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

VOLUME OF FLUID

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 17, 2004, 10:44
Default VOLUME OF FLUID
  #1
Nial Horton
Guest
 
Posts: n/a
Dear friend, I am investigating the use of the Volume of fluid method for the simulation of the free surface of flow in a shallow open channel. I have been able to seperate the vel. inlet into two parts to give myself an initial air inlet and then a water inlet at the bottom and am using the PISO function so that the under relaxation factors can be set to one. However, I am having great difficulty in gettin my solution to converge and have found that I am not sure what time step settings to enter.

In this way, any advice or hints that you could give would be greatly appreciated.

Thanks
  Reply With Quote

Old   June 18, 2004, 02:10
Default Re: VOLUME OF FLUID
  #2
Markus
Guest
 
Posts: n/a
Hi Nial, Unfortunately Fluent uses an explicit time discretization for the advection of the volume fraction equation. This means that the stability of your solution is mainly determined by the Courant-Number of your problem, i.e. by velocity*timestep/gridspacing. If this number exceeds 1 the algorithm becomes unstable, for practical applications the limit is even lower: ~ 0.5. So usually you will have to use very small timesteps. Hope this helps, there are some remarks in the fluent documentation about this topic too. markus
  Reply With Quote

Old   June 18, 2004, 06:52
Default Re: VOLUME OF FLUID
  #3
Ron
Guest
 
Posts: n/a
Use following command in text mode-

(rpsetvar 'md/verbosity 2)

and check the VOF subtimestep should not b more than 4 . If they heigher then reduce the timestep.

Hope this help.

  Reply With Quote

Old   June 23, 2004, 04:54
Default Re: VOLUME OF FLUID (for all)
  #4
ataki@rhrk.uni-kl.de
Guest
 
Posts: n/a
hallo, I am working with VOF model and I get some solutions for wetting of a complex geometry. The folloing suggestions are worthfull:

* mean Cell size 0.2^3 mm to 0.5^3 mm * initial the solution only with 0 values for all variables (also VOF) * use the ddp (double presision version) * body forces weighted, simple and first order upwind for the descritizations: * Geo-reconstruct and Courant No. 0.25, activate solve vof every iteration and implicit body forces. * Multigrid controls, pressure, termination 0.001 instead of 0.1 * hexaherdral cells * reorder domain multitimes and zones one time * time step 0.00005 to 0.00001 * 10 iterations per step and 0.005 residuals for the comtinuity at first then change to 0.0002.

I hope that will help you and good luck

Ataki

  Reply With Quote

Old   June 23, 2004, 08:23
Default Re: VOLUME OF FLUID (for all)
  #5
Podila
Guest
 
Posts: n/a
Are u using a coupled Solver ?
  Reply With Quote

Old   June 23, 2004, 11:00
Default Re: VOLUME OF FLUID (for all)
  #6
Ataki
Guest
 
Posts: n/a
hi I am using the VOF for tracking the interface between two phase (free flow). It is segregated solver. The coupled solver is not combatible with this multiphase flow model in Fluent. Best wishes Ataki
  Reply With Quote

Old   June 28, 2004, 04:43
Default Re: VOLUME OF FLUID (for all)
  #7
ataki
Guest
 
Posts: n/a
hallo again, any comment, suggestion or information is wellcome. Thanks
  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
Water subcooled boiling Attesz CFX 7 January 5, 2013 04:32
There is no fluid volume in the project Giron FloEFD, FloWorks & FloTHERM 4 June 12, 2009 17:05
On the damBreak4phaseFine cases paean OpenFOAM Running, Solving & CFD 0 November 14, 2008 22:14
How to apply negtive pressure to outlet bioman66 CFX 5 June 3, 2006 01:40
fluid hot volume in fluid cold volume zahid FLUENT 4 June 1, 2002 09:11


All times are GMT -4. The time now is 18:40.