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

Multiphase air-water filling problem

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 11, 2009, 03:49
Default Multiphase air-water filling problem
  #1
New Member
 
Join Date: May 2009
Posts: 17
Rep Power: 8
shogologo is on a distinguished road
Hi everybody,
I'm facing some strange results in a filling problem where a cylindrical tank full of air is filled with water.
Water enters the tank flowing on the lateral walls and everything is fine with a well defined interface.
But as it reaches the bottom of the tank the interface becomes really thick and it seems some air in entrained below the thick surface as the tank is filled.
I used both homogeneous and in-homogeneous (better results but not satisfying with air as dispersed phase mean diameter 0.0001 mm) on a very refined 3d sample grid.

Any suggestion?
Thanks in advance
shogologo is offline   Reply With Quote

Old   June 11, 2009, 06:59
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,805
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Hi,

This area is much improved in V12. Are you using V12? The new coupled VF solver should work well here (I did lots of beta testing on this feature and I think we ironed out all the bugs! For your information the issue was the coupled VF solver in V11 did a poor job of conserving volume fraction.)

Are you modelling surface tension? This makes a big difference.

Glenn Horrocks
ghorrocks is online now   Reply With Quote

Old   June 11, 2009, 07:19
Default
  #3
New Member
 
Join Date: May 2009
Posts: 17
Rep Power: 8
shogologo is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Hi,

This area is much improved in V12. Are you using V12? The new coupled VF solver should work well here (I did lots of beta testing on this feature and I think we ironed out all the bugs! For your information the issue was the coupled VF solver in V11 did a poor job of conserving volume fraction.)

Are you modelling surface tension? This makes a big difference.

Glenn Horrocks
Thanks Glenn for replying.
I really spent a lot of time in reading throughout the forum and I know you have gained a lot of pratice and experience in multiphase problems - really appreciated you ansewred me (i.e. you suggested in a previous thread SST instead of k-e and I agree with this choice).

I'm trying to solve this (apperantly to me) simple problem in conjunction with CFX techs with CFX 12. I'm currently taking account of surface tension with a value of 7.2e-2 [N m^-1].
To explain better what is happening: very thin film of water on the lateral walls collide on the bottom of a tank. As the filling process go on, when displaying water fraction, under the interface the color is not uniform and water is displayed as "a flame".
Buoyancy activated.
Any other suggestion is appreciated.

Thanks

Last edited by shogologo; June 11, 2009 at 16:38. Reason: .
shogologo is offline   Reply With Quote

Old   June 11, 2009, 18:30
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,805
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Hi,

Set the volume fraction smoothing to none, use adaptive timestepping homing into 3-6 iterations per timestep.

CFX is poor at this type of analysis, it is very slow. I got a speedup of 30x by switching to Fluent for free surface simulations with surface tension.

Glenn Horrocks
ghorrocks is online now   Reply With Quote

Old   June 12, 2009, 02:07
Default
  #5
New Member
 
Join Date: May 2009
Posts: 17
Rep Power: 8
shogologo is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Hi,

Set the volume fraction smoothing to none, use adaptive timestepping homing into 3-6 iterations per timestep.

CFX is poor at this type of analysis, it is very slow. I got a speedup of 30x by switching to Fluent for free surface simulations with surface tension.

Glenn Horrocks
Hi Glenn,
Thanks for your suggestion: I'll try and report about this.
I wouldn't expect these differences with Fluent since CFX coupled solver usually provide less (but longer) iterations to get to a converged solution.
Please correct me if I'm wrong: VOF's Fluent is equivalent to Homogeneous in CFX?
I am not really sure if I should use Homogeneous or non homogeneous for my problem...I got a really nice solution for homogenous with open bottom to use as initialized solution with a well defined film on the walls but as I close the bottom I got the "flame" under the interface; for non-homogeneous the film on the walls are not so well defined...

Thanks
shogologo is offline   Reply With Quote

Old   June 12, 2009, 08:42
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,805
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Hi,

Yes, VOF in Fluent is equivalent to Homogeneous multiphase in CFX.

Use Homogeneous if you want the interface to remain sharp. Use inhomogeneous if some mixing (eg foam, bubbly regions) occur.

Glenn Horrocks
ghorrocks is online now   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
Boiling of water with hot air Dr. Flow Squad CFX 2 July 27, 2009 07:37
Setfields inoutlet and water and air patches erik023 OpenFOAM Pre-Processing 1 September 29, 2008 10:05
Simulating air jet into 2D & 3D water domain Imran FLUENT 0 June 6, 2006 08:57
Converge problem for multiphase flow Jen FLUENT 2 September 8, 2005 08:47
Air and Water VOF model, Error?? boris FLUENT 5 July 19, 2002 03:08


All times are GMT -4. The time now is 19:26.