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

how to create 2d cases with netgen

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 11, 2010, 13:45
Default how to create 2d cases with netgen
  #1
Member
 
Daniel
Join Date: Jul 2010
Location: California
Posts: 39
Rep Power: 7
hyperion is on a distinguished road
Hi there - I would like to create a 2d case with the front and rear faces of the domain being of type empty. However, for meshes that I have imported using netgen I get the following error in the initialization step:

--> FOAM FATAL ERROR:
This mesh contains patches of type empty but is not 1D or 2D
by virtue of the fact that the number of faces of this
empty patch is not divisible by the number of cells.

Because the mesh is only one layer of cells thick I have to assume this is because netgen creates tetrahedral meshes. I have also tried importing quad dominated meshes from netgen without success.

It seems that others may have had similar issues, but any help would be greatly appreciated.

Thank you all very much for all the help.
hyperion is offline   Reply With Quote

Old   August 12, 2010, 13:37
Default
  #2
Senior Member
 
Philippose Rajan
Join Date: Mar 2009
Location: Germany
Posts: 530
Rep Power: 16
philippose will become famous soon enough
Hello there,

A Good Evening to you, and sorry for the delay in replying to your post.

Well... OpenFOAM more or less works exclusively with 3-D cases, with 2-D being emulated by using a mesh which is flat (2 dimensional), and contains only one layer of cells in the third dimension.

A Mesh of this kind will not be very easy to generate using Netgen, because you cannot explicitly tell Netgen to limit itself to purely one layer of cells in one dimension. Netgen is essentially an unstructured tetrahedral mesh generation tool.

What you really need, is a way to extrude 2-D meshes in the third dimension.

I looked around in the palette of OpenFOAM mesh utilities, and found two utilities "extrude2DMesh" and "extrudeMesh".

Now... "extrudeMesh" seems to work only with an already existing volume (3-D) mesh, in order to further extrude an existent patch along its normal.

"extrude2DMesh" seems to be more of a 2-D mesh extrusion tool, but I could not get it to work (yet).

I have extruded 2-D meshes into the third dimension some time ago, using the Salomé Platform.... using this program, you can easily mesh a 2-D surface, and extrude this mesh.

Once you extrude it, you can export the mesh in the "UNV" format, and use the mesh conversion tool "unvToFoam" (I think?) to convert it into the OpenFOAM format.

Hope this helps :-)!

Have a great day ahead!

Philippose
philippose is offline   Reply With Quote

Old   August 14, 2010, 09:39
Default
  #3
Senior Member
 
Elvis
Join Date: Mar 2009
Location: Sindelfingen, Germany
Posts: 577
Blog Entries: 5
Rep Power: 13
elvis is on a distinguished road
Quote:
Originally Posted by philippose View Post
H

I have extruded 2-D meshes into the third dimension some time ago, using the Salomé Platform.... using this program, you can easily mesh a 2-D surface, and extrude this mesh.

Once you extrude it, you can export the mesh in the "UNV" format, and use the mesh conversion tool "unvToFoam" (I think?) to convert it into the OpenFOAM format.
better you use ideasUnvToFoam
there is a little video howto http://www.caelinux.org/wiki/index.p...ELinux_2007.29

salome makes use of netgen or gmsh as some of the meshing tools among many (plugins for external meshers)
elvis is offline   Reply With Quote

Old   August 14, 2010, 14:11
Default
  #4
Member
 
Daniel
Join Date: Jul 2010
Location: California
Posts: 39
Rep Power: 7
hyperion is on a distinguished road
Hi Philippose and Elvis - Thanks for the help. For now I was able to get by using blockMesh, but perhaps as my geometry becomes more complex I will try out one of the software packages you recommend.

Thanks Again!
hyperion is offline   Reply With Quote

Old   August 18, 2011, 09:55
Default
  #5
New Member
 
Amin
Join Date: Oct 2010
Location: Notre Dame, US
Posts: 6
Rep Power: 6
AcfdO is on a distinguished road
Hi,

The other way to tackle this problem is to use Gambit as a mesh generator. You can generate a face mesh and then use "Geometry->Volume>Sweep Faces" and activate the option "with mesh". This will create the ideal mesh to use for 2D openfoam calculations. You can export mesh and then use "fluent3DMeshToFoam" command and set the appropriate boundary conditions in "constant/polyMesh/bondary".
AcfdO is offline   Reply With Quote

Reply

Tags
2-d, empty, netgen

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
Geometry > Netgen > OpenFOAM ericnutsch Open Source Meshers: Gmsh, Netgen, CGNS, ... 9 February 22, 2010 08:39
Actuator disk model audrich FLUENT 0 September 21, 2009 07:06
Where's the singularity/mesh flaw? audrich FLUENT 3 August 4, 2009 01:07
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
Meshing a Sphere Ajay FLUENT 9 March 29, 2004 09:14


All times are GMT -4. The time now is 03:49.