Elements can be removed during an analysis by turning on the element deletion feature. If the element deletion feature is turned on, elements will be deleted when rupture occurs (SDV1 = 2).
When an element is deleted, all of the stresses in the element are set to zero and the element no longer has any energetic contribution to the simulation. Elements with multiple integration points are not deleted until each integration point is flagged for deletion. Until the element is deleted, all integration points have a non-zero stiffness and continue to contribute to the overall strain energy of the model, regardless of their individual deletion status.
Two steps are required to turn on element deletion:
- Enable element deletion in the export dialog
- Request output of the STATUS variable
Enable Element Deletion
To enable element deletion, you must turn on the Enable element deletion check box in the Export to Structural Package dialog. This feature is turned on by default.
When the Enable element deletion feature is turned on, Advanced Material Exchange will modify the input file to include the DELETE=2 parameter. This parameter will appear after the *DEPVAR keyword. For example:
*DEPVAR, DELETE=2 11
The DELETE=2 parameter can also be added using Abaqus/CAE or by manually editing the input file with a text editor.
Request Output
The STATUS variable must be included in the list of element outputs. For example:
*OUTPUT, FIELD *ELEMENTOUTPUT SDV, STATUS
The STATUS variable can be added to the output requests with Abaqus/CAE or by manually editing the input file with a text editor. With Abaqus/CAE:
- Click Output > Field Output Requests > Manager
- Click Edit
- Select STATUS from the list of output variables
- Click OK
