A static stress procedure is one in which inertia effects are neglected. The analysis can be linear or nonlinear and ignores time-dependent material effects. For more information, see “Static stress analysis,” Section 6.2.2 of the ABAQUS Analysis User's Manual.
When you configure a static, general procedure, the Edit Step dialog box displays the Basic, Incrementation, and Other tabs. Settings you can configure with these tabbed pages include 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.
See the following sections for detailed instructions:
Use the Basic tabbed page to configure settings such as Nlgeom and stabilization.
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. For more information, see “Time period” in “Static stress analysis,” Section 6.2.2 of the ABAQUS Analysis User's Manual.
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.
Toggle on Use stabilization 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 the follow sections:
.If you toggled on Use stabilization, click the arrow to the right of the Use stabilization field, and select a method for defining the damping factor:
Select dissipated energy fraction to allow ABAQUS/Standard to calculate the damping factor from a dissipated energy fraction that you provide. Then enter a value for the dissipated energy fraction in the adjacent field (the default is 2.0 × 10–4). For more information, see “Using the dissipated energy fraction” in “Solving nonlinear problems,” Section 7.1.1 of the ABAQUS Analysis User's Manual.
Select damping factor to enter the damping factor directly. Then enter a value for the damping factor in the adjacent field. For more information, see “Using the damping factor” in “Solving nonlinear problems,” Section 7.1.1 of the ABAQUS Analysis User's Manual.
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.
Configure settings on the Incrementation and Other tabbed pages. See the following sections for detailed instructions:
Once you have finished configuring settings for the static, general step, click OK to close the Edit Step dialog box.
Use the Incrementation tabbed page to configure settings such as increment size and the maximum number of increments. For more information, see “Incrementation” in “Static stress analysis,” Section 6.2.2 of the ABAQUS Analysis User's Manual.
To configure incrementation settings:
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.
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 necessary, configure settings on the Basic and Other tabbed pages. See the following sections for detailed instructions:
Once you have finished configuring settings for the static, general step, click OK to close the Edit Step dialog box.
Use the Other tabbed paged to configure a variety of additional settings for a static, general step.
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.
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.
Select Contact iterations to use contact iterations instead of regular severe discontinuity iterations to speed up computations. Contact iterations are effective for the solution of large, geometrically linear, small-sliding, frictionless static problems with many severe discontinuity iterations.
If you select this technique, enter the following values:
Adjustment factor for the number of solutions in any iteration. This value is a correction factor on the maximum number of right-hand-side solutions during any contact iteration.
Maximum number of contact iterations. This value specifies the maximum number of contact iterations allowed before new global matrix assemblage and factorization.
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.
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 in the Incrementation tabbed page or the time period that you specified in 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.
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.
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.
If necessary, configure settings on the Basic and Incrementation tabbed pages. See the following sections for detailed instructions:
Once you have finished configuring settings for the static, general step, click OK to close the Edit Step dialog box.