CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (https://www.cfd-online.com/Forums/ansys-meshing/)

 sunnyonly May 20, 2009 04:18

hi,everyone ,i am using icemcfd to model many architechtures and a outflowfield to simulate the ventilation.My problem is that ,i want to use tetra type about architechtures and hexa about outflow field ,what steps i can do to make it come true without errors.Thanks for any your honored answer.

 sunnyonly May 20, 2009 04:20

it is only one body ,but how can i seperate many parts to do this mesh method?

 Jules May 20, 2009 18:50

If you create your mesh from surface mesh, you can choose the mesh method individually for each surface patch.
"all quad" combined with "mapped" will give you a structured quadrilateral mesh (if number of nodes is equal on opposing edges), and a volume bounded by such surfaces should have structured hexa mesh.
"all tri" will lead to triangular surface mesh and tetrahedral volume mesh.

 PSYMN May 22, 2009 13:08

Merge tet and hex mesh

1 Attachment(s)
Hello,

In the mean time…

I am assuming that you have some building or group of buildings that are complicated and you don’t want to hexa mesh them, but you have a large far field that you want to hexa mesh…

You start by creating an interface between these regions… In ICEM CFD, you can use a Create Surfaces => primitive to create a box or sphere around your buildings. Then use the create intersection curve to intersect this primitive with the terrain. You can delete the part of the primitive outside of the domain (under ground) but it is not usually necessary. Name that interface geometry as “INTERFACE” or something like that. Put a material point inside the INTERFACE volume, if you want two materials, you could also put the other one outside (in the far field), but that is not needed.

I recommend saving the model as two geometry files. Save one copy as “Hexa_portion” and one as “Tetra portion”.

Then load the Hexa portion and generate the blocking for the region outside of the interface. Save this blocking and mesh. Close that project.

Open the Tetra portion and, if possible, delete the geometry outside of the interface. This will result in a smaller far field which will mesh more quickly with OCTREE. Setup and Mesh the tetra portion. Save.

Take care that the hexa mesh size at the interface is similar to the Tetra mesh size… Go back and adjust the hexa blocking if necessary. On the hexa side, also check the mesh size normal to the boundary, you want that to have similar volume elements to the tetra side. This usually means the hexa mesh size is a bit smaller than the tetra size…

Anyway, then go back and load the Hexa Portion (this is the full geometry). Load the hexa mesh and tetra mesh… When asked if you should replace or merge, choose merge. This actually just concatenates the meshes into the same file.

Once in ICEM CFD, go to mesh editing => Merge meshes. Select the INTERFACE part as the interface… It should work very easily… It is a very robust operation… It asks if you want to freeze anything, but you can leave that blank…

Afterward, you can convert tets to hexas, run prisms thru or whatever.

If you have any questions, Tech support at techsupp@ansys.com should be able to help.

 lalula2 September 23, 2010 11:33

Hi PSYMN, currently I am using ICEM to model building and simulate the ventilation around the building as well. Can you send me the ppt you mentioned in your previous post? Thanks. Regards.

 All times are GMT -4. The time now is 09:12.