Nonlinear Solution Control Parameters

Modify the solution control parameters using a text editor.

It is widely accepted that good convergence (or any convergence at all) is difficult to achieve in progressive failure simulations of composite structures. In fact, many progressive failure simulations terminate early, not due to global structural failure, but simply due to the inability of the finite element code to obtain a converged solution at a particular load step. One of the major advantages of Helius PFA is that it has been optimized to significantly improve the overall convergence rate and robustness of progressive failure simulations of composite structures. However, in order to take full advantage of the superior convergence characteristics, you must change some of the default settings that govern the nonlinear solution process used by ANSYS. These changes can be enacted using the NROPT, PRED, NSUBST, CNVTOL, and NEQIT commands.

Regardless whether the SOLCONTROL command is ON (default) or OFF, you will need to override these nonlinear solution control parameters.

NROPT

The NROPT command is used to do two things: a) instruct ANSYS to use the 'Full' Newton Raphson algorithm, and b) prevent ANSYS from using their 'Adaptive Descent' algorithm to help the solution process. An example of the NROPT command fulfilling these two requirements is shown below.

NROPT, FULL, , OFF

In ANSYS, the nonlinear solution process is based on the fundamental assumption of the Newton-Raphson algorithm that the nonlinear response of the composite structure is sufficiently smooth at both the global and local levels. However, in a progressive failure simulation of a composite structure, the nonlinear response of the composite structure is not smooth. This is especially true at the local level where material failure results in an instantaneous reduction of material moduli. This non-smooth material response is one of the primary factors responsible for the difficulty in obtaining convergence in progressive failure simulations. Helius PFA's method of managing material nonlinearity is specifically designed to handle this localized non-smooth material response. However, the default settings of ANSYS' nonlinear solution control parameters must be changed to allow it to improve the convergence characteristics of the finite element simulation.

PRED

The PRED command prevents ANSYS from using the converged solution at the last substep to estimate the solution for the current substep. This interferes with Helius PFA's method of managing material linearity. An example of the PRED command that fulfills this is shown below.

PRED, OFF, , OFF

NSUBST

The NSUBST command specifies the minimum and maximum allowable number of substeps for the current load step. Autodesk does not recommend any minimum or maximum values and engineering judgment should be exercised. However, provided that enough equilibrium iterations are allowed per substep (discussed under NEQIT heading), Helius PFA will always find a converged solution. This is a deviation from typical nonlinear solution processes where multiple substep size cutbacks may be required. Helius PFA will converge at each substep, regardless of the size (again provided that enough equilibrium iterations are allowed per substep), so care must be taken when deciding on substep size.

CNVTOL

The CNVTOL command defines the convergence tolerance for residual node forces. There are two arguments set in this command that allow Helius PFA to better handle the nonlinear solution process: a) set forces (F) as the convergence label, and b) set the norm selection to infinite norm (check each DOF separately). An example of the CNVTOL command that fulfills these two items is shown below.

CNVTOL, F, , , 0

NEQIT

The NEQIT command specifies the minimum number of equilibrium iterations that must be performed before ANSYS evaluates the need for cutting-back the size of the current substep. Helius PFA has the unique ability to converge regardless of the substep size or extent of nonlinearity occurring during the substep. In the experience of Autodesk, convergence always occurs when the number of equilibrium iterations allowed per substep, before a substep cutback occurs is set to 1000. An example of what this command looks like is shown below.

NEQIT, 1000