CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

star-ccm mesh to O\/F

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree7Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   March 5, 2010, 08:01
Default star-ccm mesh to O\/F
  #1
DLC
Member
 
Davide Lupo Conti
Join Date: Nov 2009
Posts: 34
Rep Power: 7
DLC is on a distinguished road
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!
DLC is offline   Reply With Quote

Old   March 5, 2010, 09:05
Default
  #2
Senior Member
 
linnemann's Avatar
 
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 450
Rep Power: 15
linnemann will become famous soon enough
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+.
__________________
Linnemann

PS. I do not do personal support, so please post in the forums.
linnemann is offline   Reply With Quote

Old   March 5, 2010, 09:52
Default
  #3
DLC
Member
 
Davide Lupo Conti
Join Date: Nov 2009
Posts: 34
Rep Power: 7
DLC is on a distinguished road
Hi,

I already tried... same result...

any other ideas?
DLC is offline   Reply With Quote

Old   March 5, 2010, 11:03
Default
  #4
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,301
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
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
wyldckat is offline   Reply With Quote

Old   March 7, 2010, 11:30
Default
  #5
DLC
Member
 
Davide Lupo Conti
Join Date: Nov 2009
Posts: 34
Rep Power: 7
DLC is on a distinguished road
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!
DLC is offline   Reply With Quote

Old   March 8, 2010, 08:24
Default
  #6
New Member
 
Luc Bordier
Join Date: Feb 2010
Posts: 10
Rep Power: 7
lbordier is on a distinguished road
if you use OF1.6 then you need to compile 1.6.x version of ccm26ToFoam available from git repository. Otherwise compilation will fail.
lbordier is offline   Reply With Quote

Old   March 8, 2010, 13:27
Default
  #7
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,301
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Quote:
Originally Posted by lbordier View Post
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
wyldckat is offline   Reply With Quote

Old   March 10, 2010, 03:09
Default
  #8
New Member
 
Join Date: Mar 2010
Posts: 14
Rep Power: 7
fiona is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
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
fiona is offline   Reply With Quote

Old   March 10, 2010, 07:31
Default
  #9
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,301
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
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
wyldckat is offline   Reply With Quote

Old   March 10, 2010, 13:58
Default
  #10
New Member
 
Join Date: Mar 2010
Posts: 14
Rep Power: 7
fiona is on a distinguished road
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
fiona is offline   Reply With Quote

Old   March 10, 2010, 14:10
Default
  #11
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,301
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Quote:
Originally Posted by fiona View Post
Thank you! ParaFoam works.
You're welcome

Quote:
Originally Posted by fiona View Post
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

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   March 11, 2010, 03:27
Default
  #12
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 777
Rep Power: 18
olesen will become famous soon enough
Quote:
Originally Posted by fiona View Post
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?
olesen is offline   Reply With Quote

Old   April 1, 2010, 16:25
Default
  #13
New Member
 
Navein
Join Date: Dec 2009
Posts: 5
Rep Power: 7
navnair87 is on a distinguished road
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
navnair87 is offline   Reply With Quote

Old   April 1, 2010, 17:40
Default
  #14
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,301
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
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
wyldckat is offline   Reply With Quote

Old   April 1, 2010, 17:56
Default
  #15
New Member
 
Navein
Join Date: Dec 2009
Posts: 5
Rep Power: 7
navnair87 is on a distinguished road
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?
navnair87 is offline   Reply With Quote

Old   April 1, 2010, 18:08
Default
  #16
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,301
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
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

Last edited by wyldckat; April 1, 2010 at 18:23. Reason: code typo fixed...
wyldckat is offline   Reply With Quote

Old   April 1, 2010, 18:16
Default
  #17
New Member
 
Navein
Join Date: Dec 2009
Posts: 5
Rep Power: 7
navnair87 is on a distinguished road
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.
navnair87 is offline   Reply With Quote

Old   April 1, 2010, 18:31
Default
  #18
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,301
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
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

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

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   April 1, 2010, 18:49
Default
  #19
New Member
 
Navein
Join Date: Dec 2009
Posts: 5
Rep Power: 7
navnair87 is on a distinguished road
Thanks Bruno

Kind Regards,
Navein
navnair87 is offline   Reply With Quote

Old   April 1, 2010, 21:07
Default
  #20
New Member
 
Navein
Join Date: Dec 2009
Posts: 5
Rep Power: 7
navnair87 is on a distinguished road
Hi Bruno,

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

Kind Regards,
Navein
navnair87 is offline   Reply With Quote

Reply

Tags
.msh, .vrt, mesh conversion, star-ccm

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Mesh Transfer from ICEM to STAR CCM+ Waseem Siddique CD-adapco 4 February 12, 2009 07:02
Problem wih MESh in Star Design Waseem Siddique CD-adapco 3 January 28, 2009 08:19
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
basic of mesh refinement arya CFX 4 June 19, 2007 12:21
unstructured vs. structured grids Frank Muldoon Main CFD Forum 1 January 5, 1999 11:09


All times are GMT -4. The time now is 16:27.