# Volume of Fluid help please!

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

 January 19, 2008, 09:17 Volume of Fluid help please! #1 Gareth Uglow Guest   Posts: n/a Hi, I'm fairly new to CFD, but have embarked on a university project so I'm having to take things on trust rather than develop a full understanding behind the theory, so I'd really appreciate so help, in laymans terms! I'm trying to model a free surface (water:air) flow in an open channel, over a cylinder. I'm using Volume of Fluid. Dimensions are of the order 1m, and flow rate approx 1m/s. The boundary conditions are: velocity inlet, pressure outlet, walls top and bottom and initial volume fraction 0.5:0.5. time step 0.01s (and also 0.001s) and 200 iterations per timestep. Residuals converge after about 100 iterations. The problems I've encountered are wierd reflecting waves off the rear boundary, and, more importantly, a very dissipative water-air interface. The distance between pure air and pure water is about 0.4m, whereas I had expected it to be just one element width. Any suggestions?

 January 19, 2008, 15:53 Re: Volume of Fluid help please! #2 bohis Guest   Posts: n/a 200 it per time step? I have never needed such a number. It is to much. Better to decrease timestep.By the way, sorry, but I didnot undestand your geometry and flow character. Bye, John

 January 20, 2008, 18:38 Re: Volume of Fluid help please! #3 Gareth Uglow Guest   Posts: n/a OK, I will decrease the number of iterations. What timestep would you recommend? 0.001s? The problem is 2-D, and models a horizontal cylinder of diameter 0.24m in a flow, 0.06m above the bottom. The domain extends 1m upstream, 4m downstream, and 1m high. I'd like the free surface to be about 0.5m above the cylinder. Thanks Gareth

 January 21, 2008, 03:30 Re: Volume of Fluid help please! #4 bohis Guest   Posts: n/a Hi, I think there should be no problem. Your task sounds quite easily. (are you using Geo-reconstruct scheme? are you sure about your boundary conditions? gravity? etc.) A width of interface also depends on mesh quality. Are cells fine enough? Anyway, I still cannot understand your task. If you wanted, you would send me description in more details (bohacek.jan@gmail.com) (figure,dimensions, BC,..) Otherwise, Good Luck!! John

 January 24, 2008, 10:29 Re: Volume of Fluid help please! #5 Gareth Guest   Posts: n/a Hello again, I'm still having some problems with this. I have tried all sorts of boundary conditions, but i think the problem is in the solver rather than the conditions. Even with a timestep 1e-5 the air-water interface still is not a thin line but is very dissipative. Are there any particular settings to be made in the solver options? thanks Gareth

 January 24, 2008, 11:28 Re: Volume of Fluid help please! #6 bohis Guest   Posts: n/a for sharpener interface choose modified HRIC discretization for volume fraction eq.

 January 24, 2008, 11:58 Re: Volume of Fluid help please! #7 Matthieu Guest   Posts: n/a Perhaps you should change your initial condition for the volume fraction of water. 0.5 is not a physical value but only a way to model the interface between air and water. For the initialization, you should only affect 0 or 1 for the volume fraction of water, not 0.5. It may be necessary to change your mesh in Gambit to define the initial volume of water and the initial volume of air. Then, you can affect in Fleunt the value 1 for the volume of water, and 0 for the volume of air. If it does not change anything, you can decrease the under-relaxation factor of the VOF equation. For my own experience, the under-relaxation factors must be small when the VOF model is used: generally 0.1.

 February 8, 2008, 11:30 Re: Volume of Fluid help please! #8 Martin Guest   Posts: n/a It sounds like you are solving a nano-scale problem... If you still have the problem you could check if the scale in Fluent is the same as in Gambit. (Grid -> Scale -> Grid was created in … )

 February 13, 2008, 13:15 Re: Volume of Fluid help please! #9 Graham Guest   Posts: n/a The blurring is somewhat unavoidable numerical diffusion of the phase. mHRIC works well but will may give you some blurring still if the mesh is poorly aligned for the interface/flow and/or contains lots of unstrucutred regions. Try CICSAM if georeconstruct is giving you issues - or if looking for a s.state solution solve to convergence using HRIC then run georeconstruct with low # interations per cycle and small time step to sharpen.

 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 14:02.

 Contact Us - CFD Online - Top