[Yann]

Hello all,

I'm running OpenFOAM-v2406 on WSL/Ubuntu.
I installed the precompiled openfoam2406-default package.

I need to use ccmToFoam, which requires to be compiled after building the libccmio library, but I fail to do so.

EDIT: I solved my issue, so I'm going to turn this post into a tutorial.

Here is the process:

1. Start a WSL session. In order to have write permission in the default OpenFOAM installation directory, you will need to start a shell with root privilege: sudo -s
2. Load the OpenFOAM environment: source /usr/lib/openfoam/openfoam2406/etc/bashrc
3. Move to the OpenFOAM install directory: foam
4. Download the ThirdParty-v2406.tgz archive: wget https://dl.openfoam.com/source/v2406...arty-v2406.tgz
5. Unpack the archive: tar -xzf ThirdParty-v2406.tgz
6. Rename the extracted directory: rm ThirdParty && mv ThirdParty-v2406 ThirdParty
7. Move to ThirdParty/sources directory and download the libccmio-2.6.1.tar.gz archive: cd ThirdParty/sources/ && wget https://sourceforge.net/projects/foa...o-2.6.1.tar.gz
8. Unpack the archive: tar -xzf libccmio-2.6.1.tar.gz
9. Get back to the ThirdParty directory and reload the OpenFOAM environment: cd .. && source /usr/lib/openfoam/openfoam2406/etc/bashrc
10. Compile the libccmio library: ./makeCCMIO
11. Move to: cd $FOAM_SRC/conversion/ccm
12. Build the libccm library: ./Allwmake
13. Move to: cd $FOAM_UTILITIES/mesh/conversion/ccm/
14. Build the ccm utilities: ./Allwmake
15. All done, exit the root shell and reload the OpenFOAM environment: exit && source /usr/lib/openfoam/openfoam2406/etc/bashrc

Here you go, you should now be able to use ccmToFoam and foamToCcm

If anyone more competent than me knows a better way to do this, let me know!
Yann

[hernanrmz]

Hello Yann,

Great tutorial, it works for me!

I haven´t use this application (ccmToFoam), I have use the ccm26ToFoam application from the Foundation version sometimes

Do you use ccmToFoam regularly? What kind of meshes had you use?

This case attached was composed for two regions so I use the "-merge" option and works fine.

OpenFOAM-Mesh.jpg

StarCCM-Mesh.jpg

Best regards

Hernán Ramírez

[Yann]

Hello Hernán,

Thank you, I'm glad this has been useful for you!

I needed ccmToFoam for a specific case so I did not have many opportunities to use it, but I've been able to convert hex and poly meshes. It also worked to convert a multi region mesh for a CHT case, with some extra step required after conversion to deal with region interfaces.

I don't know the exact differences, but according to these release notes, ccm26ToFoam has been deprecated and replaced by ccmToFoam since OpenFOAM-v1612+ in the OpenCFD branch.

Cheers,
Yann

[hernanrmz]

Hello Yann,

Thank you for your answer. In the company I work, we use Star-CCM+ (I've been using it for the last 7 years), but I want to implement OpenFOAM as an option to solve some cases.

My next step (in a few weeks) is to convert a mesh of a CHT case. Could you explain what extra steps are requiered after conversion?

Cheers,

Hernán

[Yann]

Hello Hernán,

For CHT cases in OpenFOAM, we usually use splitMeshRegions to split the mesh and create the coupled interfaces between regions.

You can use ccmToFoam to convert a CHT mesh using the -solids option, but you end up with disconnected regions.
I used stitchMesh to reconnect the regions together, and then used splitMeshRegions to split the mesh and create the interfaces.

It's probably possible to use splitMeshRegions first and then deal with the interfaces using something like createPatch, but I'm lazy and I'd rather let splitMeshRegions do the job for me

I couldn't find a way to avoid disconnected regions after running ccmToFoam (-merge does not seem to change anything in this case).
Let me know if you find another way to achieve it without having to stitch the mesh!

Cheers,
Yann

[juancfd]

Originally Posted by Yann

Hello all,

I'm running OpenFOAM-v2406 on WSL/Ubuntu.
I installed the precompiled openfoam2406-default package.

I need to use ccmToFoam, which requires to be compiled after building the libccmio library, but I fail to do so.

EDIT: I solved my issue, so I'm going to turn this post into a tutorial.

Here is the process:

1. Start a WSL session. In order to have write permission in the default OpenFOAM installation directory, you will need to start a shell with root privilege: sudo -s
2. Load the OpenFOAM environment: source /usr/lib/openfoam/openfoam2406/etc/bashrc
3. Move to the OpenFOAM install directory: foam
4. Download the ThirdParty-v2406.tgz archive: wget https://dl.openfoam.com/source/v2406...arty-v2406.tgz
5. Unpack the archive: tar -xzf ThirdParty-v2406.tgz
6. Rename the extracted directory: rm ThirdParty && mv ThirdParty-v2406 ThirdParty
7. Move to ThirdParty/sources directory and download the libccmio-2.6.1.tar.gz archive: cd ThirdParty/sources/ && wget https://sourceforge.net/projects/foa...o-2.6.1.tar.gz
8. Unpack the archive: tar -xzf libccmio-2.6.1.tar.gz
9. Get back to the ThirdParty directory and reload the OpenFOAM environment: cd .. && source /usr/lib/openfoam/openfoam2406/etc/bashrc
10. Compile the libccmio library: ./makeCCMIO
11. Move to: cd $FOAM_SRC/conversion/ccm
12. Build the libccm library: ./Allwmake
13. Move to: cd $FOAM_UTILITIES/mesh/conversion/ccm/
14. Build the ccm utilities: ./Allwmake
15. All done, exit the root shell and reload the OpenFOAM environment: exit && source /usr/lib/openfoam/openfoam2406/etc/bashrc

Here you go, you should now be able to use ccmToFoam and foamToCcm

If anyone more competent than me knows a better way to do this, let me know!
Yann

Hi Yann,

I am experiencing some issues in the 10th step. When I was trying to run the makeCCMIO script I have found the following error:




openfoam@Ubuntu:/usr/lib/openfoam/openfoam2406/ThirdParty$ ./makeCCMIO
Appear to have {wmkdepend,wmkdep} binary
Found sources: sources/libccmio-2.6.1
Starting build: libccmio-2.6.1 (lib)

cpMakeFiles libccmio .
Compiling enabled on 12 cores
wmake lib
wmake: 'Make' directory does not exist in /usr/lib/openfoam/openfoam2406/ThirdParty/sources/libccmio-2.6.1
Searching up directories tree for Make directory
Error: no Make directory for /usr/lib/openfoam/openfoam2406/ThirdParty/sources/libccmio-2.6.1

Error building: libccmio-2.6.1




To give some context, I am running the steps in Ubuntu 22.04 version inside an Oracle Virtual Box Machine. Moreover, I run some of the previous steps with the command "sudo" because without it the installations and decompressions failed saying "permission denied".

Thank you in advance!

[Yann]

Hello Juan,

I am not exactly sure, but I think your error might be related to a permission issue.

You indeed need to have root privilege to be able to write files in the OpenFOAM installation directory.
This is what step 1 is about. If you did step 1 and run all other commands in the same shell session you should not have permission issues.
However if you skipped step 1 or ran commands from another shell session you should probably run pretty much all commands with sudo.

So you can try running sudo ./makeCCMIO, or go over all the procedure again paying attention to have the right permissions (just in case other steps failed due to permission issues)

Let me know how it goes!

[juancfd]

Originally Posted by Yann

Hello Juan,

I am not exactly sure, but I think your error might be related to a permission issue.

You indeed need to have root privilege to be able to write files in the OpenFOAM installation directory.
This is what step 1 is about. If you did step 1 and run all other commands in the same shell session you should not have permission issues.
However if you skipped step 1 or ran commands from another shell session you should probably run pretty much all commands with sudo.

So you can try running sudo ./makeCCMIO, or go over all the procedure again paying attention to have the right permissions (just in case other steps failed due to permission issues)

Let me know how it goes!

Hello again Yann,

It's working now! As you said, I was trying to execute the commands from another shell. I've opened a new terminal and executed all steps again, finally it's working.

I've also tried to use the ccmToFoam package and it modifies the mesh from .ccm format into polyMesh without issues.

Thank you for your time and support!