Configuring a static, Riks procedure

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

2. On the Basic, Incrementation, and Other tabbed pages, configure settings such as stopping criteria, the maximum number of increments, the arc increment length, and whether to account for geometric nonlinearity 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.

4. 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.

5. Since the loading magnitude is part of the solution, you need a method to specify when the step is completed. Choose one or both of the following options:

   • Toggle on Maximum load proportionality factor to enter a maximum value for the load proportionality factor, ${\lambda }_{end}$. Abaqus/Standard uses this value to terminate the step when the load exceeds a certain magnitude. For more information, see Proportional loading

   • Toggle on Maximum displacement to enter a maximum displacement value at a specific degree of freedom (DOF). You must also specify the Node Region that Abaqus/Standard will monitor for finishing displacement. If this maximum displacement is exceeded, Abaqus/Standard terminates the step.

   If you leave both of these finishing conditions unspecified, the analysis continues for the number of increments that you specify on the Incrementation tabbed page.

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 to allow Abaqus/Standard to choose the size of the arc length increments based on computational efficiency.

   • Choose Fixed to specify direct user control of the incrementation. Abaqus/Standard uses an arc length increment that you specify as the constant increment size throughout the step. This method is not recommended for a Riks analysis since it prevents Abaqus/Standard from reducing the arc length when a severe nonlinearity is encountered.

   For more information, see Incrementation.

3. 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.

4. If you selected Automatic in Step 2, enter values for Arc length increment:

   1. In the Initial field, enter the initial increment in arc length along the static equilibrium path in scaled load-displacement space, $\mathrm{\Delta }{l}_{in}$.
   2. In the Minimum field, enter the minimum arc length increment, $\mathrm{\Delta }{l}_{min}$. If you enter zero, Abaqus assumes a default value of the smaller of the suggested initial arc length or 10⁻⁵ times the total arc length.
   3. In the Maximum field, enter the maximum arc length increment, $\mathrm{\Delta }{l}_{max}$. If this value is not specified, no upper limit is imposed.
   4. In the Estimated total arc length field, enter the total arc length scale factor associated with this step, $l_{period}$. If this entry is zero or is unspecified, Abaqus/Standard assumes a default value of $1.0$.

5. If you selected Fixed in Step 2, enter a value for the constant arc length increment in the Arc length increment field.

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 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.

3. 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.

4. 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 1% linear extrapolation of the previous incremental solution to begin the nonlinear equation solution for the current increment.

   • Select None to suppress any extrapolation.

   (The Parabolic option is not relevant for Riks analyses.) For more information, see Extrapolation of the solution.

5. 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 the maximum number of increments that you specified on the Incrementation tabbed page is exceeded.

6. 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.

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

7. 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, Riks step, click OK to close the Edit Step dialog box.