CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > ANSYS > FLUENT

Help! mesh error- "only one adjacent cell thread."

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

LinkBack Thread Tools Search this Thread Display Modes
Old   April 6, 2005, 21:29
Default Help! mesh error- "only one adjacent cell thread."
Posts: n/a
When loading a gmabit mesh into fluent i received the error "only one adjacent cell thread" for a group of lines i had defined as 'interior' within gambit. These lines were thence loaded into fluent as "wall" types rather than "internal." They are internal lines (part of the mesh) and cannot be walls.

Does anyone know how to fix this? I'm thinking some walls in gambit need to be altered somehow.
  Reply With Quote

Old   April 7, 2005, 07:51
Default Re: Help! mesh error- "only one adjacent cell thre
Posts: n/a
That's happening because you only have a volume mesh on one side of the wall (or face mesh on one side of the edge in 2D... if you're working in 2D, whenever I say volume, it's a face in 2D, and whenever I say face, it's an edge in 2D). In your model you probably have mesh on both sides, but you did not connect the face so there are actually 2 faces sharing the same space. Since they aren't connected, gambit doesn't recognize the volume mesh on the opposite side. You have two options. The best option is to connect the faces, and you'll probably have to do some remeshing. If the faces are connected, they don't need a BC, gambit will recognize that they are internal, and will write the mesh as being continuous. The other option is to use the interface bc. Name each face (remember there are 2... one on top of the other, so i'll call them faceA and faceB) as its own interface bc, then in Fluent do Define->Grid Interfaces and you can tell it that faceA and faceB are an interface. Fluent claims there is no lose of accuracy when using a grid interface, but intuitively I would say "of course there is".

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

Old   April 14, 2005, 11:56
Default Re: Help! mesh error- "only one adjacent cell thre
Posts: n/a
Set them in gambit as wall,and the in fluent change boundary type.good luck
  Reply With Quote

Old   August 27, 2013, 06:02
New Member
Join Date: Apr 2013
Posts: 7
Rep Power: 11
ferra89 is on a distinguished road
I know it's an old topic but I am in the same condition of Kuba but using ICEM.
How can I do to select and rename a face, as you suggested?

Thank you
ferra89 is offline   Reply With Quote

Old   August 27, 2013, 17:46
Senior Member
A CFD free user's Avatar
A-A Azarafza
Join Date: Jan 2013
Posts: 226
Rep Power: 12
A CFD free user is on a distinguished road
The interior B.C is kind of wall between two fluid zones which let the flow exchange between these two zones directly. In fact, you can consider it "nothing"! Now, this error happens in two conditions: first: one of the zones is not correctly defined as fluid and the second and foremost, the interior face is sort of overlapped with another face. In fact, in this case you have two different faces which lay on each other and you can't distinct them easily. The latter one could be due to an incorrect splitting very often and it's kind of difficult to understand quickly. The solution is to connect the two faces via the corresponding tools embed in mesh modelers.
Hope it helps
Regard yours
A CFD free user is offline   Reply With Quote

Old   October 25, 2016, 11:38
Default Cleanup!
New Member
Join Date: Feb 2016
Posts: 13
Rep Power: 8
Sabomb is on a distinguished road
Ladies and gentlemen, another possible solution is to use the cleanup geometry function. Using this, you may delete duplicate vertices, edges, faces and volumes in order to avoid such conflicts.
Sabomb is offline   Reply With Quote


Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
How many particles can be placed in each mesh cell in each time step? therockyy FLOW-3D 4 September 24, 2012 11:45
[ICEM] Hugh cell jump in Tetra mesh jeevankumarb ANSYS Meshing & Geometry 3 June 2, 2010 11:45
Convergence moving mesh lr103476 OpenFOAM Running, Solving & CFD 30 November 19, 2007 15:09
How to control Minximum mesh space? hung FLUENT 7 April 18, 2005 10:38
unstructured vs. structured grids Frank Muldoon Main CFD Forum 1 January 5, 1999 11:09

All times are GMT -4. The time now is 02:04.