CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > SU2

How to use ICEM-CFD to generate CGNS mesh that could be recognized by SU2

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

Like Tree2Likes
  • 1 Post By EMolina
  • 1 Post By denzell

Reply
 
LinkBack Thread Tools Display Modes
Old   January 18, 2014, 17:43
Default How to use ICEM-CFD to generate CGNS mesh that could be recognized by SU2
  #1
Member
 
Tommy Chen
Join Date: Mar 2011
Location: University of Michigan
Posts: 91
Rep Power: 6
Tommy Chen is on a distinguished road
I wanna use icem-cfd to generate CGNS format mesh file for SU2

However there are two problems

1. How to name the markers using icem, it seems that the makers' names given by the icem-cfd could not be recognized by su2

2. Could SU2 Version 3.0 handle more than one zone with CGNS ? SU2 v2 could only handle one single zone when using CGNS fromat mesh file.


Thank you guys
Tommy Chen is offline   Reply With Quote

Old   January 19, 2014, 16:11
Default
  #2
New Member
 
Eduardo Molina
Join Date: Sep 2010
Location: Brazil
Posts: 27
Rep Power: 6
EMolina is on a distinguished road
Hi Tommy,

1. I use Icem to generate my grids for SU2. You have to export the CGNS using version 2.4 in ICEM14.0, this settings work for me including the markers names.

2. I am also interesting in that question, SU2 is not able to handle multiple zones using CGNS. I know that there is a Matlab code in folder meshtools that appears to concatenate grids. Unfortunately I do not have Matlab so I am not able to test it (Octave fails due to some different commands from Matlab). Any help is appreciated.

Regards

Eduardo.
vetri likes this.
EMolina is offline   Reply With Quote

Old   January 21, 2014, 13:05
Default CGNS mesh conversion problem with ICEM for SU2 simulations
  #3
New Member
 
vetriselvan
Join Date: Jan 2010
Posts: 14
Rep Power: 7
vetri is on a distinguished road
Hi EMolina,
As per your suggestion I am exporting my mesh from ICEM 14.5 to CGNS 2.4 version. But even then, I am unable to convert it into SU2 mesh using SU2_v3.0. I am having a hybrid mesh with prism, tetra, quad and tri elemets. When I convert prism elements into tetra I am able to convert it into SU2 format. Could you suggest any solutions without this conversion? Do you also have the same element types as I have for your grid? or am I missing some options while exporting it to CGNS 2.4 version?

I am getting the following error in SU2

Reading grid coordinates...
Number of coordinate dimensions is 3.
Reading CoordinateX values from file.
Reading CoordinateY values from file.
Reading CoordinateZ values from file.
Reading connectivity information...
Number of connectivity sections is 4.


!!! Error !!!
Unrecognized element type.
Now exiting...


Thanks in advance.
Vetri

Quote:
Originally Posted by EMolina View Post
Hi Tommy,

1. I use Icem to generate my grids for SU2. You have to export the CGNS using version 2.4 in ICEM14.0, this settings work for me including the markers names.

2. I am also interesting in that question, SU2 is not able to handle multiple zones using CGNS. I know that there is a Matlab code in folder meshtools that appears to concatenate grids. Unfortunately I do not have Matlab so I am not able to test it (Octave fails due to some different commands from Matlab). Any help is appreciated.

Regards

Eduardo.
vetri is offline   Reply With Quote

Old   January 25, 2014, 16:10
Default
  #4
New Member
 
Eduardo Molina
Join Date: Sep 2010
Location: Brazil
Posts: 27
Rep Power: 6
EMolina is on a distinguished road
Hi Vetri

Do you have any pyramids in your grid. Sometimes ICEM create pyramids to connect the prism that is growing with tetra specially in complex geometries. I don't know if SU2 can handle pyramids probably does. In my grids I prefer use HEXA and Quads for viscous meshes and TRI+TETRA for inviscid meshes in icem. Maybe the guys from Stanford can help.

Another thing you can try export on ICEM using others CGNS versions. You compile SU2 with what CGNS version?

Please see this topic: CGNS output problem

They report the CGNS error on ICEM.

Good luck

Regards

Eduardo.
EMolina is offline   Reply With Quote

Old   January 27, 2014, 11:41
Default
  #5
New Member
 
vetriselvan
Join Date: Jan 2010
Posts: 14
Rep Power: 7
vetri is on a distinguished road
Hi Emolina,

Thanks for your reply.

As of now I do not have any pyramids in the grid as I am trying SU2 for a very simple problem just to check everything is fine. Yes, in future I will use SU2 for complex problems which will definitely have pyramids. Even without pyramids we seem to have problems.

I am compiling with cgns 3.1.4 version. I will try to compile it with lower version of cgns 2.5 and will keep it posted. In ICEM, I have tried with all the cgns export versions, but not successful

Hoping for the best. Thanks for the help again

Regards,
Vetri
vetri is offline   Reply With Quote

Old   February 27, 2014, 10:29
Smile A workaround for ICEM CGNS problem..
  #6
New Member
 
vetriselvan
Join Date: Jan 2010
Posts: 14
Rep Power: 7
vetri is on a distinguished road
Hi all,
I am able to somehow find a work around for this problem. I initially compiled SU2 v2.0 in serial with CGNS support after replacing the geometry_structure.cpp in /Common/src folder with the file suggested from this thread
cgns grid problem.

I just did make file and did not do make install. I used the SU2_CFD binary in SU2_CFD/bin folder to convert mesh from cgns to SU2. Then I installed SU2 eagle in parallel and used the converted mesh to run my simulations. Till now, I am not getting any problems.

Thanks to CFD-online members and SU2 developers... I am a beginner in CFD and working in SU2 is a great learning curve to me. Keep up the good work.Thanks again.

Regards,
Vetri
vetri is offline   Reply With Quote

Old   March 1, 2014, 20:44
Default
  #7
Member
 
Tommy Chen
Join Date: Mar 2011
Location: University of Michigan
Posts: 91
Rep Power: 6
Tommy Chen is on a distinguished road
Quote:
Originally Posted by vetri View Post
Hi all,
I am able to somehow find a work around for this problem. I initially compiled SU2 v2.0 in serial with CGNS support after replacing the geometry_structure.cpp in /Common/src folder with the file suggested from this thread
cgns grid problem.

I just did make file and did not do make install. I used the SU2_CFD binary in SU2_CFD/bin folder to convert mesh from cgns to SU2. Then I installed SU2 eagle in parallel and used the converted mesh to run my simulations. Till now, I am not getting any problems.

Thanks to CFD-online members and SU2 developers... I am a beginner in CFD and working in SU2 is a great learning curve to me. Keep up the good work.Thanks again.

Regards,
Vetri
Hi Vetri

Have you tried multi-zone CGNS mesh ?
Can SU2 successfully converted multi-zone CGNS mesh file ?
Tommy Chen is offline   Reply With Quote

Old   March 2, 2014, 00:06
Default
  #8
New Member
 
vetriselvan
Join Date: Jan 2010
Posts: 14
Rep Power: 7
vetri is on a distinguished road
Hi Tommy Chen,

I have not tried any multi-zone mesh. I have only used simple unstructured meshes. Even for that I faced all these conversion problems.

Regards,
Vetri
vetri is offline   Reply With Quote

Old   February 17, 2015, 16:58
Default
  #9
New Member
 
denzell
Join Date: Mar 2014
Posts: 12
Rep Power: 3
denzell is on a distinguished road
Tommy,

Do you intend to use multi-zone cgns in order to run use multiple processors for your simulation?

I encountered the same issue and solved it like this.
First compile SU2 from source, construct it with CGNS and MPI support.

Create your mesh in CGNS format.

Using a single zone CGNS mesh, call the SU2_CFD - space - testfile.cfg

Within your testfile.cfg set the option Convert mesh to SU2 format to YES.

This will translate your CGNS mesh to SU2 format.

Modify your testfile.cfg such that it now reads

meshfile = yourmesh.su2

and set the convert mesh to SU2 format to NO.

Now you can run your simulation on as many nodes as you like!

Good luck,

denzell
varghese9 likes this.
denzell is offline   Reply With Quote

Reply

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
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
[ANSYS Meshing] Generating Hexa-Core with ICEM CFD Interactive dawdybishop ANSYS Meshing & Geometry 0 July 15, 2013 05:29
[ICEM] Problem with volume mesh in ICEM CFD kolapoasafa ANSYS Meshing & Geometry 2 September 16, 2011 03:54
ICEM 12 CFD help creating volume mesh from stl EmpError ANSYS 0 November 13, 2010 07:38
How to extrude 2D Mesh in ICEM CFD? VSB CFX 7 December 27, 2006 12:58


All times are GMT -4. The time now is 04:55.