
[Sponsors] 
September 21, 2011, 07:50 
problem with two phase flow (air injected in water)

#1 
Member
Miles
Join Date: Sep 2011
Posts: 48
Rep Power: 6 
Hi
I am simulating the flow in a water box equipped with a nozzle in the bottom. The nozzle injects a mix of air and water (alpha = 0.1) After some reading on this kind of flow on this forum I have chosen the twophaseeuler solver. To initialize the flow I have taken the velocity distribution for a case with only water. I have reproduced the settings of the bubble column tuto. Except for the drag force. A t=0, I start to inject some air. What i do not understand is that after a few iteration I get a full air velocity field even in region in which the air is not present I have the impression that this strange behavior is due to the fact that OF calculates my air velocity by scaling the water velocity. Why is this happenning? If any body has some advice I'd be glad. Another question concerns the pressure field. Since the box is filled with water the pressure changes with altitude. So I don't want to impose pressure at the outlet of the domain. What alternative type could I put? If I put an inletoutlet velocity condition what is the corresponding condition I should use for pressure? Thanks a lot The picture illustrating my case are given. 

September 21, 2011, 08:44 

#2 
Member
Greg Melling
Join Date: Nov 2010
Posts: 41
Rep Power: 7 
You've fixed the pressure at the top, so zeroGradient on your outlet should work...


September 21, 2011, 10:21 

#3 
Member
Miles
Join Date: Sep 2011
Posts: 48
Rep Power: 6 
Thanks for your answer.
I put a zero gradient at the outlet but due to the recirculation I have some flow in and out the exit surface, So I may try a inletoutlet BC. Do you have any guess why Ua is indexed on Ub even when specie A (i.e. air) is not present? In should be zero in such case. Thanks again. 

September 22, 2011, 13:14 

#4 
Member
Miles
Join Date: Sep 2011
Posts: 48
Rep Power: 6 
Hi
I have solved my pressure distribution problèms. What I do not get it's why and how a velocity of a phase that is not present in a fluid domain (i.e. vol fraction alpha=0.0) can be non equal to zero????!!!! I am using twophaseeulerfoam. I have reproduced the tuto of the bublle column and i have found the same issue when velocity is set to zero at the beginning. Please has anyone any guess where it might come from? regards, 

September 23, 2011, 22:24 

#5  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
Hi Miles,
Quote:
This is a quite common approach in many codes for nuclear safety applications and it was also adopted by Oliveira and Issa in one of their papers. The phaseintensive momentum equation has the (correct) property that it makes the velocity tend to the particle terminal velocity if interaction terms are removed. In other words, seeing a nonzero velocity where alpha is zero, is expected. However this should not lead to problems since all the terms depend on alpha. Best, Alberto
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

September 25, 2011, 13:22 

#6 
Member
Miles
Join Date: Sep 2011
Posts: 48
Rep Power: 6 
Dear all,
Thanks a lot for your answers. I have another question. I try to reproduce a two phase flow simulation made with Fluent. It is the same case as described above except the fact that I do not simulate the air volume above the free surface of water. I have concerns about the BC to define for the free surface and the outlet. For the free surface for principal phase (i.e. water, phaseB) I use the slip BC on Ub. I am confused for the air (phase a). The air can flow out of the domain at the free surface. Therefore witch BC do you think would be suitable for velocity Ua and alpha? I have the same concern for the outlet. I enclose to my post a picture of my test case and the BC I want to define. Thanks a lot for your help and advices. Regards, 

September 25, 2011, 22:07 

#7  
Senior Member
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 437
Rep Power: 13 
Quote:
here are few questions: 1# Alpha = 0.1 , means that 0.1 x Water + 0.9 x Air? Am I right. 2# Wouldn't it be better to define a new fluid with properties derived from alpha x Water + (1Alpha) * Air , should be called Steam and solve for this fluid. So main phase would be steam and secondary phase would be water. At inlet Alpha = 1 then. Am I wrong about it, are there problems in this approach that would give wrong results? Please correct me. 3# what are the geometric dimensions of box you presented as domain. This I am asking because currently I am trying to write VOF code myself and if I get time would like to run your case myself. (If possible, just for pleasure and fun). 

September 26, 2011, 13:44 

#8  
Member
Miles
Join Date: Sep 2011
Posts: 48
Rep Power: 6 
Hi,
sorry for the delay of answer Quote:
alpha is the vol fraction of air so in fact it's the opposite: 0.9 watter 0.1 air Quote:
I can't do that. It's a filtration process. So I want to see how air and water separate. So I don't want to define a mixture of air+water. Quote:
inlet: 0.5m outlet: 0.25m Regards, Miles 

September 26, 2011, 18:00 

#9  
Senior Member
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 437
Rep Power: 13 
Quote:
I was able to run your case. So far it is 'Colourful Fluid Dynamics', it does show me some results. Look alright to me. (off course not usable). There are few things: 1. I did not know the nozzle design so i just used slit of 10mm as inlet. My guess is that inlet is smaller than this in diameter. 2. About the free surface at top, I used outflow condition. That is in this case flow can go out and some of it can come in. Question: Can flow really come in and go out of it. OR it is closed?? 3. I extended the outlet part and fixed it to a pressure boundary condition. Anyway i do not have problems, SO FAR, solver runs fine (at least for last 10 minutes that i tried ). PS: I did not run it fully, but here is where i stopped it. Last edited by arjun; September 26, 2011 at 18:24. 

September 27, 2011, 12:39 

#10 
Member
Miles
Join Date: Sep 2011
Posts: 48
Rep Power: 6 
Hi
Great simulations. Is it made with your own code? What method it is? VOF? The problem is the BC at the top of the domain. Since it is air in a water box, the water can't escape from the upper surface. That's why I need to fix a different BC for water phase and air phase!!! And since I need two study diameter sensibility, I am stuck with twophaseeulerfoam model. Another question: what did you put as a BC for the outlet? p=0? Why did you add this long duct at the outlet? regards, P.S.: does anyone know what is pressure in OF2.0.1? I have read that in previous version of the code it was in fact Pstaticrho*g*h, than in antother version it was just Pstatic. What is the actual statement for OF 2.0.1? Last edited by miles_davis; September 27, 2011 at 13:00. 

September 27, 2011, 22:38 

#11  
Senior Member
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 437
Rep Power: 13 
Quote:
I am following this paper: http://webfea.fea.aub.edu.lb/cfd/pdf...SComplete.pdf The code is same as discribed in this paper with a minor change from my side, instead of SUPERBEE , I am using Bounded Downwind of HRIC scheme. Results are impressive so far, but I would now try to make it implicit. Quote:
I think partial blocking of water , though possible by modifying code, is not suggested. Quote:
BUT, I could switch to outflow conditions instead of pressure outlet, where pressure at only 1 point is fixed (not at whole outlet). Usually in the solver when you have outflow conditions solver tries to balance the mass flux and make it equal to flow coming in through inlets. For running your case I had to switch that thing off. So thanks, now I can provide user an option to switch forcing of mass balance at outflow. Before your case it did not occur to me. PS: I am solving for air and water is my secondary phase. This means VOF equations are solved for air and water C = 1  Air_C 

September 30, 2011, 06:35 

#12 
Member
Miles
Join Date: Sep 2011
Posts: 48
Rep Power: 6 
Hi ,
I have kept on trying to simulate air injection with the Twophaseeulerfoam. After having performed a transient simulation of the water injection, I added the air. The air bublles diameter is 150µm. I take into account drag with a shcillerneuman model (I have reproduced the bubble column tutorial for drag interaction but I hope the reading of Rush thesis will give me a better rule of choice for bubble drag). Lift and virtual mass. Are on as well. I get a rising air flow (see picture) What I do not understand is why the velocity of the buble remain strictly aligned on the water velocity. it seems that drag effects are very high and so bubbles stay in close contact with the air flow. I was expecting buoyancy effect to help bubble to rise faster than the water flow! I am currently reading Numerical aspects of an algorithm for the Eulerian simulation of twophase flows Paulo J. Oliveira Raad I. Issa and the thesis from Rush. It seems that buoyancy effects are indeed taken into acount. So I do not understand why I can't reproduce these effects with the model. Maybe I misunderstood something in the model. Thanks for your help. Regards, Miles 

October 7, 2011, 11:46 

#13 
Member
Miles
Join Date: Sep 2011
Posts: 48
Rep Power: 6 
Hi,
I have made a test: a simple volume of air in the domain at the beginning of the calculation. It appears that the air is rising in the water due to buoyancy effect. So this is not the problem in my simulation. I have run another tests and in every case for d<500µm, the velocity field for watter and air are exactly the same. As if the drag force of water on air bubbles tends to infinity. I have checked and read the solver, I do not see anything strange in its formulation. Has anyone ever encountered such problems? Thanks for your help. Regards, 

October 8, 2011, 01:10 

#14 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
What is the injection velocity of the air in the real system you are simulating? Is it consistent with your setup?
If the air is injected at a high enough velocity, it will clearly create a sort of jet. Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

October 11, 2011, 17:53 

#15 
Member
Miles
Join Date: Sep 2011
Posts: 48
Rep Power: 6 
Hi,
The air enters at the same velocity as water: 0.2 m/s. And it does create a jet. I am ok with that. My concern is on the fact that at the free surface of water, I was expecting the bubble of 150µm to continue rising and escape! But they reach the surface and slip on the free surface as the water. Besides the air velocity is strictly alined on water velocity. I have to check Stokes number but it seems wired. Regards, 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
introduce air to water flow  masoudarami  FLOW3D  6  February 19, 2012 06:31 
mass flow in is not equal to mass flow out  saii  CFX  2  September 18, 2009 08:07 
Problem of air bubbles in water. Please help !!!  xc  FLUENT  4  February 6, 2008 06:05 
Is there any one working on two phase flow problem  sina  FLUENT  2  October 6, 2004 06:55 
Problem on boundry of two phase flow  youngan  CFX  2  June 30, 2003 02:11 