CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   Mesh 2 bodies in 2 different programs (http://www.cfd-online.com/Forums/ansys-meshing/92633-mesh-2-bodies-2-different-programs.html)

Doginal September 20, 2011 09:49

Mesh 2 bodies in 2 different programs
 
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

brunoc September 20, 2011 14:31

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

Doginal September 20, 2011 20:25

Quote:

Originally Posted by brunoc (Post 324921)
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

brunoc September 20, 2011 20:35

Glad it helped.

Doginal September 21, 2011 12:16

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


All times are GMT -4. The time now is 22:00.