| Abaqus Keywords Reference Guide |
|
| How to find keyword examples |
| Abaqus Keywords Reference Guide |
|
| How to find keyword examples |
This option is used to write element variables to the output database. It must be used in conjunction with the *OUTPUT option.
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE
Type: History data
Level: Step
Abaqus/CAE: Step module
Set this parameter equal to the name of the element set for which this output request is being made.
This parameter applies only to Abaqus/Explicit analyses using adaptivity.
Set this parameter equal to the name of the tracer set for which this output request is being made.
Include this parameter to indicate that output should be written for all section points in shell, beam, or layered solid elements for which output is requested. If this parameter is present, section points specified on the data lines are ignored.
This parameter applies only to Abaqus/Standard and Abaqus/Explicit analyses.
Set DIRECTIONS=YES (default) to write the element material directions to the output database. Set DIRECTIONS=NO to indicate that the element material directions should not be written to the output database.
Set this parameter equal to the name of the element set for which this output request is being made.
If this parameter and the EXTERIOR parameter are omitted, output will be written for all the elements in the model.
This parameter applies only to Abaqus/Standard and Abaqus/Explicit analyses.
Include this parameter to restrict output to only the exterior three-dimensional elements.
If this parameter and the ELSET parameter are omitted, output will be written for all the elements in the model.
Set POSITION=AVERAGED AT NODES if the values being written are the averages of values extrapolated to the nodes of the elements in the set. Averaging occurs only over elements that contribute to a node that have the same element type and properties. This parameter value is valid only in Abaqus/Standard analyses.
Set POSITION=CENTROIDAL if values are being written at the centroid of the element (the centroid of the reference surface of a shell element, the midpoint between the end nodes in a beam element). In Abaqus/CFD element output always uses POSITION=CENTROIDAL.
Set POSITION=INTEGRATION POINTS (default) if values are being written at the integration points at which the variables are actually calculated.
Set POSITION=NODES if the values being written are extrapolated to the nodes of each element in the set but not averaged at the nodes.
This parameter applies only to rebar in membrane, shell, and surface elements.
This parameter can be used to obtain output only for the rebar in the element set specified; output for the matrix material will not be given. It can be used with or without a value. If it is used without a value, the output will be given for all rebar in the element set. Its value can be set to the name assigned to the rebar on the *REBAR LAYER option to specify output for that particular rebar in the element set.
If this parameter is omitted in a model that includes rebar, the output requests govern the output for the matrix material only (except for section forces, when the forces in the rebar are included in the force calculation).
Rebar output can be obtained only in membrane, shell, or surface elements at the integration points and at the centroid of the element.
Set VARIABLE=ALL to indicate that all element variables applicable to this procedure and material type should be written to the output database.
Set VARIABLE=PRESELECT to indicate that the default element output variables for the current procedure type should be written to the output database. Additional output variables can be requested on the data lines.
If this parameter is omitted, the element variables requested for output must be specified on the data lines.
First line (optional, and relevant only if integration point variables are being written for shell, beam, or layered solid elements in an Abaqus/Standard analysis or if integration point variables are being written for shell or beam elements in an Abaqus/Explicit analysis):
Specify a list of the section points in the shell, beam, or layered solid at which variables should be written to the output database. If this data line is omitted, the variables are written at the default output points. For section points on a meshed beam cross-section, specify a list of user-defined section point labels. For elbow elements the mid-through-thickness section point must be specified to allow COORD data display in Abaqus/CAE since this point is not among the default output points. A maximum number of 16 section points can be specified. Repeat *ELEMENT OUTPUT as often as needed if output at additional points is required.
Second line:
Specify the identifying keys for the output variables to be written to the output database. The keys are defined in “Abaqus/Standard output variable identifiers,” Section 4.2.1 of the Abaqus Analysis User's Guide, “Abaqus/Explicit output variable identifiers,” Section 4.2.2 of the Abaqus Analysis User's Guide, and “Abaqus/CFD output variable identifiers,” Section 4.2.3 of the Abaqus Analysis User's Guide.
Repeat the second data line as often as necessary to define the list of variables to be output to the output database.