are being read. This parameter can also be set to a substructure identifier to read a substructure matrix from an Abaqus/Standard results file.
- STEP
Set this parameter equal to the step number in which the element matrix was written. This parameter is not required if using a substructure whose matrix was output during its generation.
- INCREMENT
Set this parameter equal to the increment number in which the element matrix was written. This parameter is not required if using a substructure whose matrix was output during its generation.
Required parameters if the FILE parameter is omitted
- LINEAR
Include this parameter to indicate that the behavior of the element type is linear and is defined by a stiffness matrix and/or a mass matrix. The MATRIX option is required to define the element's behavior.
- NODES
Set this parameter equal to the number of nodes associated with an element of this type.
Optional parameters if the FILE parameter is omitted
- COORDINATES
Abaqus/Standard assigns space to store the coordinate values at each node in user subroutine UEL. The default number of coordinate values is equal to the largest active degree of freedom of the user element with a maximum of 3. Use the COORDINATES parameter to increase the number of coordinate values.
- UNSYMM
Include this parameter if the element matrices are not symmetric. This parameter will cause Abaqus/Standard to use its unsymmetric equation solution capability.
The presence or absence of this parameter determines the form in which the matrices must be provided for reading.
Data lines if the FILE parameter is omitted
- First line
Enter the list of active degrees of freedom at the first node of the element (as determined by the connectivity list). The rule in Conventions regarding which degrees of freedom can be used for displacement, rotation, temperature, etc. must be conformed to.
- Second line if the active degrees of freedom are different at subsequent nodes
Enter the position in the connectivity list (node position on the element) where the new list of active degrees of freedom first applies.
Enter the new list of active degrees of freedom.
Repeat the second data line as often as necessary.