CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Fluent mesh Check error (http://www.cfd-online.com/Forums/fluent/92034-fluent-mesh-check-error.html)

Mohsin August 31, 2011 02:29

Fluent mesh Check error
 
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?

-mAx- August 31, 2011 02:54

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)

Mohsin August 31, 2011 03:04

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

http://www.cfd-online.com/Forums/flu...ell-zones.html
http://www.cfd-online.com/Forums/flu...ck-failed.html

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

-mAx- August 31, 2011 03:11

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****
*************

Mohsin August 31, 2011 03:23

1 Attachment(s)
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?

-mAx- August 31, 2011 03:30

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 August 31, 2011 04:03

Well, that's extraordinary...the issue resolved

Round of applause for u. Thank you very much.


All times are GMT -4. The time now is 01:51.