Configuring a static, general procedure

Display the Edit Step dialog box following the procedure outlined in Creating a step (Procedure type: General; Static, General), or Editing a step.

On the Basic, Incrementation, and Other tabbed pages, configure settings such as the time period for the step, the maximum number of increments, the increment size, the default load variation with time, and whether to account for geometric nonlinearity as described in the following procedures.

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

In the Description field, enter a short description of the 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 the time period of the step. For more information, see Time period.

Select an Nlgeom option:

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

• Toggle Nlgeom On to indicate that Abaqus/Standard should account for geometric nonlinearity during the step. Once you have toggled Nlgeom on, it will be active during all subsequent steps in the analysis.

For more information, see Linear and nonlinear procedures.

Select an automatic stabilization method if you expect the problem to have local instabilities such as surface wrinkling, material instability, or local buckling. Abaqus/Standard can stabilize this class of problems by applying damping throughout the model. For more information, see Unstable problems, and Automatic stabilization of static problems with a constant damping factor

Click the arrow to the right of Automatic stabilization, and select a method for defining the damping factor:

• Select Specify dissipated energy fraction to allow Abaqus/Standard to calculate the damping factor from a dissipated energy fraction that you provide. Enter a value for the dissipated energy fraction in the adjacent field (the default is 2.0 × 10⁻⁴). For more information, see Calculating the damping factor based on the dissipated energy fraction.

• Select Specify damping factor to enter the damping factor directly. Enter a value for the damping factor in the adjacent field. For more information, see Directly specifying the damping factor.

• Select Use damping factors from previous general step to use the damping factors at the end of the previous step as the initial factors in the current step's variable damping scheme. These factors override any initial damping factors that are calculated or specified directly in the current step. If there are no damping factors associated with the previous general step (for example, if the previous step does not use any stabilization or the current step is the first step of the analysis), Abaqus uses adaptive stabilization to determine the required damping factors.

When using automatic stabilization, Abaqus can use the same damping factor over the course of a step, or it can vary the damping factor spatially and temporally during a step based on the convergence history and the ratio of the energy dissipated by damping to the total strain energy. For more information, see Adaptive automatic stabilization scheme. If you selected Specify dissipated energy fraction, adaptive stabilization is optional and turned on by default. If you selected Specify damping factor, adaptive stabilization is optional and turned off by default. If you selected Use damping factors from previous general step, adaptive stabilization is required.

To use adaptive stabilization, toggle on Use adaptive stabilization with max. ratio of stabilization to strain energy (if necessary), and enter a value in the adjacent field for the allowable accuracy tolerance for the ratio of energy dissipated by damping to total strain energy in each increment. The default value of 0.05 should be suitable in most cases.

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.

When you have finished configuring settings for the static, general step, click OK to close the Edit Step dialog box.

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

(For information on displaying the Edit Step dialog box, see Creating a step, or Editing a step.)

Choose a Type option:

• Choose Automatic to allow Abaqus/Standard to choose the size of the time increments based on computational efficiency.

• Choose 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:

1. In the Initial field, enter the initial time increment. Abaqus/Standard modifies this value as required throughout the step.
2. 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.
3. 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.

When you have finished configuring settings for the static, general step, click OK to close the Edit Step dialog box.

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

(For information on displaying the Edit Step dialog box, see Creating a step, or Editing a step.)

Choose an Equation Solver Method option:

• Choose Direct to use the default direct sparse solver.

• Choose Iterative to use the iterative linear equation solver. The iterative solver is typically most useful for blocky structures with millions of degrees of freedom. For more information, see Iterative linear equation solver.

Choose a Matrix storage option:

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

• Choose Unsymmetric to restrict Abaqus/Standard to the unsymmetric storage and solution scheme.

• Choose 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.

Choose a Solution technique:

• Choose 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.

• Choose 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 choose 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.

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, regardless of the magnitude of the penetration and force errors. 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 On to use local convergence criteria to determine whether a new iteration is needed. Abaqus/Standard will determine the maximum penetration and estimated force errors associated with severe discontinuities and check whether these errors are within the tolerances. Hence, a solution may converge if the severe discontinuities are small.

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

For more information on severe discontinuities, see Severe discontinuities in Abaqus/Standard.

Choose an option for Default load variation with time:

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

• Choose 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.

Toggle on Stop when region region name is fully plastic if “fully plastic” analysis is required with deformation theory plasticity. If you toggle on this option, enter the name of the region being monitored for fully plastic behavior.

The step ends when the solutions at all constitutive calculation points in the element set are fully plastic (defined by the equivalent strain being 10 times the offset yield strain). However, the step can end before this point if either the maximum number of increments that you specified on the Incrementation tabbed page or the time period that you specified on the Basic tabbed page is exceeded.

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.

Toggle on Obtain long-term solution with time-domain material properties to obtain the fully relaxed long-term elastic solution with time-domain viscoelasticity or the long-term elastic-plastic solution for two-layer viscoplasticity. This parameter is relevant only for time-domain viscoelastic and two-layer viscoplastic materials.

When you have finished configuring settings for the static, general step, click OK to close the Edit Step dialog box.