CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   star-ccm mesh to O\/F (http://www.cfd-online.com/Forums/openfoam/73356-star-ccm-mesh-o-f.html)

DLC March 5, 2010 07:01

star-ccm mesh to O\/F
 
Hi Foamers,

I'm trying to convert a mesh made with star-ccm, in order to use OpenFOAM, using starToFoam, but continues to error... my mesh is called test.ccm and the converter keeps asking a .vrt file....

I've converted several meshes form .msh without any problems, but this time I can't do it...

can anyone help me?

thanks!

linnemann March 5, 2010 08:05

Hi

I think you need to use the star4ToFoam command to convert the ccm file.

starToFoam is based on StarCD cases which where different from ccm+.

DLC March 5, 2010 08:52

Hi,

I already tried... same result...

any other ideas?

wyldckat March 5, 2010 10:03

Greetings DLC,

Although I'm still to get a successful conversion from ccm+ to foam (hadn't had the time to do it yet), you're trying to use the wrong utility! For ccm you need ccm26ToFoam. You'll have to build ccm26ToFoam:
Code:

$FOAM_APP/utilities/mesh/conversion/Optional/Allwmake
And you'll need to visit and read this thread (well, just the 1st post or the 21st post on it) before trying to build ccm26ToFoam ;)

Best regards,
Bruno

DLC March 7, 2010 10:30

Thank you for your illuminating post, I'll try next days to convert this mesh... I'll let know if I'll make it!

Thanks again!

lbordier March 8, 2010 07:24

if you use OF1.6 then you need to compile 1.6.x version of ccm26ToFoam available from git repository. Otherwise compilation will fail.

wyldckat March 8, 2010 12:27

Quote:

Originally Posted by lbordier (Post 248964)
if you use OF1.6 then you need to compile 1.6.x version of ccm26ToFoam available from git repository. Otherwise compilation will fail.

Good catch! I had it in mind, but completely forgot to mention about it :(

And yes, copying the source folder ccm26ToFoam from the 1.6.x to the 1.6 version, and then building with the OpenFOAM 1.6 version will do the trick! Thus not needing to build a full OpenFOAM 1.6.x version :)

fiona March 10, 2010 02:09

Quote:

Originally Posted by wyldckat (Post 248999)
Good catch! I had it in mind, but completely forgot to mention about it :(

And yes, copying the source folder ccm26ToFoam from the 1.6.x to the 1.6 version, and then building with the OpenFOAM 1.6 version will do the trick! Thus not needing to build a full OpenFOAM 1.6.x version :)

Hi Luc and Bruno,

Following your instructions, I was able to make ccm26ToFoam and test the sample ccm files in OpenFOAM/ThirdParty-1.6/libccmio-2.6.1/data. Do you know where I can find tutorials/explanation of these sample cases? How can I load and visualize the generated mesh?

thanks,

Fiona

wyldckat March 10, 2010 06:31

Greetings Fiona,

Sweet, I didn't even know there was a case sample with the ccmio library! Sadly, I don't know of any tutorials for ccm to foam :(

As for loading and visualizing the generated mesh (the foam version), you just use paraFoam as you normally would with any other OpenFOAM simulation case! Additionally, some days ago I found what starts in this post, has a solution a few posts later on how to visually debug the mesh in Paraview, because cutting the mesh will triangulate the mesh where it is cut.

Oh, if paraFoam is unwilling to work, use foamToVTK to export the mesh to VTK and then use Paraview to open the exported .vtk files directly!

So at least one question is still unanswered: does anyone know of any tutorials for ccm to foam?

Best regards,
Bruno

fiona March 10, 2010 12:58

Hi Bruno,

Thank you! ParaFoam works.

From what I've got, it seems that ccm26ToFoam can capture the interface boundary patches. Does this mean the MRF or sliding mesh created in Star-CCM+ can be preserved and imported into OpenFoam? The User Manual says utilities such as fluentMeshToFoam and starToFoam can't.

Fiona

wyldckat March 10, 2010 13:10

Quote:

Originally Posted by fiona (Post 249399)
Thank you! ParaFoam works.

You're welcome :)

Quote:

Originally Posted by fiona (Post 249399)
Does this mean the MRF or sliding mesh created in Star-CCM+ can be preserved and imported into OpenFoam?

I honestly have got no clue. My best guess is that the mesh itself is converted, but the additional definitions will have to be done by hand. I suggest looking at the OpenFOAM tutorial cases that have MRF and sliding meshes and see what might be missing in the conversion process.

By what I estimate, ccm26ToFoam won't be seeing updates/upgrades in the near future, but I might be wrong :rolleyes:

Best regards,
Bruno

olesen March 11, 2010 02:27

Quote:

Originally Posted by fiona (Post 249399)
Hi Bruno,

Thank you! ParaFoam works.

From what I've got, it seems that ccm26ToFoam can capture the interface boundary patches. Does this mean the MRF or sliding mesh created in Star-CCM+ can be preserved and imported into OpenFoam? The User Manual says utilities such as fluentMeshToFoam and starToFoam can't.

How are the Star-CCM+ MRF and sliding mesh case actually saved?
The ccm->Foam conversion only handles stuff that is in the ccm geometry file.
AFAIK ccm->Foam either takes the first one or States/default.
Which other states are there states in the ccm geometry file?

navnair87 April 1, 2010 16:25

Hi Fiona and Bruno, I have just install OF1.6.x and I have done what Bruno posted in post #4 but I still can't get ccm26ToFoam to work. Can you please help me as I am really desperate to get this to work.

Thank you in advance.

Kind Regards,
Navein

wyldckat April 1, 2010 17:40

Greetings Navein,

Give me a step by step of what you've done so far. My guess is that you didn't follow the link to the other thread!

Best regards,
Bruno

navnair87 April 1, 2010 17:56

Hi Bruno,

Thank you for the quick reply.

I installed ubuntu 9.10 and installed OpenFOAM 1.6.x, following the instructions created by Mads Reck and revised by yourself. After that, I typed in the command that you posted in post #4 and you are right, I did not follow the link to the other thread. To be perfectly honest, I'm brand new to Linux and I don't really understand what you meant in the other thread. Would you mind giving me a step by step guide on how I have to go about doing this?

wyldckat April 1, 2010 18:08

OK, lets do this step by step then :)
  1. Got to the --> #21 <-- ;) post on the dedicated thread to libccmio
  2. Download the attached file and move it to the folder ~/OpenFOAM
  3. Now run:
    Code:

    cd ~/OpenFOAM/ThirdParty-1.6.x
    tar -xzf ../awlibccmio.tar.gz
    chmod +x AllwmakeLibccmio
    ./AllwmakeLibccmio

    These will unpack the files, make the script executable and build the ccm library for OpenFOAM to use.
  4. Finally run:
    Code:

    $FOAM_APP/utilities/mesh/conversion/Optional/Allwmake
And voilá, your brand new ccm26ToFoam is ready to go :) Ironically, I no experience using it :(

navnair87 April 1, 2010 18:16

Thanks Bruno, I really appreciate your help.
Stupid question here: Do I just move the file in the OpenFOAM folder and not in the OpenFoam-1.6.x folder?
I am currently in the midst of reinstalling OpenFOAM as I messed with the files too much over the past couple of days trying to figure this out. Once that is done, I'll be giving this a go and hopefully I'll do the right thing this time around.

wyldckat April 1, 2010 18:31

Uhm... OK, look at the two first code lines on step 3:
  • The first line makes the bash go to the ThirdParty folder:
    Code:

    cd ~/OpenFOAM/ThirdParty-1.6.x
  • The second line unpacks the file that is in the parent folder, namely "~/OpenFOAM":
    Code:

    tar -xzf ../awlibccmio.tar.gz
This way, all of the downloaded OpenFOAM packages will be in the base folder of OpenFOAM :cool:

Well you got lucky that I visited the forum so soon ;) I'm glad I could help :)

Best regards,
Bruno

navnair87 April 1, 2010 18:49

Thanks Bruno :)

Kind Regards,
Navein

navnair87 April 1, 2010 21:07

Hi Bruno,

I've managed to get it working! Thanks again for your assistance. Have a good Easter weekend!

Kind Regards,
Navein


All times are GMT -4. The time now is 08:12.