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

Getting GGI-ready mesh from conversion

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

Like Tree1Likes
  • 1 Post By lentschi

Reply
 
LinkBack Thread Tools Display Modes
Old   May 4, 2011, 21:54
Default Getting GGI-ready mesh from conversion
  #1
Senior Member
 
Robert
Join Date: Sep 2010
Posts: 154
Rep Power: 6
lordvon is on a distinguished road
I am trying to use Pointwise to create structured meshes for a GGI case (which I run unstructured grids with successfully). The openfoam export does not seem to be ready for ggi (includes 'boundary','faces','neighbor','owner','points'). So I try to export it to fluent and convert it.

My question is, has anybody converted a fluent mesh for ggi?
lordvon is offline   Reply With Quote

Old   May 5, 2011, 10:42
Default
  #2
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 471
Rep Power: 11
bastil is on a distinguished road
Quote:
Originally Posted by lordvon View Post
My question is, has anybody converted a fluent mesh for ggi?
Yes. What exactly is your problem?

Regards Bastian
bastil is offline   Reply With Quote

Old   May 5, 2011, 10:59
Default
  #3
Member
 
don lenardo
Join Date: Nov 2010
Posts: 75
Rep Power: 6
lentschi is on a distinguished road
Yes I have converted some fluent-meshes to Foam with fluent3DMeshToFoam.

But take a look on your converted patches - maybe you have to change them (for example from "wall" / "patch" to "ggi") in OpenFoam!

Regards
lentschi is offline   Reply With Quote

Old   May 5, 2011, 12:05
Default
  #4
Senior Member
 
Robert
Join Date: Sep 2010
Posts: 154
Rep Power: 6
lordvon is on a distinguished road
Thanks guys for the responses.

So whenever I convert the mesh it doesnt seem to be ggi-ready and im not sure what to do.

I noticed that 'cellZones' is created but it is empty. Is this an essential file for ggi?
lordvon is offline   Reply With Quote

Old   May 6, 2011, 04:58
Default
  #5
Member
 
don lenardo
Join Date: Nov 2010
Posts: 75
Rep Power: 6
lentschi is on a distinguished road
you can get "CellZones" with the command "splitMeshRegions -makeCellZones".

In your boundary-file you have to define the desired ggi-patches - take a look on the validation test cases to get an overview of setting up a case!

http://openfoamwiki.net/index.php/Si...ion_test_cases

In the "centrifugal pump" there is described how to create ggi patches correctly.
elvis likes this.
lentschi is offline   Reply With Quote

Old   May 8, 2011, 20:14
Default
  #6
Senior Member
 
Robert
Join Date: Sep 2010
Posts: 154
Rep Power: 6
lordvon is on a distinguished road
Thanks guys for the replies. I have been able to make progress with you all's help, but still I face a problem. The following is the procedure I used to generate the mesh case: (ggi, there exists a rotor and stator)

1. Pointwise 3D mesh OpenFoam export for 2 grids (rotor and stator), 5 files each (boundary, points, faces, neighbor, owner)
2. mergeMeshes
3. splitMeshRegions -makeCellZones
4. setSet -batch setBatch (file 'setBatch' contains: (line 1) 'faceSet insideZone new patchToFace insideSlider' (line 2) 'faceSet outsideZone new patchToFace outsideSlider' (line 3) 'quit')
5. setsToZones -noFlipMap

Then i run it using 'decomposePar' and 'foamJob -s -p turbDyMFoam'.

It runs for a while, but then things start going crazy on the readout, because i have not set it up for ggi to work properly, please see the attached images of the ggi interface.

Anybody know what I am doing wrong? I will be trying to debug this and try splitMeshRegions on a Pointwise export with both rotor and stator in one mesh (differently defined cell 'sets') to see if that works.
Attached Images
File Type: jpg originalmesh.jpg (54.4 KB, 20 views)
File Type: jpg extremeskew.jpg (54.8 KB, 22 views)
lordvon is offline   Reply With Quote

Old   May 9, 2011, 03:39
Default
  #7
Member
 
don lenardo
Join Date: Nov 2010
Posts: 75
Rep Power: 6
lentschi is on a distinguished road
do you set up the "dynamicMeshDict" file?
please post your boundary- and the dynamicMeshDict-file and the log-files of checkMesh and your run , so that we can get an overview of your problem!
What happens,if you run the solver with only ONE CPU??
lentschi is offline   Reply With Quote

Old   May 9, 2011, 09:06
Default
  #8
Senior Member
 
Robert
Join Date: Sep 2010
Posts: 154
Rep Power: 6
lordvon is on a distinguished road
Attached are the 3 files you requested. I will try serial run and let you know how that goes.

The case is an o-grid external flow (so it has a circular outer boundary).
Attached Files
File Type: txt boundary.txt (1.9 KB, 4 views)
File Type: txt checkmesh log.txt (3.0 KB, 6 views)
File Type: txt dynamicMeshDict.txt (1.2 KB, 6 views)
lordvon is offline   Reply With Quote

Old   May 9, 2011, 09:25
Default
  #9
Member
 
don lenardo
Join Date: Nov 2010
Posts: 75
Rep Power: 6
lentschi is on a distinguished road
Did you adapt your field-files correctly (in the field-files there are "boundary-fields" too, and they must have the same entries as your boundary-file!!)?

In the cellZones-file, the ROTATING ZONE MUST have the name "movingCells" - ckeck this out! (If you use a transient solver,you do not need to create a cellZones file, mixerGGI... will do this for you!Delete the cellZones-file,start the solver and check the things I described above).


...and please post the log of your calculation!!
lentschi 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
mesh conversion for dispersed liquid drop flowing upward in a continous phase hossein.mashhadi OpenFOAM Running, Solving & CFD 0 February 3, 2011 17:42
mesh conversion for dispersed liquid drop flowing upward in a continous phase hossein.mashhadi OpenFOAM 0 February 2, 2011 11:43
ansys icem tetra mesh to fluent_v6 conversion problems milleniumrider OpenFOAM Meshing & Mesh Conversion 3 May 13, 2010 14:54
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
Turbogrid-icem mesh ggi Kumar CFX 1 May 18, 2007 04:19


All times are GMT -4. The time now is 02:23.