Parametric study: Batch mode


I am trying to run a parametric study by varying the side-slip angle for an automobile and I am looking for information on how to run it in batch mode on a Linux cluster. I have created the project in Workbench 2020 R1.  Based on the side-slip angle (this is one of the parameters) and the extent of the outer domain (another parameter), the geometry and refinement regions are updated using DesignModeler, followed by mesh generation, and followed by the flow solution (Fluent).

I would like to run this in a batch mode on a Linux cluster. I have used batch mode for Fluent before using the following command, but not Workbench.

fluent 3ddp -g -slurm -t$SLURM_NTASKS -mpi=openmpi -ssh -pinfiniband -cnf=$SLURM_NODELIST -i filename.jou

What command and arguments do I need to use to run a parametric sweep using Workbench? Do you have any sample script and journal files to run a parametric sweep?

Thank you.



  • kkanadekkanade Forum Coordinator

    On linux you start WB in batch as following:

    /path/runwb2 -B -R journal.wbjn > log

    where the journal file is given using option -R, and

    instruction to not open the GUI is given with option -B

    path is the path to the WB installation on your linux system, you may check with your IT where to find it.

    Journaling a WB meshing script can be complex, so the best approach is to have all the mesh settings

    set already, e. g. on a Windows desktop. Then the only operations that need to be scripted are: read in

    the project, generate the mesh, and save the project. Such a journal can be easily constructed by using

    scripting option in WB:

    create a very simple geometry (e. g. a cube will do) and save the project

    File - Scripting - record Journal Read the project, Update Mesh, Save Project

    File - Scripting - stop record Journal

    This will create a skeleton of the script which you can easily modify, and then use it on linux. 



    Guidelines for Posting on Ansys Learning Forum

    How to access ANSYS help links

  • Thank you Keyur for the suggestions.

    I have set up everything for the geometry, mesh, and fluent apriori. As you suggested, I used the journal record option and created a journal file.

    I could use the journal file successfully in the batch mode, without opening the GUI for the first two design points. However, for the third design point the solution diverged at the first time step in Fluent. I saw the same behaviour when I ran it using GUI by selecting all design points and update them. However, it works fine without changing any settings in the GUI version if I set the third design point as "Current" in the parameter list, use manual update for the geometry and the mesh, and run fluent after initializing the flowfield. Does this has anything to do with the way initialization is done in the design points sweep? Is there anyway I can force Fluent to initialize the flow field using standard or hybrid initialization for each design point, without taking the solution from the previous design point for initialization?

    Thank you,

  • kkanadekkanade Forum Coordinator

    Select solution cell in wb.

    then in properties on the right hand, you can change the initialization method.

    please go through help for more information.



    Guidelines for Posting on Ansys Learning Forum

    How to access ANSYS help links

  • Thank you Keyur. It worked.

Sign In or Register to comment.