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

Mesh Generation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 3, 2002, 16:38
Default Mesh Generation
  #1
Dhananjay
Guest
 
Posts: n/a
Hello all,

I am trying to generate a mesh for a fairly complicated 3-D geometry in GAMBIT. However I seem to have a problem with the solution (reversed flow) and need to revise the mesh.

I have a couple of questions about meshing in GAMBIT -

a)Is there any rule of thumb for selecting between unstructrured and structured meshes?

b)Has anyone used the size function option in GAMBIT and found it to be effective?

c)How much skewness is too much skewness?

Thanks and looking forward to your replies.

Dhananjay
  Reply With Quote

Old   May 4, 2002, 01:57
Default Re: Mesh Generation
  #2
heıdarı
Guest
 
Posts: n/a
the response to your thırd questıon ıs ın the gambıt's help,so just read ıt.
  Reply With Quote

Old   May 4, 2002, 05:11
Default Re: Mesh Generation
  #3
Jonas Larsson
Guest
 
Posts: n/a
Unstructured/structured: Use structured meshes whenever possible. In general you will get better accuracy and better convergence with a structured hex-mesh, especially if you can align it with the flow direction fairly well.

Size-function: Haven't tried it yet.

Skewness: Haven't used gambit for some time now but if I remember correctly the "skewness measure" in Gambit should be better than about 0.7 for the grid to work well in FLUENT.
  Reply With Quote

Old   May 6, 2002, 07:53
Default Re: Mesh Generation
  #4
Christian
Guest
 
Posts: n/a
Unstructured/structured mesh: I have heard it before and I have experienced it, but I have never seen a mathematical description of this. Do you have a reference ?

Cheers Christian
  Reply With Quote

Old   May 6, 2002, 08:37
Default Re: Mesh Generation
  #5
Jonas Larsson
Guest
 
Posts: n/a
I can't give you a reference from memory... this has been discussed several times on these forums though. I remember that Hrvoje wrote several nice posts about this. Here is one example from the archives:

http://www.cfd-online.com/Forum/main....cgi?read=7026
  Reply With Quote

Old   May 9, 2002, 10:26
Default Re: Mesh Generation
  #6
Steven Smith
Guest
 
Posts: n/a
Regarding your skewness question, I normally continue working with tet meshes until I get the maximum volume skewness under 0.9 I'm not positive it's necessary, but I do check both equiangle and equisize skewness. Maximum skewnesses less than 0.9 are good, and allow more aggressive use of the relaxation parameters. If your maximum skewnesses is above 0.9, you might have to spend a lot of time babysitting the solver to prevent divergence.
  Reply With Quote

Old   May 14, 2002, 03:38
Default Re: Mesh Generation
  #7
Volker Pawlik
Guest
 
Posts: n/a
Concerning skewness: I observed divergence for grids where one (!) or more cells > 0.97 are found.

So I think even the advice is to avoid cells > 0.9 for tetrahedrals I think the ultimate limit is 0.97 for the fluent solver. Especially if the cell is situated in zones of low (!) massflow, bad skewness helps to fortify gradients and causes numerical diffusion.

  Reply With Quote

Old   May 14, 2002, 08:22
Default Re: Mesh Generation
  #8
Dhananjay
Guest
 
Posts: n/a
Thank you all for your replies!
  Reply With Quote

Old   May 14, 2002, 10:55
Default Re: Mesh Generation
  #9
edvin
Guest
 
Posts: n/a
try to use structed mesh if possible. you can get the same solution with lower number of cells with structed mesh and it is easy to control the mesh.

the unstructed mesh is useful when you have a complex geometry. you can apply it to almost all geometries.

and about skewness: there are several skewness types. look at gambit tutorial.
  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
[ICEM] Generating Mesh for STL Car in Windtunnel Simulation tommymoose ANSYS Meshing & Geometry 48 April 15, 2013 04:24
2D Mesh Generation Tutorial for GMSH aeroslacker Open Source Meshers: Gmsh, Netgen, CGNS, ... 12 January 19, 2012 04:52
[ICEM] Unstructure Meshing Around Imported Plot3D Structured Mesh ICEM kawamatt2 ANSYS Meshing & Geometry 17 December 20, 2011 12:45
mesh generation for in-cylinder fluent simulation hennas ANSYS Meshing & Geometry 2 May 31, 2011 15:08
General questions on grid-based computing Adrin Gharakhani Main CFD Forum 21 June 5, 2000 13:47


All times are GMT -4. The time now is 17:15.