CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [ICEM] problem to merge HEXA/TETRA grid (

bikino January 22, 2011 06:27

problem to merge HEXA/TETRA grid
Hi I am a new user of the package ANSYS for solving fluid dynamics problems, I have to mesh a burner, so I was advised to use a hybrid mesh HEXA / TETRA, within a complex domain go to directly create a geometry consists in ICEM stuck on a cylinder with a truncated cone, which will generate the HEXA mesh, and the rest of the domain will use a mesh TETRA, the problem is created when the two met through the mesh and mesh merge command, on the surface of union which remains a shell-type quad / tri once imported into CFX or FLUENT remains, but in theory there should not be because the fluid passes.
-the gate before exporting, create errors in the mesh
if imposed as a surface-interface in CFX I do not have good risultai
Does anyone have advice?? Or tell me what is wrong in the process of generating a hybrid mesh??
Thank you very much

BrolY January 24, 2011 04:42

You should have created two interfaces into ICEM (the surface where you connected your 2 mesh should be meshed in Tetra and in Hexa, so 2 interfaces).
So, once you merged your two interfaces, you should delete both of them (if the fluid is supposed to pass thru there). It would delete the surface elements, but keep the volume elements.

bikino January 24, 2011 16:48

I create a conical cylinder-shaped surface, I create the blocking splits into 5 parts, I associate the blocking parts of the curves, and splits to go to ogrid, the blocking is created in the same part that contains the body, while the surface interface is located in another part.
dell'ogrid assign to each element, a number of nodes, move the body in the domino hexa and do the command to convert unstructured mesh, carry out the body count the mesh, I'm going to do the merge of meshs, but every time I error vertex incorrect, what wrong?

BrolY January 25, 2011 04:33

Here is the procedure :

1) Go to Merge Nodes/Merge Tolerance. Then select a tolerance lower than your small mesh size for example. Select the option "Ignore Projection". And after that, select the the two interfaces which should be in contact. Click Apply.
2) Then go to the "Delete Elements mesh" tab, select "Delete by parts" and select your interface parts.

Anyway, is there a big difference between the cell sizes of your both meshes ?
Maybe you could try to play with the tolerance.
Hope it helps !

PSYMN January 29, 2011 21:00

My 2 cents...

After the merge, all the triangles on the interface part (you can use two parts or just one, it doesn't matter but some people like them to be separate so they can check them separately) should be gone and only quads should remain. If you have any triangles left, then the merge didn't work properly...

I have lots of posts about how to do this correctly, but the main thing is that the interface part(s) should only be about the interface (never used elsewhere) and that the entire perimeter should be shared with curve projected nodes (hexa side needs to be associated to the perimeter curves).

Anyway, I suspect that you did do it right and just have a layer of quads between your two connected volumes. If you want it to be one domain, make sure to move all the volume elements into a single part (right click on the one volume part => Add to part => use the selection tool bar to select all the volume elements.) Then you can delete the shells in the interface part... (Edit Mesh (tab) => Delete => Use the selection toolbar to select by parts, then select the interface parts to delete all their shells.

Best regards,


bikino January 30, 2011 05:31

Grazie per la risposta Simon,
non so cosa ci sia di sbagliato, quando creo la mesh di volume sia la parte tetra che la parte hexa sono nella stessa part, che la stessa che contiene il BODY e il BLOCKING, mentre la superficie di interfaccia si trova in un altra part e la sua mesh di tipo shell costituita sia da elementi tri sia da elementi quad.
E fino a qui tutto ok. adesso cerco di unire la mesh con il comando merge mesh, ma ogni volta ho dei vertici che non vengono uniti, come posso fare a unire questi elementi manualmente? quando creo il blocking devo mantenere in 2 part diverse le superfici e le curve? nel mesh part parameters devo impostare un parametro dimensionale per la superficie di interfaccia??
Thank you very much

PSYMN January 30, 2011 13:20

Spiacente, il mio italiano non abbastanza buono per capire questo messaggio. :o

I tried translation software, but it didn't do a very good job. :(

All times are GMT -4. The time now is 03:51.