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

Fluent mesh Check error

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

Like Tree2Likes
  • 2 Post By -mAx-

Reply
 
LinkBack Thread Tools Display Modes
Old   August 31, 2011, 02:29
Default Fluent mesh Check error
  #1
Senior Member
 
Mohsin Mukhtar
Join Date: Mar 2010
Location: South Korea
Posts: 249
Rep Power: 8
Mohsin is on a distinguished road
After exporting the mesh in fluent, and checking the mesh i get the following error in fluent:

Velocity inlet zone has two adjacent cell zones.

I have a velocity inlet zone which is inside another fluid zone. That means the velocity-inlet lies on 2 adjacent cell zones.

It seems i have to split my velocity-inlet into 2 Velocity-inlets: one for each zone. How can i do it in FLUENT?
Mohsin is offline   Reply With Quote

Old   August 31, 2011, 02:54
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
Inlet is a boundary condition.
It should have only one adjacent cell's zone.
Delete the volume zone behind your inlet, or redefine the surface for your inlet (the surface must be an "outter" surface)
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   August 31, 2011, 03:04
Default
  #3
Senior Member
 
Mohsin Mukhtar
Join Date: Mar 2010
Location: South Korea
Posts: 249
Rep Power: 8
Mohsin is on a distinguished road
Thank you Max,

I cannot delete the volume behind the boundary. It will alter the geometry. The velocity inlet boundary is inside the main domain. My situation is discussed in these following threads

adjacent cell zones
Grid check failed

in which it is recommended to split the cell zones into 2.

is there any possible way in FLUENT or GAMBIT to split the cell zones so that it recognized as a separtae boundary in FLUENT.

Thanks
Mohsin is offline   Reply With Quote

Old   August 31, 2011, 03:11
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
the last reply on second thread comes from... me
But in this case I thought the BC was applied on a Boundary face

*************
*Zone1**Zone2*
*************
Boundary Surface


But in your case (I saw in your model), you are in this case:
*************
****Zone1****
*************
Boundary Surface
*************
****Zone2****
*************
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   August 31, 2011, 03:23
Default
  #5
Senior Member
 
Mohsin Mukhtar
Join Date: Mar 2010
Location: South Korea
Posts: 249
Rep Power: 8
Mohsin is on a distinguished road
I also was assuming it was u

I have attached a picture. (For now, I deleted the lower bend region from the geomtery which i sent you). In the picture, there is a velocity inlet for air. but this inlet lies in the domain and i cannot move it out of the domain. This inlet causes trouble in FLUENT mesh check. It says it has 2 adjacent cell zones (As it is lying inside). What do u think, how this problem can be resolved?
Attached Images
File Type: jpg MAx.jpg (86.2 KB, 36 views)
Mohsin is offline   Reply With Quote

Old   August 31, 2011, 03:30
Default
  #6
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
ok
copy your inlet surface and translate it in z-direction (very small distance).
Then split the volume containing your old inlet, with the surface you just copied.
Delete the small volume containing your old inlet.
Redefine your inlet on the copied surface, which has now only one adjacent zone (on the other side it is hollow)
Mohsin and mayank199325 like this.
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   August 31, 2011, 04:03
Default
  #7
Senior Member
 
Mohsin Mukhtar
Join Date: Mar 2010
Location: South Korea
Posts: 249
Rep Power: 8
Mohsin is on a distinguished road
Well, that's extraordinary...the issue resolved

Round of applause for u. Thank you very much.
Mohsin 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
Native ParaView Reader Bugs tj22 OpenFOAM Paraview & paraFoam 266 July 1, 2015 02:00
GroovyBC the dynamic cousin of funkySetFields that lives on the suburb of the mesh gschaider OpenFOAM 300 October 29, 2014 19:00
c++ libraries and solver compiling vaina74 OpenFOAM Installation 13 February 3, 2012 18:43
Can Fluent handle a degenerate block? Error while reading mesh... Anorky FLUENT 1 May 1, 2010 12:47
OF 1.6 | Ubuntu 9.10 (64bit) | GLIBCXX_3.4.11 not found piprus OpenFOAM Installation 22 February 25, 2010 14:43


All times are GMT -4. The time now is 02:13.