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.

In the Time period field, enter a time scale for the analysis.

Select an Nlgeom option:

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

Turn Nlgeom On to indicate that ABAQUS/Standard 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.

Toggle on Include adiabatic heating effects if you are performing an adiabatic stress analysis. This option is relevant only for isotropic metal plasticity materials with a Mises yield surface. For more information, see “Adiabatic analysis,” Section 6.5.5 of the ABAQUS Analysis User's Manual.

To configure settings on the Incrementation tabbed page:

In the Edit Step dialog box, display the Incrementation 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 Type option of your choice:

Select Automatic to allow ABAQUS/Standard to choose the increment sizes based on computational efficiency.

Select Fixed to specify direct user control of the incrementation. ABAQUS/Standard uses an increment size that you specify as the constant increment size throughout the step.

Fixed incrementation is not generally recommended; it should be used only in special cases when you have a thorough understanding of how to interpret results obtained in this way. Impact events are particularly difficult to solve using fixed time increments.

In the Maximum number of increments field, enter the upper limit to the number of increments in the step. The analysis stops if this maximum is exceeded before ABAQUS/Standard arrives at the complete solution for the step.

If you selected Automatic in Step 2, do the following:

Enter values for Increment size:

In the Initial field, enter the initial time increment. ABAQUS/Standard modifies this value as required throughout the step.

In the Minimum field, enter the minimum time increment allowed. If ABAQUS/Standard needs a smaller time increment than this value, it terminates the analysis.

In the Maximum field, enter the maximum time increment allowed.

In the Half-step residual tolerance field, enter the equilibrium residual error (out-of-balance forces) halfway through a time increment.

This half-step residual check is the basis of the adaptive time incrementation scheme. If the half-step residual is small, it indicates that the accuracy of the solution is high and that the time step can be increased safely; conversely, if the half-step residual is large, the time step used in the solution should be reduced. For more information, see “Automatic time incrementation” in “Implicit dynamic analysis using direct integration,” Section 6.3.2 of the ABAQUS Analysis User's Manual.

If you selected Fixed in Step 2, do the following:

Enter a value for the constant time increment in the Increment size field.

If desired, toggle on Suppress half-step residual calculation to reduce the solution cost.

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.

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.

Select an option for Default load variation with time:

Select Instantaneous if you want loads to be applied instantaneously at the start of the step and remain constant throughout the step.

Select Ramp linearly over step if the load magnitude is to vary linearly over the step, from the value at the end of the previous step to the full magnitude of the load.

Click the arrow to the right of the Extrapolation of previous state at start of each increment field, and select a method for determining the first guess to the incremental solution:

Select Linear to indicate that the process is essentially monotonic and ABAQUS/Standard should use a 100% linear extrapolation, in time, of the previous incremental solution to begin the nonlinear equation solution for the current increment.

Select Parabolic to indicate that the process should use a quadratic extrapolation, in time, of the previous two incremental solutions to begin the nonlinear equation solution for the current increment.

Select None to suppress any extrapolation.

For more information, see “Extrapolation of the solution” in “Procedures: overview,” Section 6.1.1 of the ABAQUS Analysis User's Manual.

In the Numerical damping control parameter field, enter a value for the numerical (artificial) damping control parameter, , in the implicit operator. Allowable values are zero (no damping) to –0.333 (maximum damping). The default is –0.05, which provides slight numerical damping. For more information, see “Artificial damping” in “Implicit dynamic analysis using direct integration,” Section 6.3.2 of the ABAQUS Analysis User's Manual.

By default, ABAQUS/Standard calculates accelerations at the beginning of a dynamic step. However, you can toggle on Bypass calculations of initial accelerations at the beginning of step if you prefer the following approach:

If the current step is the first dynamic step, ABAQUS/Standard assumes that the initial accelerations for the current step are zero.

If the immediately preceding step was also a dynamic step, ABAQUS/Standard uses the accelerations from the end of the previous step to continue the new step.

This approach is appropriate only if the loading does not change suddenly at the start of the new step. For more information, see “Controlling calculation of accelerations at the beginning of a dynamic step” in “Implicit dynamic analysis using direct integration,” Section 6.3.2 of the ABAQUS Analysis User's Manual.

If you selected Fixed time incrementation on the Incrementation tabbed page, you can toggle on Accept solution after reaching maximum number of iterations. This option directs ABAQUS/Standard to accept the solution to an increment after the maximum number of iterations allowed has been completed, even if the equilibrium tolerances are not satisfied. Very small increments and a minimum of two iterations are usually necessary if you use this option.

This approach is not recommended; you should it only in special cases when you have a thorough understanding of how to interpret results obtained in this way.