Specify Solution Controls with ANSYS APDL

Modify the parameters that govern the finite element solution to work optimally with Helius PFA.

The default solution controls in ANSYS typically do not allow for an efficient solution in a progressive failure problem. Specific solution control parameters allow for a solution with a decreased tendency for time increment cutbacks when used with Helius PFA. This results in a faster overall solution time.

We have already created our model geometry and are now ready to modify the solution controls.

1. Enter the following commands into the command prompt:
   • NROPT, FULL, , OFF - This command instructs ANSYS to use the 'Full' Newton Raphson algorithm and prevents it from using the 'Adaptive Descent' algorithm.
   • PRED, OFF, , OFF - This command prevents ANSYS from using the converged solution at the last substep to estimate the solution for the current substep.
   • TIME, 1 - Specifies a step size equal to 1.
   • NSUBST, 50, 50, 50 - This command specifies the number of substeps to be used in the analysis. Since the step time is 1, each substep time increment will be 0.02. Multiple substeps help to identify when failure initiates and how it progresses as the load increases.
   • NEQIT, 1000 - This command specifies the number of equilibrium iterations that must be performed before ANSYS evaluates the need to reduce the time increment size. It is intentionally large in order to force ANSYS to converge at each of the specified time steps.
2. Switch to the solution processor by clicking Main Menu > Solution. Enter the following command into the command prompt.
   • CNVTOL, F, , , 0 - This command is used to define the convergence tolerance for residual node forces.

Back | Next