CFD Online Discussion Forums

CFD Online Discussion Forums (
-   FLUENT (
-   -   VOF (

Béatrice November 27, 2001 12:22

I am using the VOF method geo-reconstruct to compute the impact of a water jet on a wall in 3D. It is an unsteady case, my problem is that the computation converges well during the first twenty or fourty time steps (it depends on the value of the time step). But after, the computation diverges even if I put a time step much smaller than the previous one. Firstly I thought it was because of my grid which had some element with a skewness more then 0.7 but in fact, I have two grids with the same quality of skewness and one is running well but the other not. If someone could help me please!!!

anna November 27, 2001 13:10

-check the quality of your mesh after reading it in Fluent. Better check would be if you do it in Gambit, under Volume/Mesh/Inquiery right mouse button/Check Volume mesh. You'll get a report for each of the volume in your domain. -check if you've enabled gravitation, its direction, as well as reference density in the Operationg conditions panel. PISO for p-v coupling, body force weighted for momentum, and how you are decreasing relaxation factors.

But, first make sure your mesh is high quality mesh, is it uniform in the jet cone area or if its of varying cell size, what is the transition from smaller to larger cells.

regards, anna

Béatrice November 29, 2001 02:11

Thank you for your help. I have checked my two grids, as you told me, and obtained, for the grid which converges, a maximum equiangle skew of 0.6963 and for the other grid 0.6975. I think there is no real difference. For my case I don't take care of the gravity, but i am using PISO for p-v coupling and body force weighted for momentum but I don't modify the relaxation factors. Do you think it 's better to decrease it or not ?

By the way, for the grid, do you know if there is something on gambit or fluent to check the transition from smaller to larger cells ?

sincerely , Bea

anna November 29, 2001 09:41

in Gambit, go to Volume/Mesh/Inquiery,right mouse button click,choose Check, and select all of your volumes. After a little while, you will get in the text editor a report on the volume cells quality for each of them.

Instead of checking for equangle skew, check for Volume quality. So you will click on mesh quality icon, choose, Range and Volume. You should not have as a lower limit any negative number, that would mean you have negative volumes. In case you have them, to see them type in zero for upper limit. If you have them, find a way to divide domain into smaller volumes,create new ones or whatever, just to get better final mesh.

If you want to se the transition of cell sizes, when you click mesh quality icon, choose Plane, and move with mouse tabs on x-, y-, and z-axis. That will show you mesh in crossection planes, and the transition.

Try instead body force weighted, a scheme based on continuity. In Fluent text editor choose solve/set/discretization shemes/pressure, and type 15 and press enter. Before doing this, decrease relaxation factors, for momentum to 0.3, and k-, e- to 0.3. But, first focus on mesh volume quality.


All times are GMT -4. The time now is 13:57.