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

Volume of Fluid help please!

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 19, 2008, 09:17
Default 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?
  Reply With Quote

Old   January 19, 2008, 15:53
Default 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
  Reply With Quote

Old   January 20, 2008, 18:38
Default 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
  Reply With Quote

Old   January 21, 2008, 03:30
Default 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
  Reply With Quote

Old   January 24, 2008, 10:29
Default 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
  Reply With Quote

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

Old   January 24, 2008, 11:58
Default 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.
  Reply With Quote

Old   February 8, 2008, 11:30
Default 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 … )

  Reply With Quote

Old   February 13, 2008, 13:15
Default 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.
  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 15:30.