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

Interior/internal face

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 9, 2005, 17:14
Default Interior/internal face
  #1
Mattis Voss
Guest
 
Posts: n/a
I am modelling a turbine blade in a flow. I have created a nice structured mesh around the blade itself, and a triangular paved mesh that covers the rest of the problem. To do this, I subtracted the face that the structured mesh is on from the surrounding face. My problem now is that when I run this in fluent, it sees the boundary between the structured and the unstructured mesh as a wall. I have tried changing the relevant edges to interior, interface and internal, but it just won't let me. Any ideas on what I'm doing wrong?
  Reply With Quote

Old   November 10, 2005, 09:55
Default Re: Interior/internal face
  #2
Jason
Guest
 
Posts: n/a
You talk about faces, so I'm assuming its a 2D model. The problem is that the two faces aren't connected. When you subtract one face from another, now there are two edges where the faces touch. The edges are at the same exact location, but its two separate edges (one for each face). Since the edges aren't connected, there are two sets of nodes, and two sets of elements, and Gambit and Fluent have no way of knowing they are supposed to be attached (you can use the interface option in Fluent... I'll describe that one later). You should have used a split command with the "connected" option turned on. When you do this, only one edge is created, and both faces will share this edge. Since both faces share this edge, the nodes and elements along this edge will be shared when meshing both faces. Since the mesh is now continuous, no BC is needed on this edge, and Gambit will recognize that it's a continuous mesh when it writes the *.msh file. You can go back to Gambit and manually connect the edges. In the face commands, it's on the first row of icons, second from the right... looks like a black plug being plugged-in. In that command, you select the two edges and it will connect them. You might have to fix your mesh after you do this. The other option is using the interface BCs. You have to assign the interface BC on both edges in Gambit. Then in Fluent go to Define->Grid Interfaces and tell Fluent that those two interface BCs are to be one single interface. This introduces a little more error, but if it's not in a high gradient region and as long as there isn't a big change in cell size across the interface, the error should be negligible.

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

Old   November 10, 2005, 09:57
Default Re: Interior/internal face
  #3
Jason
Guest
 
Posts: n/a
Oh, I meant to mention that all of that works in 3D as well. Just instead of edges being connected, you need edges AND faces connected. There is a connect face option in the face commands that will automatically connect nodes, edges, then faces for you (Gambit always works from the lowest order up... so when you tell it to connect edges, in the background it will connect the nodes first, then the edges). The interfaces also work in 3D.

Jason
  Reply With Quote

Old   November 10, 2005, 16:53
Default Re: Interior/internal face
  #4
Mattis Voss
Guest
 
Posts: n/a
Brilliant, just got my first converged solution. Thank you so much!
  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
Import netgen mesh to OpenFOAM hsieh Open Source Meshers: Gmsh, Netgen, CGNS, ... 32 September 13, 2011 05:50
BlockMeshmergePatchPairs hjasak OpenFOAM Native Meshers: blockMesh 11 August 15, 2008 07:36
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
Axisymmetrical mesh Rasmus Gjesing (Gjesing) OpenFOAM Native Meshers: blockMesh 10 April 2, 2007 14:00
Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15


All times are GMT -4. The time now is 21:14.