
[Sponsors] 
November 25, 2012, 09:26 
Multiphase  Eulerian (air and water)

#1 
New Member
Markus
Join Date: Nov 2012
Posts: 7
Rep Power: 6 
Dear all,
I am trying to implement a multiphase flow of air and water. The water content is present as dispersed droplets. Number and diameter are given. The flow that I am trying to model is basically the flow around an optical probe, which is cylindrical. The optical probe has to be protected against the water droplets. This protection is realized by implementing air jets at the probe. So far I ran steady state and transient calculations without any droplets which worked out perfectly fine. But once I apply the dispersed flow with a certain volume fraction of the water my simulations crashed because of an overflow caused by too high Mach numbers. I took a look at the results right before the overflow where I recognized that the high Mach numbers of the air are in the vicinity of the wall. Does anyone have an idea what could cause this problem? Thanks in advance! 

November 25, 2012, 17:40 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,201
Rep Power: 103 
This suggests that simply turning the water on is numerically unstable. Try slowly ramping it in. Alternately try a transient simulation...... but this will take a long time to run I suspect.
Also try double precision numerics, that can sometimes help; and for the steady state run where you first turn on the water make sure the physical time step is small and ramp it up as convergence progresses. 

November 25, 2012, 18:26 

#3 
New Member
Markus
Join Date: Nov 2012
Posts: 7
Rep Power: 6 
Hey! Thanks a lot for you feedback! Already ran a double precision transient simulation which did not help a lot. I used a water volume fraction of 0.05 and respectively 0.95 volume fraction of air as initial condition for the whole domain and the same fractions for the velocity inlet. But therefore I'll try to decrease this volume fraction for the water and start another run.
Do you think the accumulation of water droplets on the surface of the probe could cause this problem? Is the dispersed fluid setting not capable of handling accumulation of water droplets? 

November 25, 2012, 18:29 

#4 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,201
Rep Power: 103 
Also  I assume the air flow is fast enough to be compressible? What speed is it running at?
If you want to model the accumulation of water on the surface you will need a wall film model. 

November 25, 2012, 18:34 

#5 
New Member
Markus
Join Date: Nov 2012
Posts: 7
Rep Power: 6 
Right now the inlet velocity is 113m/s, which corresponds to M=0.3. But test cases with M=0.6 will follow... Would you recommend to include compressible control already at M0.3? Therefore I'll have to include a wall film model because the accumulation will not be avoidable in some cases.


November 26, 2012, 08:06 

#6 
Senior Member
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 278
Rep Power: 14 
You might be getting high Reynolds numbers because when you add water, even at 5% volume, your mixture density increases by 50x or more, depending on air local density.
I'm not sure how robust it will be, but if you only have 5% of water you could try modelling it using a Lagrangian particle model. 

November 26, 2012, 09:46 

#7 
New Member
Markus
Join Date: Nov 2012
Posts: 7
Rep Power: 6 
Lagrangian particle model is not an option so far, because I have to implement 10^3 up to 10^5 particles per cm^3 with a diameter of 100 micrometer dispersed in the air flow. I assume such high number of particles can't be handled with the Lagrangian approach.
But you are right about the high density change... could be a problem. 

November 26, 2012, 11:00 

#8 
Senior Member
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 278
Rep Power: 14 
You don't have to model each single particle. The solver works with a concept called parcel, where each parcel represents a number of real particles. That's why even when you have particles with a constant diameter you need to enter both the number of particles and the mass flow rate.
I think one of the tutorials on Langrange covers this. 

November 26, 2012, 11:07 

#9 
Senior Member
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 278
Rep Power: 14 
Actually at 1e5 particles you're no longer at a region where the CFX particle model is valid because you'd have a volume fraction of ~42%, which is too high. In such case Eulerian is the way to solve it.


November 26, 2012, 14:36 

#10 
New Member
Markus
Join Date: Nov 2012
Posts: 7
Rep Power: 6 
I have calculated a volume fraction of 5% with a particle number of 1e+5 per cm^3 with a diameter of 100 micrometer! I have no idea how you come up with a volume fraction of 42%?
Anyway, my problem of the numerical instability by turning the water on persists. I have set the physical timestep to 1e6s and I decreased the water volume fraction to 0.005 in order to be able to slowly increase the water content. Still there is almost no change of the sudden increase the Mach number. 

November 26, 2012, 16:05 

#11 
Senior Member
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 278
Rep Power: 14 
I used a wrong value for the particle diameter, that's how I got it wrong. But that's better, because it means you can definitely use the Lagrangian particle model.
If you rather use Eulerian, try saving a backup file right before your problem diverges. This way you can look at the velocity field in Post to see where the problem is originating. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Multiphase model, water disperses in air  bugra  Main CFD Forum  1  January 30, 2010 11:57 
multiphase model, water in air?  bugra  Main CFD Forum  10  January 2, 2010 14:09 
air bubble is disappear increasing time using vof  xujjun  CFX  9  June 9, 2009 07:59 
air and water vapour mixture  multiphase model  Saba  FLUENT  0  February 10, 2009 13:05 
Help!!!problems in air jet into water bath  kim  FLUENT  4  June 9, 2003 07:04 