CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

VOF

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   November 27, 2001, 11:22
Default VOF
  #1
Béatrice
Guest
 
Posts: n/a
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!!!
  Reply With Quote

Old   November 27, 2001, 12:10
Default Re: VOF
  #2
anna
Guest
 
Posts: n/a
-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

  Reply With Quote

Old   November 29, 2001, 01:11
Default Re: VOF
  #3
Béatrice
Guest
 
Posts: n/a
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
  Reply With Quote

Old   November 29, 2001, 08:41
Default Re: VOF
  #4
anna
Guest
 
Posts: n/a
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.

anna
  Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
VOF Inlet condition Rizwan FLUENT 13 May 29, 2011 16:01
Question:Considerations about the evaporation in VOF dokeun FLUENT 10 February 24, 2011 20:47
vof + hydrostatic pressure ariorus FLUENT 0 August 7, 2009 10:57
urgent query regarding vof model plz rply Garima Chaudhary FLUENT 0 July 13, 2007 02:20
Difficult BCs about Freesurface Simulation by VOF Yongguang Cheng FLUENT 0 September 19, 2003 07:39


All times are GMT -4. The time now is 14:16.