CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ...

Pointwise grid export to Openfoam

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

Like Tree2Likes
  • 2 Post By cnsidero

Reply
 
LinkBack Thread Tools Display Modes
Old   January 4, 2011, 10:52
Default Pointwise grid export to Openfoam
  #1
Member
 
The True
Join Date: Dec 2010
Posts: 80
Rep Power: 5
Eren10 is on a distinguished road
Hi,

I want to export the mesh generated with the Pointwise to OpenFoam. How should I do this.

There is three options at the export: Grid , Database or CAE.
I have only generated mesh, after this only the export > Grid is available. I do not see the right export extensions, even for Fluent.
Eren10 is offline   Reply With Quote

Old   January 4, 2011, 14:00
Default
  #2
Member
 
Dennis Kingsley
Join Date: Mar 2009
Location: USA
Posts: 45
Rep Power: 7
dkingsley is on a distinguished road
Quote:
Originally Posted by Eren10 View Post
Hi,

I want to export the mesh generated with the Pointwise to OpenFoam. How should I do this.

There is three options at the export: Grid , Database or CAE.
I have only generated mesh, after this only the export > Grid is available. I do not see the right export extensions, even for Fluent.
You will have to build your volume grids in Pointwise and add boundary conditions to the faces before you can export to OpenFOAM using the CAE option.

Dennis
dkingsley is offline   Reply With Quote

Old   January 4, 2011, 16:28
Default
  #3
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 338
Rep Power: 11
cnsidero is on a distinguished road
@Eren10

I will add to dkingsley's post.

First, be sure to set you CAE type to OpenFOAM (CAE > Select Solver ... OpenFOAM).

Next, like dkingsley said, you have to have a volume mesh complete. As you know OpenFOAM works in 3D all the time so even if you are doing a 2D simulation you must make the grid 3D first.

Then you can set volume conditions on the volume mesh and boundary conditions on the domains.

Once the above steps have been complete, to save you mesh in the native OpenFOAM format, choose File > Export > CAE ... and the choose the folder to save the files.

For your reference, exporting to Grid allows you to save the mesh only in various neutral or generic formats (PLOT3D, NASTRAN, etc) but no volume or boundary conditions. Export to Database allows you to save the geometry only to various neutral or generic formats (DBA, IGES). The last one, Export to CAE allows to save the mesh, the volume and the boundary conditions to the solver you have chosen.

Hope that helps.
cnsidero is offline   Reply With Quote

Old   January 10, 2011, 02:53
Default
  #4
New Member
 
Join Date: Jul 2009
Posts: 10
Rep Power: 7
Lodda is on a distinguished road
Befor you can export the mesh you have to select all blocks. Then you can export your Volume-Mesh with File -> Export to CAE.

Best regards

Lodda
Lodda is offline   Reply With Quote

Old   January 10, 2011, 06:43
Default
  #5
Member
 
The True
Join Date: Dec 2010
Posts: 80
Rep Power: 5
Eren10 is on a distinguished road
Thank you guys. I have done it. Also it is important for 2D to generate the third dimension only with 1 step.
Eren10 is offline   Reply With Quote

Old   June 10, 2013, 14:49
Default Pointwise - OpenFOAM
  #6
MDB
New Member
 
Manuel Díaz Brito
Join Date: Jun 2013
Posts: 16
Rep Power: 3
MDB is on a distinguished road
I am new with this Pointwise - OpenFOAM interface, but the issues discussed in this thread are well known to me and already overcome. However I am getting very bad results in OpenFOAM and the settings don't look too bad, so I keep questioning the grid generation... Setting the Boundary Conditions (BCs) is pretty straightforward, but when I set Volume Conditions (VCs) I doubt: should I give a specific name so OpenFOAM recognises it?
My case is quite simple and I only have 1 volume which should be fluid (air), so setting all blocks of the mesh as "set" (which is the only option pointwise offers) is the only thing I can do... so how and where does OpenFOAM read these VCs?
Thanks
MDB is offline   Reply With Quote

Old   August 16, 2013, 07:36
Default
  #7
New Member
 
tobyB
Join Date: Aug 2013
Posts: 11
Rep Power: 3
tobyB is on a distinguished road
You mention building volume condtions. When I tried to this there were no changes to the outputfiles compared to when I only specified bounarys.

How do you specify volume conditions on pointwise and what should the resulting output files looklike?

Thanks

Toby
tobyB is offline   Reply With Quote

Old   August 17, 2013, 04:48
Default
  #8
MDB
New Member
 
Manuel Díaz Brito
Join Date: Jun 2013
Posts: 16
Rep Power: 3
MDB is on a distinguished road
Dear tobyB,

As far as I have used Pointwise, when exporting to OpenFOAM, it doesn't make any difference whether you specify volume conditions or not. I do not know if it has an implication I might not be aware of, but for how OpenFOAM read the files, specifying volume conditions is not necessary. If you are exporting into OpenFOAM you should get 5 files named boundary, faces, neighbour, owner and points.

Hope this helps,

MDB
MDB is offline   Reply With Quote

Old   August 19, 2013, 05:03
Default
  #9
New Member
 
tobyB
Join Date: Aug 2013
Posts: 11
Rep Power: 3
tobyB is on a distinguished road
Ah okay then, do you know then how I would use those files in order to define different regions?

I am working of the example: chtMultiRegionSimpleFoam->multiRegionHeater. Which seems to define different regions by using boxToCell and then setToCellZone, highlighting cells within a cuboid shape. Although this is fine for simple examples, I need to define more complex geometries to a specific region.

Would this be possible using some of the boundary conditions that you can export from pointwise, and then using faces to select the cells.
Or should I perhaps export the mesh twice, selecting each block section seperatley, two get two sets of boundary points etc? If so, how would I connect these up?

Thanks,

Toby
tobyB is offline   Reply With Quote

Old   August 19, 2013, 08:55
Default
  #10
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 338
Rep Power: 11
cnsidero is on a distinguished road
As MDB said, setting volume conditions for OpenFOAM export does nothing.
cnsidero is offline   Reply With Quote

Old   August 19, 2013, 11:00
Default
  #11
New Member
 
tobyB
Join Date: Aug 2013
Posts: 11
Rep Power: 3
tobyB is on a distinguished road
right then, so what do you think the best way of implemeting different cellzones from pointwise meshes would be?
tobyB is offline   Reply With Quote

Old   August 19, 2013, 11:26
Default
  #12
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 338
Rep Power: 11
cnsidero is on a distinguished road
Actually, I spoke too quickly. I forgot the ability to export volume conditions as cellZones and cellSets was recently added to Pointwise OpenFOAM exporter. If you grab the latest release candidate, it has this capability:

http://www.pointwise.com/support/dload_rc.shtml

What the volume condition writes out is controlled by the solver attributes found in CAE, Set Solver Attributes.

-Chris
dkingsley and tobyB like this.
cnsidero is offline   Reply With Quote

Old   August 19, 2013, 12:01
Default
  #13
New Member
 
tobyB
Join Date: Aug 2013
Posts: 11
Rep Power: 3
tobyB is on a distinguished road
which version are you talking about specifically?
I just got 17.1 R3, does it have to be C4 too? If this works then it will be a great help.
tobyB is offline   Reply With Quote

Old   August 19, 2013, 12:37
Default
  #14
New Member
 
tobyB
Join Date: Aug 2013
Posts: 11
Rep Power: 3
tobyB is on a distinguished road
Ok, ive only tried it briefly but the new version (not just R4) did give me some good results. Ill try tommorow to encorperate them into an existing case. Thanks alot cnsidero.

Toby
tobyB 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
Cyclic BCs in PointwiseOpenFOAM export cnsidero OpenFOAM Meshing & Mesh Conversion 18 July 30, 2013 09:36
The OpenFOAM extensions project mbeaudoin OpenFOAM 16 October 9, 2007 09:33
How to generate OpenFOAM grid from DEM data rcpoudel OpenFOAM Pre-Processing 1 May 22, 2006 13:41
OpenFOAM Training and Workshop Zagreb 2628Jan2006 hjasak OpenFOAM 1 February 2, 2006 21:07
Combustion Convergence problems Art Stretton Phoenics 5 April 2, 2002 04:59


All times are GMT -4. The time now is 21:56.