August 10, 2020 at 2:11 pmrkoomulSubscriberHi,nI 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).nI 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.nfluent 3ddp -g -slurm -t$SLURM_NTASKS -mpi=openmpi -ssh -pinfiniband -cnf=$SLURM_NODELIST -i filename.jounWhat 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?nThank you.n
August 11, 2020 at 5:10 amKeyur KanadeAnsys EmployeeOn linux you start WB in batch as following:n/path/runwb2 -B -R journal.wbjn > lognnwhere the journal file is given using option -R, andninstruction to not open the GUI is given with option -Bnnpath is the path to the WB installation on your linux system, you may check with your IT where to find it.nJournaling a WB meshing script can be complex, so the best approach is to have all the mesh settingsnset already, e. g. on a Windows desktop. Then the only operations that need to be scripted are: read innthe project, generate the mesh, and save the project. Such a journal can be easily constructed by usingnscripting option in WB:nncreate a very simple geometry (e. g. a cube will do) and save the projectnFile - Scripting - record Journal Read the project, Update Mesh, Save ProjectnFile - Scripting - stop record JournalnnThis will create a skeleton of the script which you can easily modify, and then use it on linux. nnRegards,nKeyurnGuidelines for Posting on Ansys Learning ForumnHow to access ANSYS help linksnn
August 13, 2020 at 2:55 amrkoomulSubscriberThank you Keyur for the suggestions. nI 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. nI 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?nThank you,n n
August 13, 2020 at 5:58 amKeyur KanadeAnsys EmployeeSelect solution cell in wb. nthen in properties on the right hand, you can change the initialization method. nplease go through help for more information. nnRegards,nKeyurnGuidelines for Posting on Ansys Learning ForumnHow to access ANSYS help linksnn
August 13, 2020 at 5:42 pmrkoomulSubscriberThank you Keyur. It worked.n
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Local Sensitivity and Sensitivities: what difference?
- How many designs are generated while performing optimization using Optislang with NLPQL?
- DesignXplorer vs optiSLang for Workbench CFD Optimization
- Optislang workbench add-in
- Parameter relationships for Optimization
- ANSYS Optislang
- DOE all design points give the same results as the first calculation
- Errors about integrate executable into ANSYS Workbench using ACT
- Parametric study: Batch mode
- Design of Experiment points: Design Exploration
© 2023 Copyright ANSYS, Inc. All rights reserved.