CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   2 Phase flow - applying Lift (http://www.cfd-online.com/Forums/fluent/45463-2-phase-flow-applying-lift.html)

Jayant July 22, 2007 08:01

2 Phase flow - applying Lift
 
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 ...


kp July 22, 2007 09:56

Re: 2 Phase flow - applying Lift
 
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

kp July 22, 2007 09:58

Re: 2 Phase flow - applying Lift
 
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

Summer August 2, 2007 10:51

Re: 2 Phase flow - applying Lift
 
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!

KP August 2, 2007 10:57

Re: 2 Phase flow - applying Lift
 
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

Summer August 2, 2007 11:35

Re: 2 Phase flow - applying Lift
 
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!


All times are GMT -4. The time now is 05:59.