Inserting a New General Static Step
Inserting a general static step within the Simulation History indicates that a static solution procedure should be used for the computation of the system response to applied static or quasi-static time varying loads under given constraints. You can create environmental specifications (for example, boundary conditions and loads) within the step. General static steps are available only in a Nonlinear Structural case. They can be defined in new analysis cases or in analysis cases that contain other general static or static linear perturbation steps; they cannot be defined in analysis cases that contain heat transfer steps. However, analysis documents can contain additional cases with heat transfer steps. Sequentially coupled thermal-stress analyses, in which the stress/displacement solution is dependent on a temperature field but there is no inverse dependency, can be performed by reading the temperature solution from a heat transfer analysis case into a stress analysis case as a predefined field. See Step Sequence Restrictions for more information. Abaqus for CATIA V5 creates a General Static step by default for a new Nonlinear Structural case.
By default, geometrically nonlinear effects are considered for general static steps. See Accounting for Nonlinear Geometric Effects for more information.
Abaqus divides a step into increments so that it can follow the nonlinear solution path. Typically, you suggest the size of the first increment, and you allow Abaqus to choose the size of the subsequent increments automatically. This approach ensures that nonlinear problems are solved easily and efficiently. At the end of each increment the structure is in (approximate) equilibrium and results are available for writing to the output database file. Alternatively, you can specify a fixed increment size that will be used throughout the step. The latter approach is recommended only if you have considerable experience with a particular analysis case.
The ratio of the initial time increment to the total step time specifies the proportion of load applied in the first increment. The default initial increment size is the same as the total time period for the step. As a result, Abaqus applies all of the loads defined in the step in the first increment; if the problem is linear or mildly nonlinear, Abaqus will converge to a solution in a single increment. In contrast, if your model is highly nonlinear, Abaqus must reduce the increment size repeatedly in an attempt to converge to a solution. You can minimize the time spent reducing the increment size by providing a reasonable initial increment size; for most analyses an initial increment size that is 5% to 10% of the total step time is sufficient. This value will be modified as required if automatic incrementation is used or will be used as the constant time increment if fixed time incrementation is used.
Note: You can change the default loading behavior to apply all the loads instantaneously at the beginning of the step instead of gradually applying the loads during the step. However, instantaneous loading may prevent Abaqus from reaching a converged solution for models with significant nonlinearity since reducing the increment size will no longer correspond to a reduction in the applied loads.
In some geometrically nonlinear analyses, local instabilities may occur (e.g., surface wrinkling, material instability, or local buckling). If the problem is expected to be unstable, you can choose the automatic stabilization method available in Abaqus/Standard, in which damping is applied throughout the model to prevent instantaneous buckling or collapse.
This task shows you how to insert a new General Static step in a Nonlinear Structural case.
Select Start>Analysis & Simulation>Nonlinear Structural Analysis from the menu bar to enter the Nonlinear Structural Analysis workbench.
From the New Analysis Case dialog box, select Nonlinear Structural Case.
Abaqus for CATIA V5 creates a General Static step by default for a new Nonlinear Structural case.
To create an additional General Static step, do either of the following:
To append a new General Static step to the end of the Simulation History, click the General Static Step icon
.Tip: Alternatively, you can select Insert>General Static Step from the menu bar.
To insert a new General Static step between two existing steps in the Simulation History, right-click the step object in the specification tree after which you want to create the new step, then select Insert Step Below>General Static Step from the menu that appears.
You can change the step identifier by editing the Step name field. This name will be used in the specification tree.
Enter a description for the step in the Step description field.
If necessary, do the following to modify the Basic Step Data:
Edit the Step time field to specify a value for the total time period of the step.
Specify whether nonlinear geometric effects should be accounted for in the step by selecting Off or On for Nonlinear geometry. (The default value is On.) See Accounting for Nonlinear Geometric Effects for more information.
If necessary, do the following to modify the Incrementation Controls:
Select the Incrementation type: Automatic or Fixed. Automatic incrementation means that Abaqus will select increment sizes based on computational efficiency. Fixed incrementation means that you specify a fixed increment size; this option is recommended only if you have considerable experience with a particular analysis case.
Enter a value for the Maximum number of increments. The default number of increments for a step is 100; if significant nonlinearity is present in the simulation, the analysis may require many more increments. If Abaqus needs more increments than the specified upper limit to complete the step, it will terminate the analysis with an error message.
Enter a value for the Initial increment size. The ratio of the initial time increment to the total step time specifies the proportion of load applied in the first increment. The default initial increment size is the same as the total time period for the step. As a result, Abaqus applies all of the loads defined in the step in the first increment; if the problem is linear or mildly nonlinear, Abaqus will converge to a solution in a single increment. In contrast, if your model is highly nonlinear, Abaqus must reduce the increment size repeatedly in an attempt to converge to a solution. You can minimize the time spent reducing the increment size by providing a reasonable initial increment size; for most analyses an initial increment size that is 5% to 10% of the total step time is sufficient. This value will be modified as required if automatic incrementation is used or will be used as the constant time increment if fixed time incrementation is used.
Enter a value for the Minimum increment size. This parameter is used only for automatic time incrementation. The analysis will terminate if excessive cutbacks caused by convergence problems reduce the increment size below the minimum value.
Enter a value for the Maximum increment size. This parameter is used only for automatic time incrementation. By default, there is no upper limit on the increment size, other than the total step time. Depending on your simulation, you may want to specify a different maximum allowable increment size. For example, if you know that your simulation may have trouble obtaining a solution if too large a load increment is applied, perhaps because the model may undergo plastic deformation, you may want to decrease the maximum increment size.
If necessary, do the following to modify the Stabilization Controls:
Click More to access additional step options.
Select Use stabilization to use automatic stabilization if the problem is expected to be unstable due to instabilities caused by localized buckling behavior or by material instability. Such instabilities are especially significant when no time-dependent behavior exists in the material modeling. Abaqus can apply damping throughout the model in such a way that the viscous forces introduced are sufficiently large to prevent instantaneous buckling or collapse but small enough not to affect the behavior significantly while the problem is stable.
Select the Stabilization method: Dissipate Energy Fraction or Damping Factor.
With the Dissipate Energy Fraction method, Abaqus chooses the damping factor such that the dissipated energy during the step is a small fraction of the change in strain energy during the step.
Alternatively, you can specify the damping factor directly if you choose the Damping Factor method. The damping factor method is intended for advanced users. You should define the damping factor directly only in cases where a certain value is known to be effective in analyses similar to the current analysis case. See Static stress analysis in the Abaqus Analysis Guide for more information.
Edit the Stabilization factor field to specify a value for the stabilization factor (either the dissipated energy fraction or the damping factor, depending on the stabilization method chosen).
If necessary, do the following to modify the Default load variation with time:
Click More to access additional step options.
Select Instantaneous to apply all the loads at the start of the step.
Select Ramp linearly over step (if it is not already selected) to apply the loads incrementally over the step.
Click OK when you have finished defining the step.
The Static Step objects set contains a default Field Output Request object in a Field Output Requests objects set. See Requesting Results for more information.