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

Importing Multiple Meshes

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

Like Tree1Likes
  • 1 Post By thomasnwalshiii

Reply
 
LinkBack Thread Tools Display Modes
Old   November 19, 2010, 11:42
Default Importing Multiple Meshes
  #1
New Member
 
Thomas Walsh
Join Date: Nov 2010
Posts: 17
Rep Power: 5
thomasnwalshiii is on a distinguished road
I would like to import multiple meshes (solid and air parts) into an OpenFoam simulation. I have briefly played around with using the snappy mesh feature but was curious if i could use Salome (or other mesh software) to mesh my various objects separately and then bring them into an OpenFoam case. Any advise on this topic would be appreciated.

Thank.
thomasnwalshiii is offline   Reply With Quote

Old   December 2, 2010, 15:24
Default
  #2
New Member
 
Jean El-Hajal
Join Date: Jun 2010
Location: Ulm
Posts: 16
Rep Power: 6
Jean El-Hajal is on a distinguished road
Hi Thomas,

i am not sure it works, but I am putting some effort on it based on the chtMultiRegionFoam/snappyMultiregionHeater. I made and meshed a coumpound geometry in Salome and export it as .UNV.

Then:

1- UNVToFoam your_mesh.UNV
2- splitMeshRegions -cellZones -overwrite

This seems to create folder similar to the chtMultiRegionFoam/snappyMultiregionHeater case.

Well I still have to work on it, change the dictionary ....

But this could be the start point. If I do any progress I will let you know , probably during X-mas holiday

hope it helps

Jean
Jean El-Hajal is offline   Reply With Quote

Old   July 22, 2011, 15:45
Default Any Updates
  #3
New Member
 
Thomas Walsh
Join Date: Nov 2010
Posts: 17
Rep Power: 5
thomasnwalshiii is on a distinguished road
Jean,

I am curious if you ever found out if this process worked? I have recently (again) tried to create compound geometry mesh and convert it into openfoam with ideasUNVToFoam but have been unsuccessful. What process did you use to create the compound mesh? I am using the 'Fuse' then 'Partition' features and finally meshing the whole assembly and creating sub-meshes of each individual part.

Here is the process which I have been using for meshing multiple parts in Salome, http://www.caelinux.org/wiki/index.p...ters/partition.
thomasnwalshiii is offline   Reply With Quote

Old   July 23, 2011, 23:59
Default Finally got it to work
  #4
New Member
 
Thomas Walsh
Join Date: Nov 2010
Posts: 17
Rep Power: 5
thomasnwalshiii is on a distinguished road
I was finally able to import an assembly mesh into OpenFOAM format with the following Salome>Gmsh>OpenFOAM process:

-Using Salome:
1. Within the Geometry module explode surfaces needed for Boundary Conditions and renamed them
2. Fused all parts together into a single assembly
3. Partitioned this assembly using each of the parts included
4. Created 'Volume Groups' for each partitioned part
5. Move to the Meshing module and mesh the whole partitioned assembly (optional: make sub-meshes of the parts to better control mesh sizing)
6. Make 'Volume Groups' of each part within the mesh
7. Make 'Surface Groups' for all the boundary conditions
8. Export mesh as MED file (need to check 'Automatically Create Groups' box)

-Using Gmsh
9. Open mesh file in Gmsh and 'Save As' Gmsh mesh file (.msh file extension, make sure file is saved as Version 2.0 ACSII and un-check all check boxes)
10. Move Gmsh mesh file into an empty case file (make sure to have constant->polyMesh (empty) and system folder with necessary files)

-OpenFOAM mesh conversion/manipulation tools
11. Run [>> gmshToFoam] in OpenFOAM terminal within the case directory
12. Run [>> splitMeshRegions -cellZonesOnly -overwrite] (this is only used if there are multiple parts (volumes) to be split up)

The following two links talk about this process:
http://www.caelinux.org/wiki/index.p...ters/partition
http://www.salome-platform.org/forum...10/thread_3005
elvis likes this.
thomasnwalshiii is offline   Reply With Quote

Old   July 24, 2011, 09:30
Default
  #5
Senior Member
 
Elvis
Join Date: Mar 2009
Location: Sindelfingen, Germany
Posts: 501
Blog Entries: 4
Rep Power: 12
elvis is on a distinguished road
Hi,

i want to mention that there seems to be a way to directly export from salome to openfoam.
http://pythonflu.wikidot.com/hybridflu

Ivor Clifford
http://www.openfoamworkshop.org/6th_...ord_slides.pdf (=>slide 19"Meshing section") mentions that direct in memory Salome2OF mesh writing via pythonflu supports meshes that ideasUnvtoFoam does not support
elvis is offline   Reply With Quote

Old   August 1, 2011, 16:41
Default
  #6
New Member
 
Jean El-Hajal
Join Date: Jun 2010
Location: Ulm
Posts: 16
Rep Power: 6
Jean El-Hajal is on a distinguished road
Hi Thomas,

Sorry for the late response i was in holiday :-)
yes I was able to do it. If you need more details let me know it.


  1. Create the fluid and solid domain in Salome in the geom mode
  2. explode the solid and the fluid domains in faces
  3. mesh the solid and the fluid domains separately and create for each domain group of the faces of interest, for example inlet, outlet and don't forget to define the faces of the solid and fluid that will be in contact
  4. in mesh mode build a compound mesh with the 2 meshs (solid and fluid).
  5. Export the compound mesh in UNV format


OpenFoam
  1. use ideasUnvToFoam to export the mesh to OpenFoam
  2. splitMeshRegions -cellZones -overwrite → this create 2 region.
  3. adjust the file boundary, fvschemes, fvsolutions ...
Jean El-Hajal is offline   Reply With Quote

Old   October 13, 2011, 06:45
Default
  #7
New Member
 
Antonello
Join Date: Apr 2010
Posts: 20
Rep Power: 6
antonessiu is on a distinguished road
Read this:
http://www.caelinux.org/wiki/index.p...ters/partition
antonessiu 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
OpenFOAM static build on Cray XT5 asaijo OpenFOAM Installation 9 April 6, 2011 12:21
Importing multiple mesh Shafiul CFX 1 July 5, 2010 19:04
Exporting Multiple Meshes to Fluent anksta FLUENT 3 May 5, 2009 08:07
Multiple Moving Meshes Animation Tristan CFX 3 March 19, 2009 20:14
Importing Meshes from ANSYS Kieran Hood CFX 3 December 18, 2006 03:53


All times are GMT -4. The time now is 08:32.