Modify the Step Definition

Change the load step definition to perform optimally with Simulation Composite Analysis.

Many linear elastic analyses require only a single increment per step. A single increment is inadequate, however, when progressive failure is modeled because multiple increments are required to visualize the initiation and propagation of failure. Default nonlinear solution controls, as recommended in the Step Modifications for Abaqus/Standard Analyses section of the Simulation Composite Analysis User's Guide, are also modified.

1. If not already open, open ASCA_Tutorial_2_Abaqus_xs.inp.
2. Locate the step definition by searching for *Step.
3. The step definition should now appear as:

   *STEP, NAME=LOAD_STEP
   *STATIC
   1., 1., 1E-05, 1.

4. Replace the third line with 0.01, 1, 1e-05, 0.01
   • The first term is the initial increment, the second is the time period of the step, the third is the minimum time increment allowed, and the fourth term is the maximum time increment allowed.
5. On the next line, add the following solution controls statement:

   *Controls, parameters=time incrementation
   1000,1000,1000,1000,1000,,1000,,,10,

   These parameters allow Abaqus to take advantage of the enhanced convergence characteristics provided by Simulation Composite Analysis.

6. The modified step definition should look like the following:

   *STEP, NAME=LOAD_STEP
   *STATIC
   0.01, 1., 1E-05, 0.01
   *Controls, parameters=time incrementation
   1000,1000,1000,1000,1000,,1000,,,10,