CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   FLUENT (https://www.cfd-online.com/Forums/fluent/)
-   -   Free surface of Step with VOF (https://www.cfd-online.com/Forums/fluent/33714-free-surface-step-vof.html)

 Azin Sharafeddin May 12, 2004 12:43

Free surface of Step with VOF

My question is:

I want to find free surface profile of a flow over a step with VOF method. How should I define my boundary conditions? Which part are phjase-1 & which phase-2 & mixture too. How should I mesh it in Gambit?

If it was in a under pressure condition I could do it, but with free surface I can't! Thanks for your help!

 akbar safarzadeh May 26, 2004 05:24

Re: Free surface of Step with VOF

Dear my friend

I'm working with vof model of fluent for 2 phase problems in hydraulic engineering.

if you want to find the free surface over a step, do this steps:

1- in the gambit, define all the domain as a single blocK (there is no need to separete the air and water parts). 2- set the pressure outlet boundary condition for the top of your domain B.C. 3- in the fluent define the water from material option. 4- go to define-> modules-> multiphase-vof. 5- if you are working with version 6. go to define->phases. and set the water as the material of phase 2. 6- adapt a region that covers the inlet depth. (go to: adapt->region-> enter the min and max cordinates of the part that at t=0 sec you want to be filled with water (vof=1)). 7- go to : grid-separate-face---- mark. then separate the inlet of your domain with the adapted region to 2 parts. one of these parts is the constant depth of water at the inlet and the other is the part that it's vof eqales 0 (air part). (the new boundary named inlet:019 (for example) is the water part.) 8- in B.C option set the velocity inlet for water part and for the air part give a small velocity compared with water vel. click on the new boundary and at the bottum set phase 2 and set vof=1 for this B.C. 9- go to initalize and initalize all zonez. 10- patch the vof=1 for adapted domain. 11- go to iterate and set dt=0.01 and then run the program.

I hope this helps you. if you have another question please write to me.