# 2 Phase flow - applying Lift

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

 July 22, 2007, 08:01 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 ...

 July 22, 2007, 09:56 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

 July 22, 2007, 09:58 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

 August 2, 2007, 10:51 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!

 August 2, 2007, 10:57 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

 August 2, 2007, 11:35 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!

 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 Sonia84 FLUENT 5 September 17, 2013 16:31 Mohsin FLUENT 5 May 24, 2010 02:57 saii CFX 2 September 18, 2009 08:07 Sunnie FLUENT 0 May 31, 2009 10:02 Atholl Main CFD Forum 2 May 7, 2002 03:49

All times are GMT -4. The time now is 00:30.