Multi-step simulations need not be defined in a single input file. Indeed, it is usually desirable to run a complex simulation in stages. This allows you to examine the results and confirm that the analysis is performing as expected before continuing with the next stage. The restart file allows an ABAQUS simulation to be restarted and the model's response to additional load history to be calculated.
The *RESTART option controls the writing of the restart file. While the option can appear anywhere in the input file, it normally appears as part of a step definition. As with other output request options, the values defined in a *RESTART option apply during the current step and any subsequent general steps, until the option is modified in a later step. The option
*RESTART, WRITE, FREQUENCY=<n>writes data to the restart file every nth increment. Restart data are also written at the end of each step, regardless of whether the last increment is divisible by n. If the FREQUENCY parameter is omitted, data are written every increment.
Restart files can become very large for large models, so it is often useful to include the OVERLAY parameter to control the size of the restart file. This parameter allows data to be overwritten on the restart file during a step. This means that at the end of the analysis there is only one set of restart data for each step, corresponding to the state of the model at the end of each step. However, if the analysis is interrupted for some reason, such as a computer malfunction, the analysis can be continued from the point where restart data were last written.
When restarting a simulation from the end of a previous analysis, use the READ parameter on the *RESTART option. You can also use the STEP and INC parameters to specify the particular point in the simulation's load history from which to restart the analysis. When performing a restart simulation, the *RESTART option should appear immediately after the *HEADING option. No model data need appear in this restart input file since the model data for the analysis will be read from the restart file. Only node set definitions, element set definitions, amplitude definitions, and additional history data can be modified in the restart input file.
Continuing an interrupted run
The new analysis continues directly from the specified step and increment of the previous analysis. If the given step and increment do not correspond to the end of the previous analysis, ABAQUS will simulate all of the remaining previously defined load history data before trying to simulate any new load history data provided in the input file. Therefore, if an analysis was interrupted by a computer malfunction, the following input file would complete the analysis as originally defined:
*HEADING Restart of interrupted run *RESTART, READ, STEP=<step>, INC=<increment>
Continuing with additional steps
If the previous analysis completed successfully and, having viewed the results, you want to add additional steps to the load history, the specified step and increment should be the last step and last increment of the previous analysis. Alternatively, they can be omitted and by default ABAQUS will read the last available data in the restart file. The *RESTART option is followed by any new step definitions.
*HEADING Add new step data *RESTART, READ, STEP=<last step>, INC=<last increment> *STEP ... new step definition... *END STEP
Changing an analysis
Sometimes, having viewed the results of the previous analysis, you may want to restart the analysis from an intermediate point and change the remaining load history data in some manner—for example, to add more output requests, to change the loading, or to adjust the analysis controls. Often this is necessary when a step has exceeded its maximum number of increments. If the analysis is restarted as described above, ABAQUS thinks that the analysis is partway through a step, tries to complete the step, and promptly exceeds the maximum number of increments again.
In such situations the END STEP parameter should be included on the *RESTART option to indicate that the current step should be terminated at the step and increment specified on the *RESTART option and all previously defined history data should be ignored. The simulation may then continue with the new steps defined after the *RESTART option. For example, if a step allowed only a maximum of 20 increments, which was less than the number of increments necessary to complete the step, the following restart input file would allow ABAQUS to restart the simulation and finish the applied load:
*HEADING Continue an analysis that exceeded the maximum number of increments *RESTART, READ, STEP=<step>, INC=20, END STEP *STEP, INC=100 ... repeat step definition... *END STEPIn this situation the entire step definition, including applied loads and boundary conditions, should be identical to that specified in the original run with the following exceptions:
The number of increments should be increased.
The total time of the new step should be the total time of the original step less the time completed in the step in the first run. For example, if the time of the step as originally specified was 100 seconds and the analysis ran out of increments at a step time of 20 seconds, the duration of the step in the restart analysis should be 80 seconds.
Any amplitude definitions specified in terms of step time need to be respecified to reflect the new time scale of the step. Amplitude definitions specified in terms of total time do not need to be changed, provided the modifications given above are used.
The magnitudes of any loads or prescribed boundary conditions remain unchanged since they are always total values in general analysis steps.