Products: ABAQUS/Standard ABAQUS/Explicit ABAQUS/CAE
When you run an analysis, you can write the model definition and state to the files required for restart. In ABAQUS/Standard these files are the restart (job-name.res), analysis database (.mdl and .stt), part (.prt), and output database (.odb) files. In ABAQUS/Explicit these files are the state (.abq), analysis database (.stt), part (.prt), and output database (.odb) files. These files, collectively referred to as the restart files, allow an analysis to be completed up to a certain point in a particular run and restarted and continued in a subsequent run. The output database file only needs to contain the model data; results data are not required and can be suppressed.
Multiple analysis database files may exist in ABAQUS/Standard if the elements are reordered during the analysis. In such a case the analysis database is split into multiple files, each file corresponding to a particular element ordering. When this occurs, a sequence identifier is attached to the job name (for example, job-name_seq_n.stt and job-name_seq_n.mdl). ABAQUS/Standard will map the step and increment number (or iteration number in the case of a direct cyclic analysis) automatically to a particular database. You should retain all analysis database files if an analysis will be continued from any increment saved to the restart database. If you are interested only in restarting at the end of the analysis, all analysis database files except the last one (the one with the highest sequence identifier) may be removed.
“Output,” Section 4.1.1, describes the process of obtaining results output from an ABAQUS/Standard restart file.
If you want to be able to restart an analysis, you must request that the files required for restart be written when the analysis is first run. If you do not request that restart data be written, restart files will not be created in ABAQUS/Standard, while in ABAQUS/Explicit a state file will be created with results at only the beginning and end of each step.
You can control the amount of data written to the restart files, as described below. The amount of data written to the restart file can be changed from step to step if you include the restart request in each step definition.
Restart information is not written during the following linear perturbation steps:
| Input File Usage: | Use the following option to request that restart data be written for an analysis: |
*RESTART, WRITE The *RESTART, WRITE option can be used as either model data or history data. |
| ABAQUS/CAE Usage: | Step module: Output |
| In ABAQUS/CAE restart requests are always associated with a particular step; you cannot define a restart request for the entire analysis. Restart requests are created by default for every step; restart requests for ABAQUS/Standard steps have a default frequency of 0, while restart requests for ABAQUS/Explicit steps have a default number of intervals of 1. |
You can specify the frequency at which data will be written to the ABAQUS/Standard restart file and the ABAQUS/Explicit state file. The variables to be written cannot be specified; a complete set of data is written each time. Therefore, the restart files can be quite large unless you control the frequency with which restart information is written.
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, 
, and at the end of each step of the analysis (regardless of the increment number at that time). In a direct cyclic 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 at which the iteration number is exactly divisible by and at the end of each step of the analysis.
| Input File Usage: | *RESTART, WRITE, FREQUENCY= |
| By default, =1. |
| ABAQUS/CAE Usage: | Step module: Output |
| By default, =0 (no restart information is written). |
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. 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. Results are always written at the end of the step, so it is not necessary to request results at the exact time intervals if results are required only at the end of a step.
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.
| Input File Usage: | Use the following option to request results at the increments ending immediately after each time interval: |
*RESTART, WRITE, NUMBER INTERVAL=n, TIME MARKS=NO Use the following option to request results at the exact time intervals: *RESTART, WRITE, NUMBER INTERVAL=n, TIME MARKS=YES By default, n=1. |
| ABAQUS/CAE Usage: | Step module: Output |
| By default, n=1. |
You can specify that only one increment (or one iteration in the case of a direct cyclic analysis) per step should be retained in the ABAQUS/Standard restart file or ABAQUS/Explicit state file, thus minimizing the size of the files. As the data are written, they overlay the data from the previous increment (or iteration), if any, written for the same step. You can specify whether or not the data should be overlaid for each step individually. Since in ABAQUS/Explicit the results are written by default only at the end of the step, it is recommended to overlay the data in conjunction with specifying a number of time intervals at which data are written; in this way the data in the restart file are advanced as dictated by the number of intervals used.
The advantage of overlaying the restart data is that it minimizes the space required to store the restart files. The disadvantage is that if an analysis terminates due to a system error, all data in the current step may be lost.
| Input File Usage: | Use the following option in ABAQUS/Standard: |
*RESTART, WRITE, OVERLAY Use the following option in ABAQUS/Explicit: *RESTART, WRITE, OVERLAY, NUMBER INTERVAL=n |
| ABAQUS/CAE Usage: | Step module: Output |
You restart (continue) an analysis by specifying that the restart or state, analysis database, and part files created by the original analysis be read into the new analysis. The restart files must be saved upon completion of the first job. In ABAQUS/Explicit the package (.pac) file and the selected results (.sel) file are also used for restarting an analysis and must be saved upon completion of the first job. Since restart files can be very large, sufficient disk space must be provided (in ABAQUS/Standard the analysis input file processor estimates the space that is required for the restart file).
You can specify the point at which the analysis is continued in the new run, as discussed below.
An analysis cannot be restarted from the linear perturbation steps listed in “Writing restart files.”
| Input File Usage: | Use the following option to restart an analysis: |
*RESTART, READ When the READ parameter is included, the *RESTART option must appear as model data. It is normally the first option in the input file after the *HEADING option. |
| ABAQUS/CAE Usage: | Job module: job editor: toggle on Restart as the Job Type |
In an ABAQUS/Standard restart analysis you must specify the name of the restart file that contains the specified step and increment (or iteration for a direct cyclic analysis). In an ABAQUS/Explicit restart analysis you must specify the name of the state file that contains the specified step and interval.
ABAQUS will issue an error message if the step and increment, iteration, or interval number at which restart is requested do not exist in the specified restart or state file.
| Input File Usage: | Enter the following input on the command line: |
abaqus job=job-name oldjob=oldjob-name |
| ABAQUS/CAE Usage: | Any module: Model |
You can specify the point (step and increment, iteration, or interval) in the previous analysis from which to restart. Truncating a step in the previous analysis when you restart is discussed below.
An ABAQUS/Standard analysis restarted from any analysis other than a direct cyclic 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.
| Input File Usage: | *RESTART, READ, STEP=step, INC=increment |
| ABAQUS/CAE Usage: | Any module: Model |
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 upon restart, you can increase the number of iterations or Fourier terms, thus allowing continuation of an analysis (see “Direct cyclic analysis,” Section 6.2.6).
| Input File Usage: | *RESTART, READ, STEP=step, ITERATION=iteration |
| ABAQUS/CAE Usage: | Direct cyclic analysis is not supported in ABAQUS/CAE. |
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.
| Input File Usage: | *RESTART, READ, STEP=step, INTERVAL=interval |
| ABAQUS/CAE Usage: | Any module: Model |
To continue an analysis without changes, only the steps subsequent to the step at which restart is being made should be defined in the restart analysis. All other information has been saved to the restart files.
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 may simply consist of the request to read restart data from another analysis.
| Input File Usage: | *RESTART, READ |
| ABAQUS/CAE Usage: | Any module: Model |
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).
| Input File Usage: | Enter the following input on the command line: |
abaqus job=job-name recover |
| ABAQUS/CAE Usage: | Job module: job editor: toggle on Recover (Explicit) as the Job Type |
You can truncate an analysis step prior to its completion when you restart the analysis. For example, by default, if the previous analysis is an ABAQUS/Standard procedure and you specify that the restart point is Step p, the restart analysis will restart from the last saved increment of Step p and continue the step to completion. However, if you specify that the restart point is increment n of Step p and that the step should be terminated before restart, the restart analysis will restart from increment n of Step p, end Step p at that point, and continue with newly defined steps. In this case the step from which the analysis is being restarted will be truncated at the time of restart, regardless of the step end time that had been given in the previous analysis. Thus, the step is considered to be completed even though all of the loading may not have been applied. Continuation of the analysis will be defined by history data provided in the restart run.
When you truncate an analysis step in an ABAQUS/Explicit restart analysis, you must specify the interval after which the analysis should be restarted.
If the step from which the restart is being made completed normally, you can truncate the step to restart within the step so that you can request additional output, write to the restart file with a higher frequency, etc. In ABAQUS/Explicit it may be necessary to truncate an analysis step when an unforeseen event occurs within a step; for example, if contact surface definitions require modification due to unforeseen displacements. If the step from which the restart is being made completed normally and the restart is being made from the last increment, iteration, or interval, truncating the analysis step will have no effect.
If the restart is being made from a job that was truncated by the operating system (for example, because of insufficient disk space, run-time limit exceeded, etc.), you will usually not choose to truncate the analysis step, so that the old step will first be completed before a new step—if any exists—is started. If restart is being made from the end of a step that terminated prematurely inside ABAQUS (for example, because it ran out of increments or it failed to converge), you must truncate the step and include a new step definition. If you do not truncate the step, ABAQUS will try to continue the old step upon restart and will terminate the analysis in the same manner as before.
| Input File Usage: | Use the following option in ABAQUS/Standard to restart from any analysis step other than a direct cyclic step: |
*RESTART, READ, STEP=p, INCREMENT=n, END STEP Use the following option in ABAQUS/Standard to restart from a direct cyclic analysis step: *RESTART, READ, STEP=p, ITERATION=n, END STEP Use the following option in ABAQUS/Explicit: *RESTART, READ, STEP=p, INTERVAL=n, END STEP |
| ABAQUS/CAE Usage: | Any module: Model |
Care should be taken if loads and boundary conditions refer to amplitude curves (“Amplitude curves,” Section 19.1.2). 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.
In ABAQUS/Standard care should be exercised when automatic stabilization is active at the point at which a step is truncated. This may happen either in the middle of quasi-static procedures using automatic stabilization (see “Solving nonlinear problems,” Section 8.2.1) or during contact analyses using automatic viscous damping (see “Common difficulties associated with contact modeling in ABAQUS/Standard,” Section 21.2.9). In such cases viscous forces may 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.
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
= the load to be applied in the first increment of the restart run,
= the remaining load to be applied in the restart run,
= the initial time increment for the restart run, and
= the total step time for the first step of the restart run.
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
*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
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 
= 
/6. The step time for the first step of the restarted job, , 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, , is set equal to 0.1.
It is possible to define steps subsequent to the step at which restart is being made. It is also possible to supply new amplitude definitions, new surfaces, new node sets, and new element sets during the restart analysis. Existing sets cannot be modified.
In ABAQUS/Standard additional surfaces defined in the model part of a restart analysis have the restriction that they can be referenced only from surface-based loading definitions (see “Loads,” Section 19.4) or output requests for user-defined surface sections (see “Output to the data and results files,” Section 4.1.2).
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:
The rules governing the continuation of optional analysis history data—loading, boundary conditions, output controls, and auxiliary controls (see “Defining a model in ABAQUS,” Section 1.3.1)—are the same for the steps defined in the restart analysis and the original analysis. For a discussion of the rules governing the continuation of optional history data, see “Procedures: overview,” Section 6.1.1.
It is possible to prescribe predefined fields (see “Predefined fields,” Section 19.6.1) in the restart analysis.
To specify predefined temperatures or field variables in an ABAQUS/Standard restart analysis, the corresponding predefined field must have been specified in the original analysis as initial temperatures or field variables (“Initial conditions,” Section 19.2.1) or as predefined temperatures or field variables (“Predefined fields,” Section 19.6.1).
User subroutines are not written to the ABAQUS/Standard restart file or to the ABAQUS/Explicit state file. Therefore, if the original analysis contained any user subroutines, these subroutines must be included again in the restart run. These subroutines can be modified on restart; however, modifications should be made with caution because they may invalidate the solution from which the restart is being made.
You can continue a previous analysis as a restart analysis and write the results from the restart analysis to a new restart file or state file. For example, if the previous analysis is an ABAQUS/Explicit procedure and in the current analysis you specify that the restart point is Step p and the restart output frequency is n, the analysis will be restarted from the last saved interval of Step p and restart states will be written in subsequent steps based on the new value of n.
To discontinue the writing of a restart file in ABAQUS/Standard when you are restarting a previous analysis, specify a restart output frequency of 0; if you do not specify a frequency, the file will continue to be written at the frequency defined for the previous analysis.
Restart files can be very large for large models or for jobs involving many restart increments (unless you choose to overlay the restart data—see “Overlaying results in the restart files”). Therefore, the previous restart file is not copied to the beginning of the new restart file when a job is restarted: only the data at restart increments requested in the current run are saved to the new restart file. However, if an eigenfrequency extraction step (“Natural frequency extraction,” Section 6.3.5) is restarted and additional eigenvalues are requested, the new restart file will contain those eigenvalues that converged during the first run as well as the additional eigenvalues.
Suppose an ABAQUS/Standard job stopped running because it ran out of disk space. The last complete information for an increment in the restart file is from Step 2, increment 4. The following two-line input file could be used to restart this job and continue writing the restart file:
Suppose you stopped an ABAQUS/Explicit job because too much output was being generated. The last information in the state file is from Step 2, Interval 4 at a time of .004. Step 2 has a time period of .010 and restart results were requested at 10 intervals. The following input file could be used to restart this job and redefine the remainder of the step with reduced output requests:
The ABAQUS output database file (job-name.odb) contains results that can be used for postprocessing in ABAQUS/CAE. By default, the output database file is not made continuous across restarts; a new output database file will be created each time a job is run. You can combine X–Y data extracted from multiple output database files in the Visualization module of ABAQUS/CAE. If necessary, you can also merge field and history results from two output database files using a Python script or a C++ program provided with the ABAQUS release. For more information, see “Adding results from one output database into another output database,” Section 8.10.7 of the ABAQUS Scripting User's Manual, or “Adding results from one output database into another output database,” Section 9.15.6 of the ABAQUS Scripting User's Manual.
The ABAQUS results file (job-name.fil) contains user-specified results that can be used for postprocessing in external postprocessing packages. In ABAQUS/Explicit results are written to the selected results file (job-name.sel), which is then converted to the results file for postprocessing. See “Output,” Section 4.1.1, for details. The results and selected results files can be made continuous across restarts if the old files are available.
ABAQUS/Standard will copy the information from the old result file into the result file for the new job up to the restart point and begin writing the new results to the new file following that point. ABAQUS/Explicit will copy the information from the old selected results file into the selected results file for the new job up to the restart point, and then begin writing the new results to the new file following that point.
If the old file is not provided, ABAQUS will continue the analysis, just writing the results of the restart analysis to the new results or selected results file. Therefore, you will have segments of the analysis results in different files, which should be avoided in most cases since postprocessing programs assume that the results are in a single continuous file. You can merge such segmented results files, if necessary, by using the abaqus append execution procedure (“Execution procedure for joining results (.fil) files,” Section 3.2.10) or by writing a postprocessing program (see “Joining data from multiple results files and converting file format: FJOIN,” Section 12.1.2 of the ABAQUS Example Problems Manual).
A restart analysis in ABAQUS/Standard can use the restart files generated from the same or any previous maintenance version of the same general release. For example, if the original analysis is executed with the Version 6.4-3 maintenance release, all subsequent Version 6.4 maintenance releases can be used to launch the restart analysis. Restart is not compatible between general releases; if the original analysis is executed with any Version 6.4 release, a Version 6.5 release cannot be used to launch the restart analysis.
In ABAQUS/Explicit the original analysis and the restart analysis must use precisely the same release. For example, if the original analysis is executed with the Version 6.4-3 maintenance release, only this exact release can be used to launch the restart analysis.
A restart analysis in ABAQUS and a recover analysis in ABAQUS/Explicit must be run on a computer that is binary compatible with the computer used to generate the restart files.
Restart Requests