Nonlinear Solution Control Parameters

Modify the control parameters to work best with Helius PFA.

Solution Sequence

When Autodesk Inventor Nastran is used with Helius PFA, you must perform a nonlinear static analysis. This is specified in the Case Control section of the input file with the SOLUTION command:

SOL NLSTATIC

SOLUTION=NONLINEAR STATIC

SOL=106

Nonlinear Solution Controls

In Nastran, the default settings for the nonlinear solution process are based on the fundamental assumption of the Newton-Raphson algorithm. This states 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, especially 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 Nastran's NLPARM entry must be changed to allow Helius PFA to improve the convergence characteristics of the finite element simulation.

Create an NLPARM entry for each step of the analysis. Consider the example below from an input file:

NLPARM, 1, 20, ITER, 1, 1000, , , ,
, , , , 1000

In this example we have created a step and given it an identification number of 1. The identification number will be called in the Case Control section. This step has been defined to use 20 increments, but it can be adjusted to meet the needs of your analysis. Field 4 (DT) is left blank as it is not required for use with Helius PFA. In Field 5 we set the KMETHOD = ITER, which tells Nastran to update the stiffness matrix at every KSTEP iteration. Next, we set KSTEP = 1. Together, KMETHOD = ITER and KSTEP = 1, instruct Nastran to use the full Newton-Raphson iteration method and update the stiffness matrix at every iteration. These two fields must be set to ITER and 1, respectively, for use with Helius PFA.

In the MAXITER field we set the maximum number of iterations allowed for each increment to 1000. This is done to significantly increase the number of equilibrium iterations that Nastran will perform before evaluating the need to reduce the time incrementation. Next, we set INTOUT = ALL to output results for each increment. Finally, we set MAXDIV to 1000.

Energy-Based Degradation

When Energy-Based Degradation is used, the following parameters must be added to your input file:

PARAM, SOLUTIONERROR, ON
PARAM, FACTDIAG, 0.0

Together, these two solution parameters allow the model to push through the nonlinear equilibrium iterations near the final reduction in stiffness of the material at the integration point in question. In EBD, the stiffness of the material is reduced using discrete interval partitioning. As the stiffness approaches zero, Nastran can report a negative term in the stiffness matrix factor diagonal. If you receive Nastran Warning E5048, adding the two solution parameters above should address the issue. Refer to the SOLUTIONERROR parameter in the Nastran Reference Guide for further details.