CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[GAMBIT] Meshing in GAMBIT (non symmetrical geometry)

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 2, 2011, 12:16
Post Meshing in GAMBIT (non symmetrical geometry)
  #1
New Member
 
Join Date: Sep 2011
Posts: 6
Rep Power: 5
sbrCFD is on a distinguished road
I am new to GAMBIT and I am working on a project that involves a lake. As a first attempt I have considered it as a big pool with some inlets and outlets (inflows/outflows). I have generated the geometry considering some points and then, I build some edges to form the pool. Moreover I have also considered some “holes” from which inlets and outlets are going to go in and out. The final geometry is not symmetrical. I have meshed the edges and finally, I intended to mesh the volume (I have considered one volume only). However, the volume mesh could not be done because une of the faces could not be meshed succesfully (according GAMBIT has told me).
Could anyone tell me the best way to deal with this kind of problem? Would it be better to consider several volumes (i.e., to divide the “pool” in diferent sections)? Should I have the same number of nodes in the parallel faces of the “pool”?
I will appreciate very much your help. Thanks!
Bel.
sbrCFD is offline   Reply With Quote

Old   November 3, 2011, 01:46
Default
  #2
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,964
Rep Power: 30
-mAx- will become famous soon enough
Gambit is giving to you an info that it could not mesh one surface.
But it also gives you the surface id.
So you can try to check this surface and you will see where is the problem.
Then if you can either try to mesh your volume on the fly, or split your domain into several subdomains as you mentionned.
If you need more help, don't hesitate to post pictures
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   November 3, 2011, 11:42
Post Meshing in GAMBIT (2)
  #3
New Member
 
Join Date: Sep 2011
Posts: 6
Rep Power: 5
sbrCFD is on a distinguished road
I have decided to split the domain in several subdomains (volumes). Then, I have tried to mesh one of the volumes (specifically volume 2), and an error has appeared with “face.16”. The error message was “Bad interval assignment for submapping face.16”. I do not know how to manage this error. Would it be necessary to have the same geometrical forms on the opposite faces of the volume (face.16 and face.9 in this case)?
I am also posting a file (please let me know if you are unable to open it).
Many thanks for you help.
Bel.
Attached Files
File Type: zip 2_Nov_2011.zip (83.2 KB, 36 views)
sbrCFD is offline   Reply With Quote

Old   November 4, 2011, 02:20
Default
  #4
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,964
Rep Power: 30
-mAx- will become famous soon enough
*delete all your volume meshes
*mesh surface 16
*check that edges 41 & 38 (also 46 & 43) have same nodes-counter
*mesh surface 8 and 17 (will fail if edges 41 & 38 - 46 & 43 don't have same nodes-counter)
*mesh surface 15
*mesh volume 2
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   November 4, 2011, 15:10
Thumbs up
  #5
New Member
 
Join Date: Sep 2011
Posts: 6
Rep Power: 5
sbrCFD is on a distinguished road
Many thanks mAx. I was able to mesh the faces and the complete volume. I will try to improve the mesh now.
Bel.
sbrCFD is offline   Reply With Quote

Old   November 7, 2011, 10:28
Post More about meshing a non-symmetrical geometry (strategy)
  #6
New Member
 
Join Date: Sep 2011
Posts: 6
Rep Power: 5
sbrCFD is on a distinguished road
Hi,
I could mesh the geometry with the strategy previously proposed by mAx. However, the mesh it too fine in some subdomains (as in volume 2), or more than I would like. I would like to have a “uniform” mesh pattern. I think that a uniform mesh pattern will allow me to solve the problem properly, obviously, with a finer mesh on the vicinity of the inflows/outflows of the geometry. I could mesh the complete geometry with the same pattern as volume 2 but I will obtain a geometry with too much nodes.
With that purpose in mind, I have created several volumes, then I meshed all the edges (with a finer pattern on the vicinity of the inflows/outflows of the geometry), and finally I tried to mesh each volume. As you can see from my previous posts, this strategy did not allow me to mesh one of the volumes (volume 2).
Could anyone tell me a “smarter or proper” strategy to achive my objective? I am not sure about how fine/sparse the mesh should be , but then I would like to refine the mesh. Do you think that having a geometry with such different dimensions between the “pool” and the inflows/outflows dimensions wouls oblige me to refine the full mesh to have a proper solution of the problem?
Many thanks for your help.
sbrCFD is offline   Reply With Quote

Old   November 8, 2011, 02:46
Default
  #7
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,964
Rep Power: 30
-mAx- will become famous soon enough
You have a thin structure.
At least you need 8-10 cells in the depth (more if you treat it with a Boundary Layer).
This is your "pre-dominant" factor, and you cannot avoid it.
So you can "play" with the other directions to stretch your cells, but not to much, else you will have aspect-ratio issues.
Do you have any symmetry in your model? If yes use it (-them) to reduce your domain
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   November 11, 2011, 14:01
Default
  #8
New Member
 
Join Date: Sep 2011
Posts: 6
Rep Power: 5
sbrCFD is on a distinguished road
Many thanks for your answer mAx!
Bel.
sbrCFD is offline   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
Problem meshing an imported geometry Alicia Open Source Meshers: Gmsh, Netgen, CGNS, ... 0 March 30, 2010 04:53
Gambit: too long meshing time! delsolman FLUENT 1 January 29, 2008 20:06
Meshing problem in GAMBIT Vidya Raja FLUENT 0 May 20, 2006 23:31
Meshing the geometry Vidya Raja FLUENT 0 February 26, 2006 20:44
Creating a Geometry in GAMBIT Sridhar FLUENT 2 November 26, 2001 11:11


All times are GMT -4. The time now is 23:56.