CFD Online Logo CFD Online URL
Home > Forums > FLUENT

Interior B.C. Problem

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

Like Tree5Likes
  • 3 Post By Jason
  • 1 Post By Sergevna
  • 1 Post By ershad

LinkBack Thread Tools Display Modes
Old   July 9, 2005, 04:46
Default Interior B.C. Problem
Samaneh Zeighami
Posts: n/a
I have created a 3-D mesh in gambit with the "interior" B.C. When I read it in FLUENT, I receive this error message:

"Cannot change i7 to interior because there is only one adjacent cell thread."

i7 is the name of the interior B.C..

Can you please guide me through this?
  Reply With Quote

Old   July 10, 2005, 11:37
Default Re: Interior B.C. Problem
Posts: n/a
Hi; You may set an outer boundary as interior. I recomend you that in a B.C. setting, at first don't set interior boundaries. But at first set all B.C.s like velocity or pressure etc. Then choose all faces and set them as interior. Gambit does not set interior condition to faces those other conditions set to them at perior. Therefore you will not encounter to a wrong interior B.C. setting. Hope this help you. ROOZBEH
  Reply With Quote

Old   July 11, 2005, 08:33
Default Re: Interior B.C. Problem
Posts: n/a
That error occurs because there is only a volume mesh on one side of the face (that's what the "one adjacent cell thread" means). An interior BC is similar to creating a plane within Fluent... it doesn't affect the flow... flow passes in one side, and out the other without any changes occuring to it. There are two possibilities here... first, you could be using this at the edge of your control volume... this doesn't work, because there's obviously no mesh on the otherside of the BC. You need to switch this to symmetry, wall, some type of inlet or outlet.

The other possibility is that you have two volumes next to one another, and you're trying to tell let the flow pass from one volume to the next. The problem is, these two faces don't share a common face. If this is the case, you have two options. The one I recommend is using the connect function in Gambit so that those two faces (one for each volume) become one within Gambit. This is also what you have to do to create a continuous mesh. Otherwise you have two faces, so two different meshes. You'll have to remesh one of your volumes, but you won't have to assign any BC to it when you export your mesh... Gambit will consider this an interior surface and will ignore it, so that when you import it into Fluent, you have one continuous mesh. You can assign it an interior BC if you wish. These are good for post-processing, or if you think you're going to change it to a pressure drop or something later, but that's about it. The other option is a non-conformal mesh interface. Assign an "interface" BC to each face (they'll each have to have different names). Then in Fluent, under Define->Grid Interfaces you pick the two faces and then click "Create"... don't turn on Periodic or Coupled. This is an easy way to create mesh transitions. Also, it's good if you want to be able to easily switch a specific volume in and out (say you have different components to try... if you have a separate volume with that component, it's easy to delete the volume and create a new volume in its place with the new component). You increase the round-off error at the interface, but if it's far enough away from the area of interest, it's not a big deal.

Hope this helps, and good luck, Jason
mcermak, elisun and harsh_999 like this.
  Reply With Quote

Old   May 22, 2012, 13:32
Default boundary condition
New Member
Ershad Amini
Join Date: May 2012
Location: Tehran
Posts: 9
Rep Power: 7
ershad is on a distinguished road
I am simulating a membrane bio-reactor. My reactor has 2 main volumes (Attached file). I subtracted smaller volume from the other, but I retained the subtracted volume.
I have defined 3 boundary conditions as follow:

1. Velocity Inlet (flow of air) : the lower face of smaller volume
2. Pressure outlet: the upper face of bigger volume: it is open to atmosphere.
3. ???I don't know how to define the boundary condition of the upper face of smaller volume. In reality the smaller volume is open from top and the air rise up in the smaller volume and goes out from top of it and enters the bigger volume, At initial, the reactor is full of water and its volume fraction is 1.
I have tried some boundary conditions for the upper face of smaller volume(face2), but I encountered ERRORS as follow:

1. OUTFLOW: "Warning both outflow and and pressure boundaries are present in the domain. This is an incompatibility and solution cannot proceed until this is fixed."

2. INTERIOR: "Error: Cannot change face2 to interior because there is only one adjacent cell thread."

"Error: Cannot change face2 to interior because there is only one adjacent cell thread."

What can I define the boundary condition of that face?
Sincerely yours,
Attached Images
File Type: jpg mbr.jpg (29.2 KB, 28 views)
ershad is offline   Reply With Quote

Old   July 3, 2012, 21:20
New Member
Anna Nasonova
Join Date: Jul 2012
Posts: 1
Rep Power: 0
Sergevna is on a distinguished road
Hello, ershad

I have exactly the same problem. I just wonder if you found the solution. I used Jasons comments and model works without any error messages, but flow doesn't go through this "interface" face. I would be very greatful if you answer.

Best regards
ershad likes this.
Sergevna is offline   Reply With Quote

Old   July 5, 2012, 14:56
Default Gambit, Interior
New Member
Ershad Amini
Join Date: May 2012
Location: Tehran
Posts: 9
Rep Power: 7
ershad is on a distinguished road
Hi, Anna
My reactor has 2 main volumes (Attached file), smaller volume (Module, Volume1) with 20 membranes and the bigger volume (total rector, Volume2) which contains module. I assumed the 20 membranes as solid volumes, not porous media because I just want to investigate the hydrodynamic in the reactor (tension on the membrane surface and velocity and gas holdup in the reactor). My reactor has 5 spargers (rectangular) at the bottom of the bigger volume (the lowest face). In Gambit I split the smaller volume (Module, Volume1) with the bigger volume (total rector, Volume2) and then subtracted the 20 membranes from the smaller volume (Module, Volume1) and I did not retain the 20 membranes, finally I had 2 volumes. The smaller volume (Module with 20 membranes, Volume1) is hollow and is open from bottom and top. The air from spargers enters the smaller volume from bottom and goes out from top of it and circulates through the reactor. I defined the low and top faces of the smaller volume (Module, Volume1) as “Interior” boundary condition, the spargers as “Velocity Inlet” and the upper face of the bigger volume (total reactor, Volume2) as “Pressure Outlet”. Number of meshes of my reactor is about 3,000,000. I use a supercomputer with 24 cores for my simulation. The distance between membranes is 8mm and the dimensions of my reactor are as follow: Smaller volume (volume1): 330mm * 1170mm * 240mm(x,y,z) Membranes (20 Membranes): 300mm * 1000mm * 2mm(x,y,z) Bigger volume (Volume2): 600mm * 1650mm * 600mm(x,y,z) For meshing the interval size of module (Volume1) is 6mm and for the rest of the reactor (Volume2) I chose a 60mm interval size. (Mesh type: Tetrahedral, TGrid). Sincerely yours, Ershad.
Attached Images
File Type: jpg MBR.JPG (34.7 KB, 14 views)
zaynah04 likes this.
ershad is offline   Reply With Quote

Old   September 8, 2012, 05:06
Senior Member
zaynah K.
Join Date: Jun 2012
Location: Mauritius
Posts: 138
Rep Power: 7
zaynah04 is on a distinguished road
Hi Anna
I also have same problem as yours
I would be very grateful if you can share how to solved that problem.

zaynah04 is offline   Reply With Quote


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
UDF compiling problem Wouter Fluent UDF and Scheme Programming 6 June 6, 2012 04:43
Gambit - meshing over airfoil wrapping (?) problem JFDC FLUENT 1 July 11, 2011 05:59
natural convection problem for a CHT problem Se-Hee CFX 2 June 10, 2007 06:29
Adiabatic and Rotating wall (Convection problem) ParodDav CFX 5 April 29, 2007 19:13
Is this problem well posed? Thomas P. Abraham Main CFD Forum 5 September 8, 1999 14:52

All times are GMT -4. The time now is 06:30.