Now that we have created a load step and defined the nonlinear solution controls, we are ready to specify output to the results file. To examine the fiber and matrix damage states generated by Simulation Composite Analysis in Abaqus/Viewer, you must first request state dependent variable (SDV) output to the results file.
- Locate the output definition by searching for *Output.
- The definition should appear as:
*OUTPUT, FIELD, VARIABLE=PRESELECT
- Delete, VARIABLE=PRESELECT. This parameter indicates that the default list of output variables will be written to the output database. State variables are not included in this list, so each output variable must be requested individually.
- Add the following lines:
*Element Output, directions=YES
1, 2, 3, 4, 5, 6, 7, 8, 9, 10, 11, 12, 13, 14, 15, 16
S, E, SDV
*Element Output, directions=YES
17, 18, 19, 20, 21, 22, 23, 24
S, E, SDV
- The first line, *Element Output, directions=YES, writes the element variables and section points to the output database. The directions=YES parameter indicates that element material directions should be written to the database.
- The second line, 1, 2, 3, ... indicates specific section points in the layered element where the output variables are computed. Two instances of these commands are required since the maximum number of section points allowed per line is 16.
- The third line, S, E, SDV is a list of variable identifying keys. S represents stress components, E represents total strain components, and SDV represents state variables.
- The definition should now read:
*OUTPUT, FIELD, VARIABLE=PRESELECT
*Element Output, directions=YES
1, 2, 3, 4, 5, 6, 7, 8, 9, 10, 11, 12, 13, 14, 15, 16
S, E, SDV
*Element Output, directions=YES
17, 18, 19, 20, 21, 22, 23, 24
S, E, SDV
- Save the file.
The only modification specific to Simulation Composite Analysis is the addition of SDV to the list of element output variable identifying keys.
Back