Configuring a geostatic stress field procedure

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

2. On the Basic and Other tabbed pages, configure settings such as controls to include nonlinear effects of large displacements and equation solver preferences as described in the following procedures.

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

2. 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.

3. 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.

1. 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.)

2. Choose a Type option:

   • Choose Automatic if you want Abaqus/Standard to determine suitable time increment sizes.

   • Choose Fixed to use a fixed increment size.

     If you select Fixed, no further entries are available on the Incrementation tabbed page.

3. If you selected Automatic incrementation in Step 2, enter values for the Increment size and for the Max. displacement change:

   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.
   4. In the Max. displacement change field, enter the maximum amount of displacement that is acceptable while Abaqus/Standard calculates the equilibrium state for models in which the initial stress state is unknown or an approximation.

1. 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.)

2. 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.

3. 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.

4. 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.

5. 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.

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