Modify an Analysis Step with a Text Editor

Define a step with the proper time incrementation and nonlinear solution controls that best allow Simulation Composite Analysis to reach a converged solution.

We have already defined our model geometry with a 24-ply layup and are now ready to create a load step using a text editor. Many linear elastic analyses require only a single increment per step. However, a single increment is inadequate for simulations of progressive failure.

1. With the input file (.inp) already open, locate the step definition by searching for *STEP.
2. The step definition should now appear as:

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

   Note: If you have not yet created the LOAD_STEP, simply enter the lines of code above beneath the material definition.
3. For our example we will use 100 increments, so we modify the third line with 0.01, 1. 1E-05, 0.01.

   Here, the first term is the initial increment, the second is the time period step, the third is the minimum time increment allowed, and the fourth is the maximum time increment allowed.

   To achieve robust convergence when using Simulation Composite Analysis, the solution controls must be modified from their default state.

4. 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.

5. 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,

Back | Next