Modify the Material Definition

Change the material definition from an elastic material type to a user-defined material type.

The materials processed by Simulation Composite Analysis are considered by ANSYS to be user-defined material types, as opposed to the standard material types recognized by ANSYS. The unmodified input file for this Tutorial uses MP commands to define an orthotropic elastic material. Hence, the material definition needs to be changed from an elastic material type to a user-defined material type.

The specific format of a Simulation Composite Analysis user-defined material command is given by:

COMPAN, MATID, NSTATV, UNITS, PFIB_DIR, PFA, PREFAIL, unused, PRESS, TEMP,FAIL_CRITERION,AUX_1,AUX_2,unused, MDEG, FDEG, MOISTURE

For detailed information regarding each argument in the COMPAN command, refer to Appendix A of the Simulation Composite Analysis User's Guide.

The following steps modify the COMPAN command for this exercise.

  1. Open Tutorial 1 and create the user material (which is named Tutorial_1) using the instructions provided in Tutorial 1 (Characterize a User Material with Composite Material Manager).
  2. Determine the ANSYS Material ID (matID) number for Tutorial_1 by opening the Simulation Composite Analysis plug-in from within ANSYS and selecting Tutorial_1 from the Material Library list. The location of the Material ID number is highlighted below. Alternatively, the matID can be determined by opening the ASCAMatDB.xml file, which is located in the Simulation Composite Analysis Material directory. The particular value of the Material ID may differ depending on the number of materials in your Simulation Composite Analysis Material directory.

  3. Locate the section containing the MP commands within ASCA_Tutorial_2_ANSYS.ans.
  4. Replace the set of MP commands with the following, ensuring that matID is replaced with the value determined in step 1: 
    COMPAN, matID, 7,3,1,1,0,0,0,0,0,0,0,0,0.1,0.01,0

    The above command consists of constants that communicate user options in Simulation Composite Analysis. In order, they specify:

    1. Material ID for Simulation Composite Analysis material
    2. Number of state variables to track
    3. The system of units
    4. Fiber direction
    5. Progressive failure analysis
    6. Pre-fail non-linearity
    7. Unused
    8. Hydrostatic strengthening
    9. Temperature
    10. Failure criterion
    11. Auxiliary criterion parameter 1
    12. Auxiliary criterion parameter 2
    13. Unused
    14. Matrix post-failure stiffness
    15. Fiber post-failure stiffness
    16. Moisture
  5. If necessary, change the matID in the section definition (secdata commands) to match the matID determined in step 1.
Parent topic: Tutorial 2 - Modify an ANSYS Input File for use with Simulation Composite Analysis