Create an Analysis Step and Define Solution Controls

Define a step allowing boundary conditions and output requests to be added to the model.

1. Switch to the Step module.
2. Create a new Static, General step (Step > Create) named Load_Step.
3. On the Basic tab of the Edit Step dialog box, turn Nlgeom On.
4. On the Incrementation tab, set the Initial and Maximum Increment size to 0.01 and set the Maximum number of increments to 1000.
   • Helius PFA normally prevents analyses from cutting back the increment size. However, when non-linear geometry is used, Abaqus may be forced to reduce the increment size in order to resolve geometric convergence difficulties. Therefore, it is a good habit to increase the maximum number of increments in case geometric convergence issues are encountered.
5. On the Other tab, change Extrapolation from Linear to None.
   • Setting the Extrapolation option to None is required only for analyses that use Helius PFA Cohesive materials.
6. Click OK.

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

7. 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.
8. From the Time Incrementation tab enter 1000 for the values of both I₀ and I_R.
9. 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.

   Increasing these specific values will ensure that Abaqus can take full advantage of the improved convergence characteristics provided by Helius PFA.

10. Click OK.