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

link mesh

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 14, 2006, 08:04
Default link mesh
  #1
Ana Raquel Rosado
Guest
 
Posts: n/a
I everyone!

here goes my problem: I have two diferent mesh, which I would like to link, but when I try to do it, gambit gives me a error message saying that lower topoligies canīt be link! Does anyone knows how can I resolve this problem???

Thanks
  Reply With Quote

Old   November 14, 2006, 09:34
Default Re: link mesh
  #2
Jason
Guest
 
Posts: n/a
Ok... linking is not used for connecting two different meshes. Linking is a way of telling Gambit that two edges/faces/volumes are similar and should have matching meshes (i.e. for a periodic BC, so that both faces match up node-to-node). If you're trying to link two faces, those faces have to have the same exact number of edges and vertices.

Connecting is taking two different volumes and making them share a common face. The problem with connecting volumes is that if the common faces have slightly different meshes, then one of the volume meshes will end up being deleted. Also, the common faces have to be identical (same number of edges and vertices, and these edges and vertices need to line up with their matching counterparts within Gambit's tolerance of 1e-06).

If you have two volumes which have different meshes, and you want them to be "connected" but you don't want to lose the mesh, then use the interface BC on each of the common faces and then in Fluent go to Define->Grid Interfaces and tell Fluent that you want those interfaces to be connected.

Hope this helps, and good luck, Jason

  Reply With Quote

Old   November 15, 2006, 07:51
Default Re: link mesh
  #3
Ana Raquel Rosado
Guest
 
Posts: n/a
thanks jason,

in fact your answer is helpful, but I have to say that I am new with fluent. so could you tell me how can I define de common faces of the volumes as "interface BC".

best regards Raquel
  Reply With Quote

Old   November 15, 2006, 08:52
Default Re: link mesh
  #4
Jason
Guest
 
Posts: n/a
You should define the type of BCs in Gambit. In Gambit make sure "Fluent 5/6" is selected under solver. Then go into the Boundary Conditions tool (it's one of the buttons at the top right of the Gambit window... looks like a cube with one face highlighted Blue) and define all of your BCs there. "Interface" is one of the available BCs.

Each of the faces that you want to be "interfaced" should have their own Interface BC... that way when you import the geometry into Fluent, you can go to Define->Grid Interfaces and pick those two "interfaces" and make them one common BC.

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

Old   November 15, 2006, 11:32
Default Re: link mesh
  #5
Ana Raquel Rosado
Guest
 
Posts: n/a
once again I apreciate your help, jason

I have done what you advice, but the problem is that after I connected interfaces, the first ones don't disapered and I can't change the boundary condition on the new one. I am traying to connect two almost identical volumes. they have one common face and four common edges. I would like to connect the common faces and connect the faces which the edges are common.can I do that?

thanks

Raquel
  Reply With Quote

Old   November 15, 2006, 12:32
Default Re: link mesh
  #6
Jason
Guest
 
Posts: n/a
The interface is what's called a non-conformal interface... it allows flow the pass from one side of the interface to the other, but does not require the two sides of the interface to have identical meshes. They'll remain two separate BCs within Fluent, but flow will be able to pass without a problem. This is good if both volumes have a complicated mesh and you don't want to re-mesh one of them, or if you have different mesh types in the volumes (i.e. one is a tet mesh and one is a quad mesh).

Instead, if you don't have the volumes meshed yet, or if you don't mind re-meshing one of them, then you can connect the common face. In the face tools, it looks like a black plug. The two faces you are trying to combine have to have the same number of vertices and edges, and these vertices and edges must align within Gambit's tolerance (1e-06). Now instead of two faces in the same space, there will be only one face. Don't apply any BC to the connected face and Gambit will simply ignore the face when it's writing the mesh file and you will get one continuous volume.

I was under the impression from your first post that the volumes were already meshed and that you were trying to do this without having to re-mesh one of the volumes, which is why I recommended the Interface BCs. If this isn't the case, then by all means connect the common face using the connect tool.

Hope this helps, Jason
  Reply With Quote

Old   November 15, 2006, 13:07
Default Re: link mesh
  #7
Ana Raquel Rosado
Guest
 
Posts: n/a
Thanks Jason,

in fact you are not mistaken,I have already the two volumes meshed, but I don't mind to re-mesh it. here goes my inicial problem: I wanted to mesh a paving stone with the following messures: 100; 350 ;800 meter (x;y;z). And in side I have smaller cubics which messures: 20;20;40 meters. From the volume of paving stone, I subtract the other volumes. Then I try to aply a volumic mesh to what is left of the pavins stone volume, but gambit says that it is not possible because mesh sizes is to large in areas of small gaps. I have tried every that I know to fix this problem, but with no result. That was why I decided to slip de paving stone volume in two and then aply to each one a volumic mesh. I don't know if this can result, but if you have other sugestions, I appreciate.

once again, I thank you for all other sugestion and I hope you can help me with this problem.

Best regards

Raquel
  Reply With Quote

Old   November 20, 2006, 08:09
Default Re: link mesh
  #8
Ana Raquel Rosado
Guest
 
Posts: n/a
Hi everyone, I have solved my initial problem. In fact it was simple; I just needed to transform my geometry in to a virtual geometry. This way I can adjust the mesh with no problem.

Thanks for everything

  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] Negative volume error in hybrid mesh siw ANSYS Meshing & Geometry 4 September 3, 2014 05:25
2D Mesh Generation Tutorial for GMSH aeroslacker Open Source Meshers: Gmsh, Netgen, CGNS, ... 12 January 19, 2012 04:52
non-smooth mesh Svensson OpenFOAM Native Meshers: snappyHexMesh and Others 11 January 18, 2012 10:13
2d irregular grid Remy Main CFD Forum 1 December 22, 2008 05:49
Face link mesh Frederick FLUENT 1 March 14, 2007 12:15


All times are GMT -4. The time now is 05:21.