Create an Analysis Step

We need to define a step that allows us to increment the tensile load on the coupon. We'll also modify the solution controls for this load step to allow for a robust, converged solution.

1. Switch to the Step module
2. Create a new Static, General step (Step > Create) named Load_Step
3. Set the Initial and Maximum Increment size to 0.01 on the Incrementation tab of the Edit Step dialog box. Click OK

To achieve robust convergence when using Helius PFA, the solution controls must be modified from their default state.

1. Open the General Solution Controls dialog box by clicking Other > General Solution Controls > Edit > Load_Step from the main toolbar, ignore the warning, and click the Specify radio button
2. From the Time Incrementation tab enter 1000 for the values of both I₀ and I_R
3. Click the first tab labeled 'more' and enter 1000 for the values of I_P, I_C, I_L, and I_S. Set I_T to 10
   Note: Increasing these specific values will ensure Abaqus can take full advantage of the improved convergence characteristics provided by Helius PFA.
4. Click OK