January 25, 2023 at 7:28 amFAQParticipant
Answer: The steps below assume that ANSYS CFX 19.2 is installed on a supported operating system and no firewalls are blocking communication across multiple computers is that is in use, CFX and HPC licenses are available. This Solution could be reused for other recent versions going back to 18.2 with changes to the v### in the path This also assumes you have working knowledge of Command Prompt on Windows OR terminal on Linux. If you are not comfortable with command lines, please request assistance from your Organization’s IT administrator. Installation and Paths On Windows Default Installation path is C:Program FilesANSYS Inc and CFX solver is in C:Program FilesANSYS Incv192CFXbin You can try including this to the PATH or use the full path to cfx5solve On Linux if /ansys_inc softlink was created to the installation location then below is the path to cfx5solve /ansys_inc/v192/CFX/bin/ Test model and working directory Create a Working Directory preferable a path without spaces or special characters on Windows say C:tempcfxtesttest1 on Linux try /home/cfxtest Copy the example file below to the working directory in above Windows C: cd tempcfxtesttest1 copy “C:Program FilesANSYS Incv192CFXexamplesStaticMixer.def” . Linux cd /home cp /ansys_inc/v192/CFX/examples/StaticMixer.def ./ Here are the steps to run CFX solver in different modes Serial Mode, uses 1 core On Windows “C:Program FilesANSYS Incv192CFXbincfx5solve.exe” -batch -serial -def StaticMixer.def On Linux /ansys_inc/v192/CFX/bin/cfx5solve -batch -serial -def StaticMixer.def Local machine only (Shared Memory Parallel) on one node change the command line flags to -batch -par -def StaticMixer.def -par-local -part 10 Local machine only (Distributed Memory Parallel) on one node change the command line flags to -batch -par -def StaticMixer1.def -par-dist “node01*2” NOTE: if you are on a headnode or loginhnode say hostname node00, then do not run the above from node00. ssh to node01 and run from there. The first node in the list should be the node you are running the command line from. To run across nodes on Linux On Linux passwordless ssh needs to be enabled. -batch -par -def StaticMixer1.def -par-dist “node01*2,node02*2” To force a particular start method from command line, this example shows Intel MPI distributed Parallel -batch -par -def StaticMixer1.def -par-dist “node01*2” -start-method “Intel MPI Distributed Parallel” For Debugging purposes add flag “-v” at the beginning without quotes To stop an existing solve say the first run, you can use the command. Be sure to run the command in the folder which contains the directory being referenced. Windows “C:Program FilesANSYS Incv19.xCFXbincfx5stop.exe” -directory StaticMixer_001.dir Linux /ansys_inc/v19.x/CFX/bin/cfx5stop -directory StaticMixer_001.dir To run Distributed Parallel Across multiple Windows machines from the CFX GUI using IBM or Intel MPI see ANSYS Customer portal Knowledge Materials listed below Solution: 2053013 Configuring and Launching ANSYS CFX 19.x – Distributed using IBM MPI or Intel MPI https://support.ansys.com/AnsysCustomerPortal/en_us/Knowledge+Resources/Solutions/CFX%20-%20SYS/2053013 Solution: 2050944 Configuring and Launching ANSYS CFX 18.x – Distributed using IBM MPI or Intel MPI https://support.ansys.com/AnsysCustomerPortal/en_us/Knowledge+Resources/Solutions/CFX%20-%20SYS/2050944 For detailed information please refer “Chapter 13: Starting the CFX-Solver from the Command Line” https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v192/cfx_solv/i1304872.html If you are running CFX on a Windows HPC cluster then the following is the command line to use: “\headnodeANSYS Incv191CFXbincfx5solve.exe” -chdir “\headnodeshared_directory” -def “\headnodeshared_directoryStaticMixer.def” -part 20 -start-method “Submit to Windows HPC Queue” If you have a node group defined you will need to add this line to the start up script: -node-group=”Node_Group_Name” Also, see Solution # 2053008 for configuring CFX on a Windows cluster. https://support.ansys.com/AnsysCustomerPortal/en_us/Knowledge+Resources/Solutions/CFX%20-%20SYS/2053008.
Introducing Ansys Electronics Desktop on Ansys Cloud
The Watch & Learn video article provides an overview of cloud computing from Electronics Desktop and details the product licenses and subscriptions to ANSYS Cloud Service that are...
How to Create a Reflector for a Center High-Mounted Stop Lamp (CHMSL)
This video article demonstrates how to create a reflector for a center high-mounted stop lamp. Optical Part design in Ansys SPEOS enables the design and validation of multiple...
Introducing the GEKO Turbulence Model in Ansys Fluent
The GEKO (GEneralized K-Omega) turbulence model offers a flexible, robust, general-purpose approach to RANS turbulence modeling. Introducing 2 videos: Part 1 provides background information on the model and a...
Postprocessing on Ansys EnSight
This video demonstrates exporting data from Fluent in EnSight Case Gold format, and it reviews the basic postprocessing capabilities of EnSight.
- Ansys Licensing: Managing Activations
- Installing ANSYS 2020 Releases on Windows
- Installing ANSYS License Manager on Windows
- Ansys Licensing: Activating Entitlements
- Troubleshooting with ANSYS License Management Center
- ANSYS Licensing Portal Overview
- Importing Zuken into ANSYS
- 2019R1 Workbench Fluent design point update (foreground in Solution and foreground in Parameter Set) stuck at end of 1st DP and doesn’t proceed to next DP. Fluent processes could not be terminated after iterations and cas/dat files are written in 1st DP.
- License Reporting in ANSYS License Management Center
- ANSYS License Manager: Configuring Firewall Exceptions on Windows