# VOLUME OF FLUID

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 June 17, 2004, 10:44 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

 June 18, 2004, 02:10 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

 June 18, 2004, 06:52 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.

 June 23, 2004, 04:54 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

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

 June 23, 2004, 11:00 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

 June 28, 2004, 04:43 Re: VOLUME OF FLUID (for all) #7 ataki Guest   Posts: n/a hallo again, any comment, suggestion or information is wellcome. Thanks

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Attesz CFX 7 January 5, 2013 04:32 Giron FloEFD, FloWorks & FloTHERM 4 June 12, 2009 17:05 paean OpenFOAM Running, Solving & CFD 0 November 14, 2008 22:14 bioman66 CFX 5 June 3, 2006 01:40 zahid FLUENT 4 June 1, 2002 09:11

All times are GMT -4. The time now is 06:48.

 Contact Us - CFD Online - Top