CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Gambit Meshing

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 18, 2003, 06:51
Default Gambit Meshing
  #1
chanchala
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   July 18, 2003, 07:28
Default Re: Gambit Meshing
  #2
zxaar
Guest
 
Posts: n/a
use interfacing .... unite them in fluent (though interfacing sometimes is not a good idea)
  Reply With Quote

Old   July 18, 2003, 08:51
Default Re: Gambit Meshing
  #3
gelislim
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   July 18, 2003, 11:41
Default Re: Gambit Meshing
  #4
chanchala
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   July 18, 2003, 12:58
Default Re: Gambit Meshing
  #5
chanchala
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   July 18, 2003, 17:32
Default Re: Gambit Meshing
  #6
gelislim
Guest
 
Posts: n/a
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

  Reply With Quote

Old   July 19, 2003, 15:34
Default Why tet? Try all HEXA
  #7
Selina Tracy
Guest
 
Posts: n/a
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
  Reply With Quote

Old   July 20, 2003, 06:05
Default Re: Why tet? Try all HEXA
  #8
Jim Clancy
Guest
 
Posts: n/a
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
  Reply With Quote

Old   July 21, 2003, 05:04
Default Re: Why tet? Try all HEXA
  #9
gelislim
Guest
 
Posts: n/a
Hi Selina,

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

Regards
  Reply With Quote

Old   July 21, 2003, 06:50
Default Re: Why tet? Try all HEXA
  #10
chanchala
Guest
 
Posts: n/a
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!
  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
Gambit - meshing over airfoil wrapping (?) problem JFDC FLUENT 1 July 11, 2011 05:59
[ANSYS Meshing] Migrating from GAMBIT to ANSYS Meshing David-CFD ANSYS Meshing & Geometry 1 April 1, 2011 05:22
[GAMBIT] Desperate student needs help meshing 3D GAMBIT model - please help! lau06165 ANSYS Meshing & Geometry 1 March 22, 2010 02:09
Meshing problem in GAMBIT Vidya Raja FLUENT 0 May 20, 2006 23:31
Meshing Aircraft with Gambit Ed FLUENT 5 November 9, 2004 06:04


All times are GMT -4. The time now is 00:19.