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 a Response option:

Select Steady-state to omit the internal energy term (the specific heat term) in the governing heat transfer equation. For more information, see “Steady-state analysis” in “Uncoupled heat transfer analysis,” Section 6.5.2 of the ABAQUS Analysis User's Manual.

Select Transient to perform time integration with the backward Euler method in the pure conduction elements. This method is unconditionally stable for linear problems. For more information, see “Transient analysis” in “Uncoupled heat transfer analysis,” Section 6.5.2 of the ABAQUS Analysis User's Manual.

Note:  After you have selected a Response option, a message appears informing you that ABAQUS/Standard has selected the Default load variation with time option (located on the Other tabbed page) that corresponds to your Response selection. Click Dismiss to close the message dialog box.

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

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 a Type option:

Select Automatic if you want ABAQUS/Standard to determine suitable time increment sizes.

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.

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, 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.

If you selected Fixed in Step 2, enter a value for the constant time increment in the Increment size field.

If you selected Transient analysis on the Basic tabbed page, do the following:

Toggle on End step when temperature change is less than n if you want the analysis to end when the temperature at every temperature degree of freedom changes at a rate that is less than a rate that you specify. If you toggle on this option, enter the desired temperature change rate in the field provided.

If you selected Automatic in Step 2, enter a value for the Max. allowable temperature change per increment. ABAQUS/Standard restricts the time step to ensure that this value is not exceeded at any node (except nodes whose temperature degree of freedom is constrained via boundary conditions, MPC's, etc.) during any increment of the step.

If you selected Automatic in Step 2 and you are performing a cavity radiation analysis, enter a value for Max. allowable emissivity change per increment, or accept the default of 0.1. If this value is exceeded, ABAQUS/Standard cuts back the increment until the maximum change in emissivity is less than the specified value. See “Cavity radiation,” Section 32.1.1 of the ABAQUS Analysis User's Manual, for more information.

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 Equation Solver Method option of your choice:

Select Direct to use the default direct sparse solver.

Select Iterative to use the domain decomposition iterative linear equation solver. For more information, see “Iterative linear equation solver,” Section 6.1.5 of the ABAQUS Analysis User's Manual.

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.

ABAQUS/Standard automatically selects the Default load variation with time option that corresponds to your Response selection on the Basic tabbed page. It is recommended that you leave the Default load variation with time selection unchanged.

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.