CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Meshing & Mesh Conversion

[Commercial meshers] Conversion of OpenFoam mesh to .msh

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

Like Tree1Likes
  • 1 Post By simrego

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 14, 2019, 05:43
Post Conversion of OpenFoam mesh to .msh
  #1
New Member
 
Srinath Reddy Gudupally
Join Date: Jul 2018
Location: Jena-Germany
Posts: 12
Rep Power: 3
Srinath Reddy is on a distinguished road
Send a message via Skype™ to Srinath Reddy
Hi,

I want to convert foam mesh to Fluent. Is there any Utility? I Have tried foamMeshTofluent but it improting my block mesh but not the main geometry.

Can any one have an Idea?

thank you
Srinath Reddy is offline   Reply With Quote

Old   January 14, 2019, 09:22
Default
  #2
Senior Member
 
anonymous
Join Date: Jan 2016
Posts: 238
Rep Power: 6
simrego is on a distinguished road
Hi!


You can export it to EnSight ("foamToEnsight") and you can import EnSight into fluent.
ramakant likes this.
simrego is offline   Reply With Quote

Old   January 14, 2019, 12:19
Default Ensight Mesh Precision
  #3
ICS
New Member
 
Join Date: Aug 2013
Posts: 12
Rep Power: 7
ICS is on a distinguished road
I'm working on a case with a very high mesh aspect ratio (I need to solve the boundary layer for a supersonic flow). Hence, I need to increase the writing precision for the "geometry" file when I use the application foamToEnsightParts... the default result using the -ascii option is scientific notation with 5 decimals and that's not enougth for me.
Changing the controlDict writePrecision doesn't help, neither the foamToEnsightParts -width option... Any ideas how to do that?
ICS is offline   Reply With Quote

Old   January 15, 2019, 06:20
Default
  #4
New Member
 
Srinath Reddy Gudupally
Join Date: Jul 2018
Location: Jena-Germany
Posts: 12
Rep Power: 3
Srinath Reddy is on a distinguished road
Send a message via Skype™ to Srinath Reddy
Hello Simrego!!!

thank you for the Information... it actually worked, but I am facing same Problem. it just improting my blockMesh. Have any idea how to do it so that i could get 3D geometry?
Srinath Reddy is offline   Reply With Quote

Old   January 23, 2019, 08:34
Default Ensight mesh precision
  #5
ICS
New Member
 
Join Date: Aug 2013
Posts: 12
Rep Power: 7
ICS is on a distinguished road
After a lot of work, here are some conclusions I came with:

1 - I managed to improve the precision of the geometry files generated by foamMeshToEnsight and foamMeshToEnsightParts. I did it by changing some parameters on both applications files and compiling again with wmake. But I found out that It was in vain, since Ensight geometry files must be written on 12.5e format (scientific notation with 5 decimal places) according to http://www3.ensight.com/EnSight92_Docs/UserManual.pdf... So I gor error messages when I tried to import into Fluent...

2 - The foamMeshToFluent combine all cell zones into one internal fluid region... but my case must have distinct cell zones since I'm modelling fluid-solid interation... the default precision of the generated .msh file is scientific notation with 10 decimal places. If you need to improve that just change "fluentMeshFile.precision(10);" on the fluentFvMesh.C file and compile with wmake.

3 - The best solution I got was:
a) use the splitMeshRegions -cellzones -overwrite in order to generate polyMesh files for each cell zone (my original mesh was generated on SALOME and imported using ideasUnvToFoam).
b) copy the polyMesh folder generated for each cell zone to the constant directory (substituting the original polyMesh folder).
c) use the foamMeshToFLuent to generate the .msh file for each cell zone once at a time and save them with diferent names.
d) open Fluent, read one .msh file and load the other ones by using the append option (see https://www.sharcnet.ca/Software/Flu...ug/node171.htm)
e) for each interface between cell zones use the combine/fuse option.

It's quite some work, but it's a solution for converting OpenFoam mesh with multiple cell zones into fluent and preserve the precision.
ICS is offline   Reply With Quote

Old   January 23, 2019, 08:59
Default
  #6
Senior Member
 
anonymous
Join Date: Jan 2016
Posts: 238
Rep Power: 6
simrego is on a distinguished road
Quote:
Originally Posted by Srinath Reddy View Post
Hello Simrego!!!

thank you for the Information... it actually worked, but I am facing same Problem. it just improting my blockMesh. Have any idea how to do it so that i could get 3D geometry?



Hi!


Sorry, but i don't know what do you mean exactly under 3D geometry. You need the mesh or the geometry itself? If you need the geometry you can use the surfaceMeshTriangulate utility to export your surface mesh as an stl file. I don't think if there are any another way to export the geometry. And also not clear for me why do you have to export the geometry.
simrego is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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
[Gmsh] 3D Mesh conversion from gmsh-2.5.0 to OpenFOAM Ancioi OpenFOAM Meshing & Mesh Conversion 17 January 8, 2019 23:50
[Commercial meshers] Problems with ANSYS mesh conversion tdog OpenFOAM Meshing & Mesh Conversion 1 March 31, 2016 17:36
[Other] vtk mesh or Abaqus mesh to OpenFOAM bigphil OpenFOAM Meshing & Mesh Conversion 27 November 23, 2015 17:31
[snappyHexMesh] No layers in a small gap bobburnquist OpenFOAM Meshing & Mesh Conversion 6 August 26, 2015 09:38
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 11:55


All times are GMT -4. The time now is 17:53.