CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Gambit Meshing (http://www.cfd-online.com/Forums/fluent/31854-gambit-meshing.html)

chanchala July 18, 2003 06:51

Gambit Meshing
 
Hi everyone, hope this isn't too easy a question! I'm modelling flow through 2 pipes- one a complex geometry, the other a simple one. I want a hexahedral mesh for the simple pipe and tetrahedral for the complex. I found that the 2 pipe geometries need to be united in Gambit for Fluent to give flow through one pipe onto the next. But if I'm uniting the 2 pipes I find I can only use one meshing scheme for both. If I mesh them separately and unite them afterwards the mesh does not export. thanks.

zxaar July 18, 2003 07:28

Re: Gambit Meshing
 
use interfacing .... unite them in fluent (though interfacing sometimes is not a good idea)

gelislim July 18, 2003 08:51

Re: Gambit Meshing
 
you need to split two volumes with eachother(bidirectional option) instead of uniting them. If you split them you will have 2 volumes which can be meshed seperately. First make hexa mesh and then make tetra mesh.

chanchala July 18, 2003 11:41

Re: Gambit Meshing
 
Hi, I tried splitting them like you said (I ticked bidirectional and said split first pipe with 2nd), but the exit of the first pipe and the entry of the second pipe then appear as walls when the mesh is imported into fluent. Please help if you can.

chanchala July 18, 2003 12:58

Re: Gambit Meshing
 
how do I interface? I tried specifying the walls in between the 2 pipes (exit and entry) as an interface by changing the boundary from a wall to interface but then the problem can't be initialised.

gelislim July 18, 2003 17:32

Re: Gambit Meshing
 
Hi,

Firstly, you need to check the "connected" box in split volumes form. This assure that two volumes use single face at interface. In your case, you should have forgotten to check the "connected" box so two different volumes have two different faces at interface section.

Finally, steps for grid interface set up in fluent are below

1) Change the apropriate walls to interface in define-boundary condition menu

2)Issue define-grid interfaces menu.If you made the first step correctly you should see two different face names in this menu.

3)Sellect them to make an interface pair (selection order is not important)and give a name.If your interface is between two different fluid region you do not need to do anything else. (After creating interface section you will see that you will have two new walls that can not be seen on the display window this is normal for interface bc's. Do not worry about them)

Remember that Fluent interpolates data at the interface sections so you must use similar element sizes on the two sides of interface to have small interpolation error.

Good Luck


Selina Tracy July 19, 2003 15:34

Why tet? Try all HEXA
 
Could you please let me share your geometry. I will try to make the mesh for you with all hex using my favorite preproccesor.

-Selina

Jim Clancy July 20, 2003 06:05

Re: Why tet? Try all HEXA
 
Chanchala,

If you still have problem with GAMBIT send me full details in word document I will try to mesh it for you the way you want.

Cheers

gelislim July 21, 2003 05:04

Re: Why tet? Try all HEXA
 
Hi Selina,

Which preprocessor is your favarite . ICEM-CFD or something else?

Regards

chanchala July 21, 2003 06:50

Re: Why tet? Try all HEXA
 
Hi guys, thanks all for the suggestions. Selina and Jim, my 2nd pipe's a twisted structure that I can't mesh with hexahedral cells in Gambit. Perhaps it can be done in other preprocessors though so I will send you the geometry after I've tried the other suggestions. Also what d'you think of meshing both pipes with tetrahedral cells? The 1st pipe as I mentioned is a normal cylindrical pipe. Is it complicating things unnecessarily? I did the simulation with all tet cells and there was no problems and the results look good.

I'm away for a week so it might be a while before I get back to Fluent and get to try your suggestions. I'll get back to you then. You're all great!


All times are GMT -4. The time now is 06:29.