CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [GAMBIT] Grid check failed (

CFDST November 30, 2012 12:10

Grid check failed

I'm simulating a Ventilation system in cinema hall, I made the model in gambit,meshed it and when I exported it into Fluent and click grid>check it failed, and it says Error: outflow zone 10 has two adjacent cell zones??? Can I continue the simulation if grid check failed? Is there any chances to get solution converged? Thank you.

-mAx- December 3, 2012 02:55

2 adjacents zones means that your outflow isn't an extremity of your domain (the boundary face (2d) has a cell (3d) on one side of its face, and another one at the other side which isn't correct

CFDST December 3, 2012 16:54

Thank you for the reply Max. It really helps because I made the stairs in the middle of the hall with the outlets on them and splited the volume, but under the stairs there is still volume,which is the real situation, but I understand that the stairs with the outlets should be splited with the volume so that they will be the external boundary of the volume am I right?, the volume under the stairs should be cut or?

-mAx- December 4, 2012 02:56

can you post a picture of your model and explain where are your BC

CFDST December 4, 2012 04:26

Thank you a lot Max.I have a project at the university and I'm seriously running out of time. My model is a cinema hall and I have to make the simulation of ventilation system. My outlets are at the bottom of the hall on the stairs. My Inlets are at the top - 30 jet noozles and about 42 air diffusers at the lower top and 4 air diffusers in front of the hall. First I made the model in Autocad and exported it into Gambit,set all the outlets,inlets and walls as boundary conditions,the volume as fluid,meshed the model,but when I exported it into Fluent and set all the settings(grid check,models,solver,viscous,residiual, etc.) I started to make Iterations but after about 3000 iterations my flow from the noozles was going under the wall and nothing was going inside the volume. My professor told me to make the model into Gambit,so I started to doing it vertex by vertex with coordinations from Autocad. I made it but my FIRST MODEL was really hard to be meshed, First I meshed the faces with the outlets and inlets,after meshing them,I started to mesh the volume and it says an Error:Segmentation violation cannot mesh the volume,this is because the foreheads of the stairs are too small and the program cannot mesh them I think. So I made a SECOND MODEL with horizontal stairs and angled foreheads, I meshed it exported into fluent and when I made grid check it failed and says Error: There are two adjacent cell zones in Outflow xxx zones. I continue with fluent set all my boundary conditions,residuals,solver,visous and start to make Iterations after 1000 iterations every time it says "reversed flow in xxx outlets", I change the outlets with pressure outlets and it says again the same. When I looked at the velocity in the hall with patlines or vectors to be computed it was about 10000 m/s , the Temperature was 10000 K :D:D and as long as I was continuing the iterations I understand that the velocity and temp rise. So I understand from you that my outlets should be at the extennal boundary of the volume and I made a "THIRD MODEL" with all the outlets at the botom without stairs and it works perfect the velocity was perfect,the temperature the same, but I need my outlets to be at stairs and their place to rise in height. So my question is :1. I have a completely empty hall " FOURTH MODEL",only the outside walls and the roof and floor I have to make the stairs as a second volume and split this volume with the Hall volume,so that my stairs will be the external boundary for the hall and put the outlets on them so that they will have only one zone from where the air is going to be exhaust or ?

CFDST December 4, 2012 04:27


CFDST December 4, 2012 04:38
Links for gambit- models

-mAx- December 4, 2012 04:58

4 Attachment(s)
yep the problem is that you modelised the stand as a baffle (no thickness), and of course the flow may go under the stand (and under your outlet)
So you need to extrude (sweep) the outer edges from your stand in z-direction (bottom), and split the volume with all generated surfaces.
Then you delete the volume which describes the bottom of your stand, and that's it.
And don't forget to split your volume with blue surfaces, else those one don't belong to the volume.
Attachment 17440 Attachment 17439Attachment 17437Attachment 17438

CFDST December 4, 2012 05:26

Thank's you a lot max I'm completely new to Gambit,so I cannot sweep the edges. First I have to go to face>sweep edges> and then how to sweep all the edges to the botom from where,because they are going all together with the same length.How to sweep them to the bottom?

-mAx- December 4, 2012 05:33

what you did is correct, you only need to sweep deeper (alle the blue surfaces have to finish out from the volume, else the split won't be successfull since it won't cut eh volume into 2 volumes)

CFDST December 4, 2012 05:35

I got it thank you.Now I'm spliting it.

CFDST December 4, 2012 05:43

Thanks I made it,but when I tried to mesh the volume there is my favourite error Initilization failed, perturb boundary condition......

CFDST December 4, 2012 05:49

I have to remake the stairs? Because I think the problem is there. Can you give an advice how to make them, because when i make them angled without any horizontal stairs, I cannot connect the outlets to the angled stairs

CFDST December 4, 2012 05:54 I meshed the faces wit Tri-Pave - 0,6 not 1 as it shows at the picture.

-mAx- December 4, 2012 06:07

you need at least 8-10 cells in your outlet disks...
so you will need to work with size fonctions
And for sure you will need to decompose you voluem for having a better control of your mesh.
The initialization failed story is due to the poor mesh on one surface: and for sure it is on your small outlets and/or inlets

CFDST December 11, 2012 04:13

Thank you a lot mAx. Finally I splited the volume and meshed it. Now the problem is in fluent.I made about 2100 iterations and still cannot get solution is converged.My professor told me that I have to get it after about 400-600 iterations.The simulation is of a ventilation system.
Velocity of the inlets 2 m/s, 2.3 m/s and 1.4 m/s . My outlets are otuflows wtih flow rating - 1. I set K-e viscous method with RNG. Flow,turbulence and energy equations, the discretization of momentum,turbulence kinetic energy,energy,dissipation rate and energy are second order upwind. I cannot figure out where is the problem, may be :
1.More iterations need
2.I change the steps of the pathlines and it shows a lot more pathlines.
3.I made a sweep surface at the stairs z=2.13 and the velocity is still low.
Thank you in advance for your help.

CFDST December 11, 2012 04:14

-mAx- December 11, 2012 07:06


Originally Posted by CFDST (Post 396839)
My outlets are otuflows wtih flow rating - 1.

Try to switch to pressure outlet with 0 Pa

CFDST December 11, 2012 10:44


Originally Posted by -mAx- (Post 396879)
Try to switch to pressure outlet with 0 Pa

Thank you I'll try it.

All times are GMT -4. The time now is 04:52.