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

2 Phase flow - applying Lift

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 22, 2007, 08:01
Default 2 Phase flow - applying Lift
  #1
Jayant
Guest
 
Posts: n/a
Hi I am trying to simulate a gas-liquid flow with the liquid being the primary phase. The problem is that whenever I include a Lift force in the interactions between the 2 phases the residuals rise very high and fluent gives a Floating Point Error

I tried a constant lift with single coefficient. Plzz Help Thnx in advance ...

  Reply With Quote

Old   July 22, 2007, 09:56
Default Re: 2 Phase flow - applying Lift
  #2
kp
Guest
 
Posts: n/a
Hello Jayant, Lift forces are very important for simulating bubbly pipe flows. Now you encounter divergence as lift forces add a momentum source term causing solution to develop more complexities as if you recall they have gradient times slip. Now you can solve this issue by practically lowering the under relaxation factors for momentum and continuity. Reduce both of them to say 0.1. It will take long time to converge but eventually it will converge. It is recommended also to use turbulent dispersion models which add stability to the solution. Now an easy way for you to enable dispersion is by using k-e dispersed phase model. From TUI (Text-User-Interface) you can activate calculation of drift velocities which in-turn lead to calculation of dispersive forces as: Define/models/viscous/multiphase-turbulence/multiphase-options/enable dispersion force yes Also you may like to change drag forces as the one by Schiller-Naumann is not good for bubbly flows. Now to add more to lift forces: A constant lift force coefficient say 0.25 is good but it is primitive. Use of advanced models like the ones by Tomiyama is recommended. I am sure you will have many more questions as the geometry seems to be simple but its the most complex one when it comes to simulating it. whose data set are you trying to work with. Feel free to ask more questions if you have any! Best: KP
  Reply With Quote

Old   July 22, 2007, 09:58
Default Re: 2 Phase flow - applying Lift
  #3
kp
Guest
 
Posts: n/a
Let me know your co-ordinates and what set up are you trying ot model? A pipe, bubble column...Are you from Chemical or power sector. It would be good if you can converse with me at kp@dal.ca . I can add more to what we discussed earlier. Best KP
  Reply With Quote

Old   August 2, 2007, 10:51
Default Re: 2 Phase flow - applying Lift
  #4
Summer
Guest
 
Posts: n/a
Hello, KP, I have read the previous messages you posted about the lift force and it is really useful. Now, I am trying to model air-water two-phase flow in a circular pipe with Eulerian model as well. And I am using unsteady solver. Since I did not get the convergent solutions with the default under-relaxation factor, I reduced them to quite a small value. The problem I met is that for every time step, it decreased sharply to 10-4 and then stay at that level until next time step. During next time step, it increases quickly to 0.1 and then decrease sharply to 10-4 and stay the level. This process keeps repeating. Do you think it is a reasonable results after some time steps? BTW, I only use first order scheme and mixture turbulence model. The flow should be in bubbly flow and I use the default drag force and lift coefficient is set to be 0.5 (I know it is a little larger according to Tomiyama's suggestion: 0.288). Any suggestion is welcome and valuable. Thank you in advance!
  Reply With Quote

Old   August 2, 2007, 10:57
Default Re: 2 Phase flow - applying Lift
  #5
KP
Guest
 
Posts: n/a
For pipe flows use steady state. Unsteady is not necessary. Now if its a bubble columns then you can use unsteady. In unsteady two things can come in picture: COurant number and also your size of grid. KP
  Reply With Quote

Old   August 2, 2007, 11:35
Default Re: 2 Phase flow - applying Lift
  #6
Summer
Guest
 
Posts: n/a
Thanks for replying. However, since I noticed there some instabilities in my solution when the gas velocity was high, I decided to use the unsteady solver. I use implicit method so that the two parameters (courant number and grid size) do not matter a lot. Please correct me if I make some wrong statements. Thank you very much!
  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
behavior of two phase flow in a pipe Sonia84 FLUENT 5 September 17, 2013 16:31
Two phase flow in a distributor Mohsin FLUENT 5 May 24, 2010 02:57
mass flow in is not equal to mass flow out saii CFX 2 September 18, 2009 08:07
Two phase flow with condensation Sunnie FLUENT 0 May 31, 2009 10:02
Two phase flow models Atholl Main CFD Forum 2 May 7, 2002 03:49


All times are GMT -4. The time now is 22:09.