The analysis restart capability in Abaqus for CATIA V5 allows you to run a new analysis using the results from a previous analysis as the starting point. If a previous analysis failed, you can resume the simulation from the most recent successful increment after addressing the cause of the failure (disk space, convergence problems, etc.). If your model contains multiple steps, you do not have to analyze all of the steps in a single analysis case; instead, you can examine intermediate results and confirm that the analysis is performing as expected before continuing with the next stage in another analysis case. The results of a previous analysis can also form the preloaded base state of a new restart analysis or analyses.
You can restart an analysis from any increment in the original analysis during which restart data were written. By default, restart data are not written for Nonlinear Structural cases and Thermal cases. Restart data are written by default at the end of every step in an Abaqus Explicit Dynamics case. You can adjust the frequency at which restart data are written for all cases.
Use the Restart tabbed page to control the writing and reading of restart data. You can request that Abaqus write restart data after a regular number of increments or at regular intervals throughout a step; in either case Abaqus writes restart data at the end of each step. If you are defining a restart job, you must specify the increment in the previous analysis from which you want to continue the analysis.
When configuring a restart job, you indicate the name of the job that ran the previous analysis and select the step and increment from which to resume the analysis. The following files from the previous job must be present in the computation directory for the restart job (see Specifying File Storage Directories):
Restart (.res) file
Model (.mdl) file
State (.stt) file
Part (.prt) file
Abaqus/Explicit state (.abq) file (Explicit Dynamics cases only)
Package (.pac) file (Explicit Dynamics cases only)
Selected results (.sel) file (Explicit Dynamics cases only)
You can create a restart job based on restart data in the same analysis case as the new job (to complete an aborted analysi, for example) or in a different analysis case (to add steps to a previous analysi, for example). For more information about restart capabilities in Abaqus, see Restarting an analysis in the Abaqus Analysis Guide.
This task shows you how to configure a restart analysis.
In the job editor, click the Restart tab to display the Restart tabbed page.
Use the Restart Write options to control whether restart data is written during the analysis job. You can choose one of the following options:
None
No restart data are written.
Every increment
Restart data are written after every increment, including at the end of each step.
This option is not available in an Explicit Dynamics case.
Last increment
Restart data are written at the end of each step and after the last increment of the analysis.
This option is not available in an Explicit Dynamics case.
Frequency
Restart data are written every specified number of increments. For example, if you specify a frequency of two, restart data are written after increments 2, 4, 6, etc. Restart data are also written at the end of each step.
This option is not available in an Explicit Dynamics case.
Number interval
A step is divided into the specified number of intervals and restart data are written at the end of each interval.
When Abaqus uses a variable incrementation scheme, the end of a step interval may not line up exactly with the end of an increment. By default, Abaqus writes restart data at the increment that ends immediately after the specified interval time. To force Abaqus to adjust the incrementation scheme to line up exactly with the step intervals, toggle on Time marks.
If you request the writing of restart data multiple times per step, toggle on Retain only latest increment data to request that Abaqus retain restart data for only one increment per step, thus minimizing the memory consumed. Restart data from each increment that Abaqus writes overlays the data from the previous increment for the same step. Regardless of the setting, Abaqus writes the restart data for the last increment of each step.
If you selected a Restart job on the Submission tabbed page, you must complete the Restart Read options on the Restart tabbed page.
In the Read data from job field, enter the name of the job that ran the analysis you are restarting.
Specify the step in the previous analysis from which you want to restart the new job.
If the previous analysis is open in the specification tree, choose Select step, and select the appropriate step from the specification tree.
To specify the step number directly, choose Step number, and enter the appropriate step number.
Specify the increment within the selected step from which you want to restart the new job.
Choose End of step to restart the analysis from the final increment in the specified step.
Choose Increment/Interval, and enter a specific increment (for Structural and Thermal cases) or interval (for Explicit Dynamics cases) number from which you want to restart the new job.
If you are restarting the analysis from an intermediate increment or interval in a step, specify whether or not Abaqus should complete the step from the previous analysis in the new job.
Choose Terminate the step to end the previous step at the specified increment or interval, then continue with any new steps defined in the restart job.
Choose Complete the step to complete the previous step before continuing with any new steps defined in the restart job.
Click OK to close the job editor and to save your settings.