To configure settings on the Basic tabbed page:

In the Edit Step dialog box, display the Basic tabbed page.

(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)

In the Description field, enter a short description of what occurs during this analysis step. ABAQUS stores the text that you enter in the output database, and the text is displayed in the state block by the Visualization module.

Select an Nlgeom option:

Turn Nlgeom Off to perform a geometrically linear analysis during the current step.

Turn Nlgeom On to indicate that ABAQUS/Explicit should account for geometric nonlinearity during the step. Once you have turned Nlgeom on, it will be active during all subsequent steps in the analysis.

For more information, see “Linear and nonlinear procedures,” Section 14.3.2.

To configure settings on the Other tabbed page:

In the Edit Step dialog box, display the Other tabbed page.

(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)

Select the Matrix storage option of your choice:

Select Use solver default to allow ABAQUS/Standard to decide whether a symmetric or unsymmetric matrix storage and solution scheme is needed.

Select Unsymmetric to restrict ABAQUS/Standard to the unsymmetric storage and solution scheme.

Select Symmetric to restrict ABAQUS/Standard to the symmetric storage and solution scheme.

For more information on matrix storage, see “Matrix storage and solution scheme in ABAQUS/Standard” in “Procedures: overview,” Section 6.1.1 of the ABAQUS Analysis User's Manual.

Select the Solution technique of your choice:

Select Full Newton to use Newton's method as a numerical technique for solving nonlinear equilibrium equations. For more information, see “Nonlinear solution methods in ABAQUS/Standard,” Section 2.2.1 of the ABAQUS Theory Manual.

Select Quasi-Newton to use the quasi-Newton technique for solving nonlinear equilibrium equations. This technique can save substantial computational cost in some cases. Generally it is most successful when the system is large and the stiffness matrix is not changing much from iteration to iteration. You can use this technique only for symmetric systems of equations.

If you select this technique, enter a value for the Number of iterations allowed before the kernel matrix is reformed. The maximum number of iterations allowed is 25. The default number of iterations is 8.

For more information, see “Quasi-Newton solution technique,” Section 2.2.2 of the ABAQUS Theory Manual.

Select Contact iterations to use contact iterations instead of regular severe discontinuity iterations to speed up computations. Contact iterations are effective for the solution of large, geometrically linear, small-sliding, frictionless static problems with many severe discontinuity iterations.

If you select this technique, enter the following values:

• Adjustment factor for the number of solutions in any iteration. This value is a correction factor on the maximum number of right-hand-side solutions during any contact iteration.

• Maximum number of contact iterations. This value specifies the maximum number of contact iterations allowed before new global matrix assemblage and factorization.

For more information, see “Contact iterations,” Section 7.1.2 of the ABAQUS Analysis User's Manual.

Click the arrow to the right of the Convert severe discontinuity iterations field, and select an option for dealing with severe discontinuities during nonlinear analysis:

Select Off to force a new iteration if severe discontinuities occur during an iteration.

Select On to estimate residual forces associated with severe discontinuities and to check whether the equilibrium tolerances are satisfied. A solution may converge if the severe discontinuities (such as penetrations or tensile contact forces) are small. This option also changes some time incrementation parameters and uses different criteria to determine whether to do another iteration or to make a new attempt with a smaller increment size.

Select Propagate from previous step to use the value specified in the previous general analysis step. This value appears in parenthesis to the right of the field.