Restarting an Analysis

Specifying the Frequency of Output to the Abaqus/Standard Restart File in Increments

By default, Abaqus/Standard will write data to the restart file after each increment at which the increment number is exactly divisible by a user-specified frequency value, N, and at the end of each step of the analysis (regardless of the increment number at that time). In a direct cyclic or a low-cycle fatigue analysis, Abaqus/Standard will write data to the restart file only at the end of a loading cycle; therefore, Abaqus/Standard will write data to the restart file after each iteration (or cycle in a low-cycle fatigue analysis) at which the iteration number (or cycle number in a low-cycle fatigue analysis) is exactly divisible by N and at the end of each step of the analysis.

RESTART, WRITE, FREQUENCY=N

Step module: OutputRestart Requests: enter N in the Frequency column for each step

Specifying the Frequency of Output to the Abaqus/Standard Restart File in Time Intervals

Abaqus/Standard can divide the step into a user-specified number of time intervals, n, and write the results at the end of each interval, for a total of n points for the step. If n is specified, by default data will be written to the results file at the exact times calculated by dividing the step into n equal intervals. Alternatively, you can choose to write the information at the increment ending immediately after the time dictated by each interval.

You can specify the frequency of restart output in time intervals only for the procedures listed in Table 1. In addition, this capability is not supported for linear perturbation analyses.

RESTART, WRITE, NUMBER INTERVAL=n, TIME MARKS=YES

RESTART, WRITE, NUMBER INTERVAL=n, TIME MARKS=NO

Step module: OutputRestart Requests: enter n in the Intervals column; toggle on the Time Marks column for each step if you want the results written at the exact time intervals

Time Incrementation

If the output frequency is specified in terms of the number of intervals, Abaqus/Standard will adjust the time increments to ensure that data are written at the exact time points specified. In some cases Abaqus might use a time increment smaller than the minimum time increment allowed in the step in the increment directly before a time point. However, Abaqus will not violate the minimum time increment allowed for consolidation, transient mass diffusion, transient heat transfer, transient couple thermal-electrical, transient coupled temperature-displacement, and transient coupled thermal-electrical-structural analyses. For these procedures if a time increment smaller than the minimum time increment is required, Abaqus will use the minimum time increment allowed in the step and will write restart data at the first increment after the time point.

When the output frequency is specified in terms of the number of intervals, the number of increments necessary to complete the analysis might increase, which might adversely affect performance.

Specifying the Frequency of Output to the Abaqus/Explicit State File

Abaqus/Explicit will divide the step into a user-specified number of time intervals, n, and write the results at the beginning of the step and at the end of each interval, for a total of n+1 points for the step, with the last point matching the end of the step. By default, the results will be written to the state file at the increment ending immediately after the time dictated by each interval. Alternatively, you can choose to write the results at the exact times calculated by dividing the step into n equal intervals.

If a problem precludes the analysis from continuing to completion, such as if an element becomes excessively distorted, Abaqus/Explicit will attempt to save the last completed increment in the state file.

Alternatively, you can specify the number of intervals as zero to turn off all restart frame output. This setting can be used to reduce the disk usage if there is no continuation after the current analysis.

RESTART, WRITE, NUMBER INTERVAL=n, TIME MARKS=NO

RESTART, WRITE, NUMBER INTERVAL=n, TIME MARKS=YES

RESTART, WRITE, NUMBER INTERVAL=0

Step module: OutputRestart Requests: enter n in the Intervals column; toggle on the Time Marks column for each step if you want the results written at the exact time intervals

Synchronizing Restart Information Written in a Co-Simulation

Restart output must be synchronized between co-simulation analyses for a co-simulation restart to be successful. You should request that restart data are written at the co-simulation target times when both solutions are considered at equilibrium. The SIMULIA Co-Simulation Engine supports a capability for the solvers participating in a co-simulation to synchronize writing restart data at target times. Any solver participating in the co-simulation can request that a restart frame is saved at an upcoming target time. This restart synchronization capability is supported only when the co-simulation participants support the option to synchronize.

You can set the number of time intervals, n, equal to 1 to indicate the co-simulation participants dictate when Abaqus writes restart data. In this case, restart data are always written at the end of the analysis step. You can set n to a value larger than 1 to divide the analysis step into n intervals to write restart data. The frequency of writing restart data is honored; however, the exact times depend on upcoming co-simulation target times.

You cannot request restart at specific time points in a co-simulation step.

RESTART, WRITE, NUMBER INTERVAL=1

RESTART, WRITE, NUMBER INTERVAL=n

Step module: OutputRestart Requests: enter n in the Intervals column

Specifying the Restart Point for an Abaqus/Standard Analysis (Except When Restarting from a Direct Cyclic or a Low-Cycle Fatigue Analysis)

An Abaqus/Standard analysis restarted from any analysis other than a direct cyclic or a low-cycle fatigue analysis will continue the analysis immediately after the user-specified step and increment. If you do not specify a step or increment, the analysis will restart at the last available step and increment found in the restart file.

RESTART, READ, STEP=step, INC=increment

Any module: ModelEdit Attributesmodel_name: Restart: toggle on Read data from job, Step name: step, toggle on Restart from increment, interval, iteration, or cycle, and enter the increment

Specifying the Restart Point for an Abaqus/Standard Analysis Restarted from a Direct Cyclic Analysis

An Abaqus/Standard analysis restarted from a previous direct cyclic analysis can be restarted only from the end of a loading cycle. In this case you should specify the step and iteration number at which the new analysis will be resumed.

In a direct cyclic analysis that has not reached a stabilized cycle on restart, you can increase the number of iterations or Fourier terms, thus allowing continuation of an analysis (see Direct Cyclic Analysis).

RESTART, READ, STEP=step, ITERATION=iteration

Any module: ModelEdit Attributesmodel_name: Restart: toggle on Read data from job, Step name: step, toggle on Restart from increment, interval, iteration, or cycle, and enter the iteration

Specifying the Restart Point for an Abaqus/Standard Analysis Restarted from a Low-Cycle Fatigue Analysis

An Abaqus/Standard analysis restarted from a previous low-cycle fatigue analysis can be restarted only from the end of a loading cycle. In this case you should specify the step and cycle number at which the new analysis will be resumed.

RESTART, READ, STEP=step, CYCLE=cycle

Any module: ModelEdit Attributesmodel_name: Restart: toggle on Read data from job, Step name: step, toggle on Restart from increment, interval, iteration, or cycle, and enter the cycle

Specifying the Restart Point for an Abaqus/Explicit Analysis

An Abaqus/Explicit restart analysis will continue the analysis immediately after the user-specified step and interval. You must specify the step from which an Abaqus/Explicit restart analysis will continue. If you do not specify an interval from which to restart or that the current step should be terminated at a specified interval, the analysis is restarted from the last interval available in the state file for the specified step.

RESTART, READ, STEP=step, INTERVAL=interval

Any module: ModelEdit Attributesmodel_name: Restart: toggle on Read data from job, Step name: step, toggle on Restart from increment, interval, iteration, or cycle, and enter the interval

Continuing an Abaqus/Standard Analysis without Changes

In Abaqus/Standard, in cases where restart is being performed simply to continue a long step (which might have been terminated because the time limit for the job was exceeded, for example), the data for the restart run might simply consist of the request to read restart data from another analysis.

RESTART, READ

Any module: ModelEdit Attributesmodel_name: Restart: toggle on Read data from job

Continuing an Abaqus/Explicit Analysis without Changes

In Abaqus/Explicit, in cases where restart is being performed simply to continue a long step (which might have been terminated because a CPU time limit was exceeded, for example), do not use a restart analysis; instead, use a recover analysis. In this case, no data are needed (unless user subroutines are being used).

Job module: job editor: toggle on Recover (Explicit) as the Job Type

Amplitude References

Care should be taken if loads and boundary conditions refer to amplitude curves (Amplitude Curves). If the amplitude is given in terms of total time, the loads and boundary conditions will continue to be applied according to the amplitude definition. However, if the amplitude is given in terms of step time (default), the loads and boundary conditions will be held constant at their values at the time the step is terminated.

Temperatures, field variables, and mass flow rates applied in the old step will remain in the new step if they are not redefined. If an amplitude curve was not specified, these quantities will continue to be applied according to the default amplitude for the procedure.

Automatic Stabilization in Abaqus/Standard

In Abaqus/Standard care should be exercised when automatic stabilization is active at the point at which a step is truncated. This might happen either in the middle of quasi-static procedures using automatic stabilization (see Solving Nonlinear Problems) or during contact analyses using automatic viscous damping (see Generally Applicable Contact Controls in Abaqus/Standard). In such cases viscous forces might be present, which will not be carried over to the subsequent step, therefore causing convergence difficulties.

In the case of quasi-static procedures using automatic stabilization, it is recommended that the stabilization continue to be enforced during the following step and that you specify the damping factor directly, using the last value printed out by Abaqus/Standard in the message file. In the case of automatic viscous damping in a contact pair when contact has not yet been fully established, it is recommended that the damping be applied again, although there is no guarantee that the amount of damping applied will be the same as in the original step.

Choosing the Initial Time Increment for an Abaqus/Standard Restart Analysis

In Abaqus/Standard take care in choosing the time period and initial time increment for the new step if the previous step was truncated. In transient analyses the initial time increment for the new step should be similar to the time increment that was used at the point of restart in the old step. In quasi-static analyses choose the initial time increment of the new step so that the increments in loads or prescribed boundary conditions are similar to those at the point of restart in the old step.

In a nonlinear analysis the increment of load applied in the first increment of the restart run should be similar to that applied in the last converged increment of the previous run. Let

$\mathrm{\Delta }{l}_1$

= the load to be applied in the first increment of the restart run,

$l_{\mathrm{rem}}$

= the remaining load to be applied in the restart run,

$\mathrm{\Delta }{t}_1$

= the initial time increment for the restart run, and

$t_{\mathrm{step}}$

= the total step time for the first step of the restart run.

The following equation can then be used to determine the initial time increment for the restart run:

Example

Suppose an Abaqus/Standard job stopped running because it reached the maximum number of increments specified for the step. The original input file was as follows:

HEADING
 …
STEP, INC=4
STATIC, DIRECT
 0.1, 1.0
CLOAD
 1, 2, 20.0
RESTART, WRITE, FREQUENCY=2
END STEP

This run ended at Step 1, increment 4 with a load of 8.0 applied. The following input file could be used to restart this job and to complete the loading:

HEADING
RESTART, READ, STEP=1, INC=4, END STEP
STEP, INC=120
STATIC, DIRECT
 0.1, 0.6
CLOAD
 1, 2, 20.0
END STEP

Notice that the concentrated load applied is the same as in the previous step.

In this example, assume that a load increment of 2.0 was applied in the last converged increment of the previous run. Therefore, the initial time increment for the restart run is chosen such that the load increment applied during the first increment is also 2.0. The remaining load to be applied in the restart run is 12.0 (20.0 total − 8.0 applied in the previous run). Substitution into the equation for the initial time increment yields $\mathrm{\Delta }{t}_1$ = $t_{\mathrm{step}}$ /6. The step time for the first step of the restarted job, $t_{\mathrm{step}}$ , is chosen to be 0.6 so that the total accumulated time is 1.0 when the applied load is 20.0 (at the end of the step). Thus, the initial time increment for the restart run, $\mathrm{\Delta }{t}_1$ , is set equal to 0.1.

Example

For example, suppose a one-step Abaqus/Explicit job stopped prior to completion because a CPU time limit was exceeded and you have decided that a second step should be added with new boundary condition definitions. The following input file could be used to restart this job, complete the remaining part of Step 1, and complete Step 2:

HEADING
RESTART, READ, STEP=1
**
** This defines Step 2
**
STEP
DYNAMIC, EXPLICIT
 , .003
BOUNDARY, OP=NEW
 …
END STEP