Post Processing in ANSYS Mechanical / Workbench

I just solved simulation problem in Ansys Mechanical. The problem is complex and takes a long to converge.

How do I post process the results and avoid solving the problem again and again. For eg. I need to change force and check deformation without solving entire simulation again. Any way around ? Using APDL commands ?

Thanks.

Comments

  • I had a model with bolt pretension applied in Step 1, which took a long time to converge, and was a common first step for all analyses. Then I wanted to apply many different forces in Step 2, which took very little time to solve. If you have that situation, then there is a simple method to save time.

    The important Analysis Setting is under Restart Controls, where you want to set things as shown in the image below.

    Put all the loads you ever want to analyze into the model. These loads will all be zero in step 1 and have a value in step 2. Then you Deactivate the loads for Step 2. You insert a command object in the Static Structural branch and it has the command /eof which stops the analysis. You edit the Details of that Command to only work in Step 2 as shown below.

    Now you solve that model. The result will be a solved model for step 1, but ready to restart. In Workbench, you duplicate the solved Static Structural model System A. In the copy (System B) you read in the results file from System A. Suppress the Command object, edit one Force and Activate the load for Step 2. Now Restart the solution. It will start at the end of load step 1 and quickly do load step 2. You can repeat this process for each force in the model, making copies of System A to make System B, System C, etc.

    I wrote those instructions many years ago. There may be a simpler way now. You can see if anyone else has a better workflow.

  • Thanks a lot peteroznewman for detailed and quick reply. I will try your method and let you know.

  • Hi @peteroznewman . I tried all the steps as you said. But it solves the whole model again. Can you check if the Analysis settings are correct ? In the Model, Spring Force remains constant, however I need to change the probing force .

    So, First System solves the spring force with probing force deactivated. While in the second system , probing force is activated and solved. The whole model solves again.



  • Did you read in the results file? Did you restart from the end of Step 1? There are many steps in the process.

    I recorded some videos, but there is no audio, so you might get some details that you skipped in your process.

    Good luck!

  • Hi @peteroznewman , It Works Thanks a Lot. Saved a lot of time :) Video was upto the point.

Sign In or Register to comment.