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

Doubt on VOF

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 20, 2002, 00:18
Default Doubt on VOF
  #1
some1
Guest
 
Posts: n/a
I'm using a commercial CFD software and I need to model a liquid film flowing over a sphere using VOF. Air is flowing in the same direction at a higher velocity ( not too high).

I want to change the drag forces in the gas-liquid and liquid-air interfaces. I suspect that the equations I want to implement must hold only in the gas-solid interface and in the free surface ( volume fraction<>0 or 1).

I asked the technical staff on how to do it, as only answer they wondered why should I want to change the drag forces in VOF.

I want to change them, but it rised questions on if what I'm doing is right.

Can somebody help solve my doubts?

Thanks a lot in advance.

some1

  Reply With Quote

Old   March 20, 2002, 03:30
Default Re: Doubt on VOF
  #2
edward g. cruz
Guest
 
Posts: n/a
I did a multi-phase problem on Fluent. And I agree with "the technical staff" on why you have to or not change the drag forces in VOF. Also Vol Fraction is between 0 and 1. When it comes to computer simulations(i.e. CFD) start with a simple and quick solution approach, (use the default values whenever possible) and when you get your initial solution, you can then play around with your approach to get the solution that you want. This is the only way(I hope I'm wrong...) you're going to find the answer to your "Doubt on VOF". Can you send me a picture of your problem? Thanks. I hope I was of some help and Go with the Flow, Edward
  Reply With Quote

Old   March 20, 2002, 13:13
Default Re: Doubt on VOF
  #3
some1
Guest
 
Posts: n/a
Thanks a lot for your answer. I have already solved the problem with the default values, I'm in the next step as you mention.

I'm sending you the figure.

Thanks again

some1
  Reply With Quote

Old   March 21, 2002, 00:23
Default Re: Doubt on VOF
  #4
edward g. cruz
Guest
 
Posts: n/a
Arturo; Thanks for the picture. Now, I know what you're up to. I agree with your initial assessment of your initial solution. Here are some more hints:

It is possible for you to animate your solution. For example, for every 10 iteration you make, save a hardcopy of the window containing the resulting plot as a tiff file. (Make sure that every window is the same size) Then use a graphics package to assemble all the tiff files into 1 animated file. You can only do this manually. You can't write this into a script and run Fluent in background mode. It's nice to have an animated solution to an unsteady problem. You'll really see what's happening.

With regard to "the drag forces in the liquid-solid and gas-liquid interfaces..." You may have to change your mesh so that you have more cells in the region close to liq-solid & gas-liquid interfaces to get a better answer for everything including the drag forces. Try using TGrid to do this, Gambit will not do this. A really easy and dirty way is to go back to Gambit and increase the density of your mesh. But this method slows Fluent and if you get carried away, your Admin will not like it if he finds out that you're using almost all the resources available.

Just keep on going with Fluent, it's a really nice package. The only thing I hate about it is its mesh generators(take a look at any CFD book or paper, you'll know what I mean). If you have any more questions, just let me know. Go with the Flow, Edward

  Reply With Quote

Old   March 21, 2002, 16:00
Default Re: Doubt on VOF
  #5
Neale
Guest
 
Posts: n/a
You can't change the drag of the VOF free surface model. The drag is infinite because VOF is basically the homogenous limit of a full multiphse model. To change the drag you really need to switch to a full multiphase model so that there is a drag term for you to modify.

Neale
  Reply With Quote

Old   March 21, 2002, 17:03
Default Re: Doubt on VOF
  #6
some1
Guest
 
Posts: n/a
thanks!!!! I will try your hints!!

some1
  Reply With Quote

Old   March 22, 2002, 12:50
Default Re: Doubt on VOF
  #7
new1
Guest
 
Posts: n/a
Thanks Neale That was my doubt Do you have any advice?

I really appreciate your input.

some1
  Reply With Quote

Old   March 22, 2002, 16:20
Default Re: Doubt on VOF
  #8
some1
Guest
 
Posts: n/a
Dear Neale your answer made me think about some possible strategies. Do you think is possible to use the predicted liquid surfaces to perform further simulations with other model?

thnx

some1

  Reply With Quote

Old   March 25, 2002, 12:49
Default Re: Doubt on VOF
  #9
Helge
Guest
 
Posts: n/a
1) There is a major problem concerning drag between liquid and gas using the VOF method (implemented in Fluent, STAR-CD, CFX and others). 2) The drag is a result of the simulation itself and can only be as accurate as the liquid/gas interface is resolved. 3) The interface unfortunately smears over 3 to 6 cells so you can more or less forget drag results 4) This is not the case in a different method called MAC (Marcer And Cell). But there is no commercial code with that method implemented
  Reply With Quote

Old   March 25, 2002, 20:08
Default Re: Doubt on VOF
  #10
new1
Guest
 
Posts: n/a
Thanks Helge, it seems a weekness of VOF, from what I've read the model solves a single momentum equation and it can be added some forces, i.e. surface tension.

For me it would be natural to add drag forces but from the formulation is not evident.

new1
  Reply With Quote

Old   April 3, 2002, 16:03
Default Re: Doubt on VOF
  #11
Neale
Guest
 
Posts: n/a
Helge,

The drag is infinte in a free surface VOF model, i.e. there is no slip velocity between the phases. So, it's not that there is a problem with the commercial codes, it's a fundamental limitation of the model, no matter who implements it.

If drag is important, then in CFX-4 and CFX-5.5 you can use the full multiphase model instead, which has a slip velocity drag model. This works fine.

Neale.

  Reply With Quote

Old   April 4, 2002, 01:16
Default some clarification requested for
  #12
mukhopadhyay
Guest
 
Posts: n/a
Single phase momentum equation and a continuity equation accommodating the density (weighted average) are the basis of VOF - am I correct in my understanding ? Suppose I am modeling the surface disturbance in a liquid (say water) exposed to air, using VOF. How do I take care of the viscosity ? Is it the weighted average too ? Is that a right proposition? Viscosity is intensive property - can I do that? Has there been any attempt to evaluate/estimate the prospective numerical diffusion ? Else, what are we predicting ? At this stage, I am not talking of Newtonian behavior or not. newtonian
  Reply With Quote

Old   April 6, 2002, 14:18
Default Re: Doubt on VOF
  #13
Helge
Guest
 
Posts: n/a
To your first point. I doubt that the drag is infinite in a VOF formualtion. Of course the relative velocity between the two phases is zero. But that is also the case between a fluid and a wall in single phase flow. Nevertheless there is drag between the fluid and the wall. So it should be possible to calculate a drag between the two fluids.

To your second point. If you want to get the drag out of a simulation you should not use a velocity drag model in a full multiphase model because you are using an emperical formula for the drag i.e. you are using the result as input.
  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
Doubt about F_FLUX(f,tf) macro & VOF ?!!!!!!!! asghari FLUENT 2 October 28, 2012 04:03
ATTENTION!! Validty of Fluent's VOF?? ozgur Main CFD Forum 3 February 18, 2004 19:19
ATTENTION!! Validty of Fluent's VOF?? ozgur FLUENT 1 February 18, 2004 12:59
Difficult BCs about Freesurface Simulation by VOF Yongguang Cheng FLUENT 0 September 19, 2003 07:39
another VOF doubt some1 Main CFD Forum 6 April 16, 2002 06:52


All times are GMT -4. The time now is 03:21.