CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

Mesh 2 bodies in 2 different programs

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 20, 2011, 09:49
Default Mesh 2 bodies in 2 different programs
  #1
Member
 
anonymous
Join Date: Jun 2011
Posts: 55
Rep Power: 6
Doginal is on a distinguished road
Hello All

I'm tried to mesh 2 different domain (a larger square box and a smaller cylindrical domain) in 2 different programs. I wish to mesh the large domain using ICEM so i can create a more structured expanding mesh which will simply be used to absorb the motion of the moving inner domain. The inner domain i would like to mesh using CFX.

Does anyone know how to import the 1 mesh from ICEM while still being able to edit the mesh in CFX for the other domain. Right now when i try to import the mesh, it doesn't allow any changes in the Ansys Workbench.

Any help will be greatly appreciated

Thank You,

DM
Doginal is offline   Reply With Quote

Old   September 20, 2011, 14:31
Default
  #2
Senior Member
 
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 236
Rep Power: 12
brunoc is on a distinguished road
ICEM can do that, but I think it works best if you also have the geometry.

If you're using ANSYS Meshing it is actually quite easy.
1. Import you're entire geometry into Meshing and generate the mesh only for the regions where you don't want to use ICEM (right-click each body and select 'Generate Mesh').
2. Go to File > Export and choose to export an ICEM project. That will export both an ICEM geometry file (.tin) and an ICEM mesh file (.uns).
3. Now open the geometry file (.tin) alone in ICEM and generate the mesh for the region not occupied by mesh you already have.
4. Open the mesh from Meshing. Choose 'Merge' when ICEM asks what to do with the mesh already loaded. This only means ICEM will load both meshed, but their interfaces will still have uncorformal elements and nodes.
5. Go to the 'Edit Mesh' tab, select the 'Merge Nodes' button (8th button from the left) and choose 'Merge Meshes' (3rd buttom).
6. The faces that connect each mesh must belong to the same ICEM family. Select this family for the 'Merge surface mesh parts' field.
7. Hit 'Apply' and you're done.

If you import your mesh from somewhere else, you should import the geometry used to generate the mesh as well. Then, inside ICEM, you have to associate the mesh to the geometry. Do this on 'Edit Mesh > Repair Mesh > Associate Mesh'. After this, procede with the steps I mentioned above.

Cheers
brunoc is offline   Reply With Quote

Old   September 20, 2011, 20:25
Default
  #3
Member
 
anonymous
Join Date: Jun 2011
Posts: 55
Rep Power: 6
Doginal is on a distinguished road
Quote:
Originally Posted by brunoc View Post
ICEM can do that, but I think it works best if you also have the geometry.

If you're using ANSYS Meshing it is actually quite easy.
1. Import you're entire geometry into Meshing and generate the mesh only for the regions where you don't want to use ICEM (right-click each body and select 'Generate Mesh').
2. Go to File > Export and choose to export an ICEM project. That will export both an ICEM geometry file (.tin) and an ICEM mesh file (.uns).
3. Now open the geometry file (.tin) alone in ICEM and generate the mesh for the region not occupied by mesh you already have.
4. Open the mesh from Meshing. Choose 'Merge' when ICEM asks what to do with the mesh already loaded. This only means ICEM will load both meshed, but their interfaces will still have uncorformal elements and nodes.
5. Go to the 'Edit Mesh' tab, select the 'Merge Nodes' button (8th button from the left) and choose 'Merge Meshes' (3rd buttom).
6. The faces that connect each mesh must belong to the same ICEM family. Select this family for the 'Merge surface mesh parts' field.
7. Hit 'Apply' and you're done.

If you import your mesh from somewhere else, you should import the geometry used to generate the mesh as well. Then, inside ICEM, you have to associate the mesh to the geometry. Do this on 'Edit Mesh > Repair Mesh > Associate Mesh'. After this, procede with the steps I mentioned above.

Cheers
Thank you very much. That is exactly what I need. Probably one of the best and clearest responses I've seen here.

DM
Doginal is offline   Reply With Quote

Old   September 20, 2011, 20:35
Default
  #4
Senior Member
 
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 236
Rep Power: 12
brunoc is on a distinguished road
Glad it helped.
brunoc is offline   Reply With Quote

Old   September 21, 2011, 12:16
Default
  #5
Member
 
anonymous
Join Date: Jun 2011
Posts: 55
Rep Power: 6
Doginal is on a distinguished road
Sorry 2 more questions

When trying to merge nodes to make the mesh conformal, what do you mean by the faces must belong to the same ICEM family.

Also when i try to import the mesh file back into ansys from ICEM, It seems to do something odd like the inner domain is 1 solid rather than a fluid with boundaries. I dont suppose you know why that is.

Thank You,

DM
Doginal 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
Number of cells in mesh don't match with size of cellLevel colinB OpenFOAM Native Meshers: snappyHexMesh and Others 11 January 13, 2015 12:47
[ICEM] surface mesh merging problem everest ANSYS Meshing & Geometry 39 June 5, 2013 19:02
2d irregular grid Remy Main CFD Forum 1 December 22, 2008 05:49
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
basic of mesh refinement arya CFX 4 June 19, 2007 12:21


All times are GMT -4. The time now is 01:08.