CFD Online Discussion Forums

CFD Online Discussion Forums (
-   FLUENT (
-   -   Help on VOF boundary conditions (

Kelly August 3, 2007 10:36

Help on VOF boundary conditions

I try to use VOF to model flow through a channel/detention pond with weir as outlet. It's 2 phases:Inlet I air and Inlet II water (air in the top and an initial water depth in the channel before the weir).I am pretty sure about velocity inlet and wall boundary conditions. I wonder what boundary conditions can I apply in the top air portion (pressure outlet?)and weir outlet? I am using Fluent version 6.0.

Thanks for your attention.


msureshkumar August 4, 2007 08:02

Re: Help on VOF boundary conditions
Try with open channel option

Kelly August 4, 2007 19:20

Re: Help on VOF boundary conditions
Dear msureshkumar:

Thank you for your reply. But FLUENT 6.0 doesn't have open chanel option? Do you know any other way?


rafal August 7, 2007 07:22

Re: Help on VOF boundary conditions
Hi kelly, For such a model you can use for both surfaces presure outlets. If the weir outlet is only partialy filled with water you can also try setting the top cover as a wall and weir outlet as a presure outlet. It should help with reversive flow at the cover that will probably apear if you will simutale it with the first option. rafal

Kelly August 7, 2007 10:45

Re: Help on VOF boundary conditions
Thank you for your help, rafal. I tried as you said,however there are "reverse flow and turbulent viscosity limited to viscosity ratio***" warnings even if I extended the domain downstream. Do you have any suggestions to remove this? By the way it is a 2D problem and a broad-crested weir with the same width as channel.

I have one more question to ask about. In setting the initial values,how to determine Gauge pressure and water volume fraction? Are they mean values of the whole domain?


rafal August 7, 2007 11:41

Re: Help on VOF boundary conditions
Hi Kelly.

I am not sure if your problem is a steady or unsteady. As I imagine the problem with computations is caused by the solver connected to not good definition of a problem and i think it will help to try first to define better initial conditions. It would be good to fill the domain with the water to the level of weir top . to do this you have to:

1: adapt a region of a quad shape region/adapt... 2: fill this region with water solve/initialize/patch...

make sure also that operating presure location is where air phase is. At the outflow use the pressure of the operating conditions and before adapting region initialize with setting 'compute from...' and chose outflow.

good luck, rafal.

Kelly August 11, 2007 12:29

Re: Help on VOF boundary conditions

The problem is unsteady.I tried as you suggested:Adapt a region then patch with vof=1; Set the open air as pressure outlet BC. The result seems not right. Most of water run to the Open air domain boundary not to the outlet. Do you know what's the possible reason? Thanks a lot for your help!


rafal August 13, 2007 05:37

Re: Help on VOF boundary conditions
Kelly, It is hard to say without seeing results but there os one possible reason. If the open air domain is above the water (and outlet) check your gravity settings. if the y axis is direcetd up, you should set negative gravity acceleration (wich is not default).


Kelly August 13, 2007 10:16

Re: Help on VOF boundary conditions
Thanks for your great help, Rafal. You are right. I can't believe I made such an obvious mistake!


All times are GMT -4. The time now is 15:12.