In an earlier comprehensive blog post, Ankur Kumar outlined the step-by-step procedure for restarting an Abaqus job using the GUI. You can reach that page here.
Restarting an analysis in Abaqus can be a powerful way to save time and resources, especially for long-running simulations or when you need to modify certain aspects of your model.
Most of the CAE Engineers out there use different pre-processing tools and use Abaqus as a solver. Hence, they may really need a way to restart the jobs using a command line.
Step 1: Obtain the required files for restart.
To get necessary files for restart, we need to request for these files when we submit the initial job. To request the restart files, we need to include *RESTART, WRITE, FREQUENCY=1 in the initial input file, <job name>.inp. When we submit the job in next step, this input file will write the results of every increment (FREQ = 1) to the restart file.
Note: Setting the frequency = 1 will update restart files at every increment. This will cause large size of .stt file. It is advisable to specify Frequency=n, where “n” is an integer chosen by the user. If omitted, the last increment of the final step will be written out.
Step 2: Run the job from the command line.
To run a job, launch a CMD (command prompt) from the directory of inp file. Once in the CMD window, execute abaqus j=<job name>
Step 3: Creating a <new_job>.inp for restart.
Also, you can add additional parameters for CPUs, GPUs, and interactive run. In this example, the 2nd step is not completed. Let’s assume that in the restarted run the analysis is to be continued from the end 10th increment of the second step.
To begin the simulation from second step, 10th increment, we need to create a new inp file.
The keywords needed for the restart file are as below.
Including an END STEP command within *Restart, terminates the step in which restart is called and asks Abaqus to proceed to the next step. That means in a 3-step analysis, if restart is called in step 2 with an END STEP, then Abaqus will jump to step 3 right after step 1.
Note: Since this is a restart run, all the model data part of the input (F.E. Mesh data, material properties, etc.) is omitted. The next statement after the *RESTART statement consists of a *STEP statement.
Save Input file for the restarted run <new_job >.inp
Step 4: Run the <new_job>.inp for restart.
The job is submitted from the command line as follows:
abaqus oldjob=<job name> j=<new_job>
The following extract taken from <new_job>.dat shows that the results are read from the restart file up to the 10th increment and the analysis continuing with the next step (STEP 3).
The analysis continuing with the next step (STEP 3). Following is the extract from the status file: <new_job>.sta
Step 5: Combine the ODB files.
If the ODB files from the first run and the restarted run needs to be combined into a single ODB file for post-processing purposes, this is achieved by typing the following line from the command line. Execution procedure for joining output database (.odb) files from restarted analyses.
abaqus restartjoin originalodb=odb-file-name restartodb=odb-file-name [copyoriginal].
In summary, stopping and restarting an analysis job in Abaqus is a valuable technique for managing long-running simulations and making necessary adjustments without starting from scratch. By properly setting up restart files during the initial analysis, carefully modifying the model as needed, and correctly configuring the restart job, users can efficiently continue their simulations from a specific point. This approach not only saves time but also enhances the flexibility and robustness of the analysis process. With these steps, users can effectively handle complex simulations and achieve accurate results in Abaqus.
Leave a Reply