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

export prblem with Gambit and Fluent

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 2, 2006, 10:11
Default export prblem with Gambit and Fluent
  #1
Mignolo
Guest
 
Posts: n/a
i have a volume meshed with Hex ( type submap , worst element with angle skew <0.4). It looks like a perfect mesh but when i export it to Fluent and i display the grid (in Fluent), some strange lines across the hex appear in the sections of my volume. it seems meshed with tetrahedral elements in some zones... but if i check the grid there are only hex elements. my problem doesn't reach the convergence , and i think that it's a mesh problem. i think it's a Gambit's bug... did someone find the same bug? or did someone find the solution?

thank you

  Reply With Quote

Old   November 2, 2006, 13:49
Default Re: export prblem with Gambit and Fluent
  #2
Jason
Guest
 
Posts: n/a
I'm assuming that you're creating a surface to display the grid on... is this correct?

The lines you are seeing aren't actual cells. When you create a surface in Fluent and display the grid on that surface, what is displayed is how any cells intersect that suface. Every cell face that intersects your surface will show up on your surface as a line. The extra lines you are seeing are because the cell faces you're cutting through aren't perfectly parallel to the surface you created. Imagine a square face where two of the corners are on your surface. If the other corners are off your surface at all, then you'll see a line that goes between the two corners that are on your surface. If one vertex is on one side and the other three are on the opposite side of your surface, it'll show up as a diagonal line that cuts through at some weird location.

This has nothing to do with the quality of the grid. When Gambit meshes a hex mesh it'll try to smooth the mesh in three dimensions. If the geometry you're meshing is a perfect block (all 90deg corners) then the mesh will be perfectly aligned, but if there's anything in your box, or any other shape to your domain, then the mesh becomes skewed (I know you don't have a perfect block because you mentioned you have skewness <0.4... if you had a perfect block your skewness should've been 0).

You can play around with where you're slicing the mesh to see if you can get a better image, but odds are you won't be able to find a good slice. Gambit has better tools for looking at the mesh though. Use the Examine mesh tool (icon on the bottom right... looks like a yellow grid with a magnifying glass... play around with where you're slicing in gambit and that will show up as a jagged grid in Gambit... this will give you some idea of what I was trying to describe above).

Your problem could still be your mesh, but what you're describing is a problem with how the mesh is displayed, not how the mesh actually is.

Put more details about what you're analyzing, what models you used, compressible/incompressible, inviscid/laminar/turbulent (and if turbulent, what model did you use and what y+ range are you in), solver settings, etc., and someone may be able to help you resolve your problem.

Hope this helps, and good luck, Jason
  Reply With Quote

Old   November 3, 2006, 10:36
Default Re: export prblem with Gambit and Fluent
  #3
Mignolo
Guest
 
Posts: n/a
Thank you Jason for your perfect enlightenment!

then my problem is not a grid problem but a convergence problem... i'm analyzing an heat transfer problem, a semiconfined jet impingement on a plane surface with 4 squared nozzles ( flow in y negative direction), no-aligned, with a periodic condition in z directions and a simmetry condition in x direction. There is 1 exhausted port (flow in y positive direction), like chimney, divided by the simmetry plane. my settings: segregated solver, steady flow, incompressible, turbolent with k-w SST model (as suggested by lots of articles), Simplec (skew =0), first order upwind and standard for pressure. y+ is <1 in the surface with heat transfer and <10 in the others wall. BC: pressur inlet (nozzle), pressure outlet (exhausted port), wall my solution fluctuates too much, ex: for average Nusselt number on the surface is 50 +/- 1. is it normal? i have to reduce my underelaxation factory? or increase them? actually they are a little bit lesser than defaults.. thank you for every suggestion you can give me

Mignolo

  Reply With Quote

Old   November 3, 2006, 11:31
Default Re: export prblem with Gambit and Fluent
  #4
Jason
Guest
 
Posts: n/a
I've never dealt with impinging jets, but it sounds like oscillations in the solution are common. Search the forum for impinging jets to see what other people have done, and if you still can't find a solution, then post your problem with impinging jet in the subject.

Best of luck, Jason
  Reply With Quote

Old   November 26, 2006, 10:08
Default i have problem with mesh in gambit
  #5
fouzia
Guest
 
Posts: n/a
i will mesh a distributor and column on 3D but i cant fond exemple four this case please if you have exemple send me becouse i need it
  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
Converting Fluent mesh files to Gambit neutral files samuelkc ANSYS Meshing & Geometry 5 July 24, 2013 08:02
Export streamlines from Fluent to Gambit Titasse FLUENT 4 April 22, 2010 11:59
Export stramlines from Fluent to Gambit Titasse Main CFD Forum 5 April 22, 2010 11:34
Gambit Fluent export John Go FLUENT 0 March 7, 2009 15:48
Gambit Meshing export to fluent minor problem John c. FLUENT 2 February 6, 2002 17:52


All times are GMT -4. The time now is 05:16.