Modify the Material Definition

Replace the elastic material definition with a user material definition.

Simulation Composite Analysis uses a *User Material definition instead of conventional Abaqus material definitions. In this step, the *Elastic material definition is replaced with a *User Material definition that is formatted for Simulation Composite Analysis.

1. View Tutorial 1 and create the user material using the instructions provided in Characterize a User Material with Composite Material Manager.
2. Open ASCA_Tutorial_2_Abaqus.inp in a text editor.
3. Locate the beginning of the material definition by searching for the *Material keyword statement.
4. The entire material definition includes the following:

   *Material, name=ExampleMaterial
   *Elastic, type=LAMINA
    1.5e+07, 2e+06, 0.3, 800000., 800000., 450000.

5. In the *Material keyword statement, change the name of the material from ExampleMaterial to Tutorial_1. Note, the new material name must exactly match the name of a composite material stored in the Simulation Composite Analysis Material Database. For detailed information on creating and managing Simulation Composite Analysis materials, refer to the Material Manager User's Guide.
6. Delete the *Elastic keyword statement and the single data line that follows the keyword statement.
7. Add the *Depvar keyword after the *Material, name=Tutorial_1 line. The *Depvar keyword allocates memory for Simulation Composite Analysis solution-dependent state variables at each integration point.
8. Add 7 after the *Depvar line. The value of 7 indicates that 7 solution-dependent state variables must be tracked throughout the solution process. Seven is the default number of solution-dependent variables required by MCT.
9. Add the line *User Material, constants=16 after the state variable name assignments. The parameter "constants=16" indicates that there are 16 user material constants for this user material.
10. After the *User Material line, add:

    3, 1, 1, 0, 0, 0, 0, 0
    0, 0, 0, 0.1, 1E-06, 0, 0, 0

    • Two lines of user material constants are required since Abaqus permits a maximum of 8 user material constants per line. These sixteen user material constants are used by Simulation Composite Analysis to determine the precise form of multiscale constitutive relations to use for the composite material. In order, they specify:
      1. The system of units
      2. Fiber direction
      3. Progressive failure analysis
      4. Pre-fail non-linearity
      5. Stiffness degradation scheme
      6. Hydrostatic strengthening
      7. Temperature
      8. Failure criterion
      9. Auxiliary criterion parameter 1
      10. Auxiliary criterion parameter 2
      11. Element thickness
      12. Matrix post-failure stiffness
      13. Fiber post-failure stiffness
      14. Fiber Degradation Energy
      15. Unused
      16. Moisture.

      For detailed information on the user material constants, refer to Appendix A of the Simulation Composite Analysis User's Guide.

11. The new material definition should now look like the following:

    *MATERIAL, NAME=Tutorial_1
    *DEPVAR
    7
    *USERMATERIAL, CONSTANTS=16
    3, 1, 1, 0, 0, 0, 0, 0
    0, 0, 0, 0.1, 1E-06, 0, 0, 0