This article outlines the steps required to continue a partially solved Workbench based analysis using a Multi-Frame Restart and the MAPDL Batch mode.
In this article you will learn:
- Some ways to interface between ANSYS Workbench and ANSYS MAPDL
- How to re-launch a run using a Multi-Frame Restart in ANSYS Batch mode
- The value of the jobname.abt functionality for Static Structural and Transient Structural analyses
Recently I was working in the ANSYS Workbench interface within the Mechanical application running a Transient Structural analysis. I began my run thinking that my workstation had the necessary resources to complete the analysis in a reasonable amount of time. As the analysis slowly progressed, I began to realize that I needed to make a change and switch to a computer that had more resources. But some of my analysis was already complete and I did not want to lose that progress. In addition, I wanted to be sure that I could monitor the analysis intermediately to ensure that it was advancing as I would like. This meant that however I decided to proceed I needed to make sure that I could still read my results back into Mechanical along with having the capability to restart again from a later point. Here were my options.
1: I could use the Remote Solve Manager (RSM) to continue running my analysis on a compute server machine. Check out this article for more on that.
I did use RSM in part but perhaps you do not have RSM configured or your computer resources are not connected through a network. Then I will show the other option you can use.
2: A Multi-Frame Restart using MADPL in ANSYS Batch mode
Here’s the process:
1. Make note of the current load step and last converged substep that your analysis completed when you hit the Interrupt Solution button
2. Copy the *.rdb, *.ldhi, *.Rnnn files from the Solver Files Directory on the local machine to the Working Directory on the computing machine
You can find your Solver Files Directory by right clicking on the Solution Branch in the Model Tree and selecting Open Solver Files Directory:
3. Write an MAPDL input file with the commands to launch a restart and save it in the Working Directory on the computing machine (save with extension *.inp)
Below is an example of an input that will work well for restarting an analysis, but feel free to adjust it with the understanding that the ANSYS Programming Design Language (APDL) is a sophisticated language with a vast array of capability.
4. Start the MADPL Product Launcher interface on the computing machine and:
a: Set Simulation Environment to ANSYS Batch
b. Navigate to your Working Directory
c. Set the jobname to the same name as that of the *.rdb file
d. Browse to the input file you generated in Step 3
e. Give your output file a descriptive name
f. Adjust parallel processing and memory settings as desired
5. Look at the output file to see progress and monitor the run
6. Write “nonlinear” in a text file and save it as jobname.abt inside the Working Directory to cleanly interrupt the run and generate restart files when desired
The jobname.abt will appear briefly in the Working Directory
The output file will read the following:
Note that the jobname.abt interruption process is the exact process that ANSYS uses in the background when the Interrupt Solution button is pressed interactively in Mechanical
Read more about the jobname.abt functionality in the Help Documentation links at the end of this article.
7. Copy all newly created files in Working Directory on the computing machine to the Solver Files Directory on the local machine
8. Back in the Mechanical application, highlight the Solution branch of the model tree, select Tools menu>Read Results Files… and navigate to the Solver Files Directory and read the updated *.rst file
After you have read in the results file, notice that the restart file generated from the interruption through the jobname.abt process appears as an option within the Mechanical interface under Analysis Settings
9. Review intermediate results to determine if analysis should continue or if adjustments need to be made
10. Repeat entire process to continue analysis using the new current loadstep and substep
Here are some useful Help Documentation sections in ANSYS 15 for your reference:
- Understanding Solving:
- Mechanical APDL: Multiframe Restart:
And, as always, please contact PADT with your questions!