
[Sponsors] 
How determin volume fraction in Eulerian Scheme multiphase flow 

LinkBack  Thread Tools  Search this Thread  Display Modes 
October 13, 2014, 17:18 
How determin volume fraction in Eulerian Scheme multiphase flow

#1 
New Member
Mechanical Engineer
Join Date: Sep 2014
Posts: 11
Rep Power: 11 
Hi All,
I am new to multiphase flow. I am trying to simulate multiphase flow in fluent with water and air as primary and secondary fluids respectively. The inlet velocity of air is 1.5 m/s and inlet velocity of water is 0.8 m/s. The diameter of the inlet port is 20 mm. I don't know how to calculate the volume fraction for secondary phase i.e. air in my case. Is there any particular formula for volume fraction. Velocity of air divided by summation of both velocities seems not to work. Any comments in this regard will be highly appreciated. Thanks. 

October 13, 2014, 22:36 

#2 
Senior Member
Cees Haringa
Join Date: May 2013
Location: Delft
Posts: 607
Rep Power: 0 
Hello,
I'm not quite sure what you mean. If both fluids enter simultaneously via the same inlet, then the fraction of air in there is simply flow air/flow total, in this case 1.5/2.3. Why does this not work? 

October 14, 2014, 02:13 

#3 
New Member
Mechanical Engineer
Join Date: Sep 2014
Posts: 11
Rep Power: 11 
Thank you Ceesh for you reply.
Yes, you are right, both fluids enter from the same inlet. The problem is that when I specify the volume fraction of air inlet as 0.65 (=1.5/2.3), it faces quick divergence. But if I specify it to a very low value then it runs for some time before getting diverged. Let me tell you the background of the problem. Actually I am working on Eulerian 3phase scheme with packed bed. Water and air are primary and secondary phase respectively. Third phase is solid which has volume fraction of 0.605 in the bed. It has got zero velocity, thats why I specified 'zero' in volume fraction at inlet boundary condition for solid phase. Also I am specifying '1' in backward volume fractioin for solid phase at outlet boundary condition so that it doesn't go out from the outlet. So in order to give solid phase a volume fraction of 0.605 inside the bed, I am specifying volume fraction of solid as 0.605 in initial condition. In short: Boundary Condition Air velocity : 1.5 Air inlet volume fraction: 0.65 Water Velocity: 0.8 Water inlet volume fraction: 0.35 Solid Velocity = 0 solid inlet volume fraction: 0 solid outlet backward volume fraction: 1 Initialization: Solid initial volume fraction: 0.605 Water initial volume fraction: 0.1 Air initial volume fraction: 0.295 Above specifications seem to be correct but it doesn't work and diverge quickly unless I change inlet volume fraction of air to very small value. Any comment will be highly appreciated. 

October 14, 2014, 21:53 

#4 
Senior Member
Cees Haringa
Join Date: May 2013
Location: Delft
Posts: 607
Rep Power: 0 
Ah, I see.
I have little experience with modelling packed beds, but I think I'd take a different approach. Even as a phase with 0 inlet velocity, drag and such will still act on the packing hence transport it, and I assume you just want the packing to be stationary right? Then it may be better to specify it under cell zone conditions > porous zone, and use your packed bed specifications to determine porosity and so on. Then, you are sure the phase is absolutely not moving. Furthermore, specify a 2phase Eulerian flow for your liquid and gas. Your current divergence problem has very likely to do with the 3th phase specifics, and not with the gas to liquid ratio. (maybe at a low value the transport of the solid phase is different, which buys you some time before it inevitibly still diverges) Also, outlet backflow fraction doesn't mean that it cannot go out from the outlet  it still can, and still will. At a pressure outlet, it may happen that you get flow reversal  that part of the outlet actually acts as an inlet because of a pressure minimum in your domain. In that case, the backflow fraction specifies the composition of this inflow. So with the current setting, in case of backflow, your domain will be filled with solid. And that may cause problems. Hope this helps! Cees 

October 15, 2014, 13:16 

#5 
New Member
Mechanical Engineer
Join Date: Sep 2014
Posts: 11
Rep Power: 11 
Again CeesH, Thanks for your time.
Actually I am using drag force concept to model multiphase flow through packed bed reactor. For this I need to specify user defined drag coefficient in phase interaction window of fluent. Since drag coefficient is to specify between all three phases mutually, therefore I can't remove third phase and thus can't use porosity model for that. To specify drag coefficient between three phases, I need to do simulation with 3 phase eulerian. Now, the problem is that solid phase is present in volume fraction of 0.605 in reactor, but I don't know how to specify the velocity of solid phase as zero inside the reactor while its volume fraction is zero at inlet (due to zero velocity)? I hope you got my point.. 

October 16, 2014, 02:18 

#6 
Senior Member
Cees Haringa
Join Date: May 2013
Location: Delft
Posts: 607
Rep Power: 0 
That sounds like a very complicated problem to me; as soon as you impose a force on the particle phase there is little reason for it not to start flowing; maybe you have to give the particles infinite mass or something
Otherwise, there may be solutions with UDFs  perhaps you could write a UDF that forces the particle phase velocity to be 0 regardless of the drag acting on it. Furthermore, you may be able to write codes that assure that only gas and liquid can pass inlets and outlets, similar to the degassing boundary condition that acts as an outlet for gas but a freeshear wall for liquid... Good luck! 

October 16, 2014, 02:36 

#7 
New Member
Mechanical Engineer
Join Date: Sep 2014
Posts: 11
Rep Power: 11 
Sure, its interesting
But do you have any idea what sort of udf do I need to write in order to fix the velocity of solid phase as zero? 

October 16, 2014, 02:41 

#8 
Senior Member
Cees Haringa
Join Date: May 2013
Location: Delft
Posts: 607
Rep Power: 0 
At the moment, no idea. I don't think there are many people using CFD software to set a velocity field to 0 in the whole domain, for that matter... So I guess you'd have to find out if it is even possible first.


October 16, 2014, 02:49 

#9 
New Member
Mechanical Engineer
Join Date: Sep 2014
Posts: 11
Rep Power: 11 
I am pretty sure its already done, it has been mentioned in this paper
"CFD study andexperimental validationof trickle bed hydrodynamics under gas,liquid and gas/liquid alternating cyclic operations" Its described on 3rd and 4th page of the paper, but I am not sure how to do it 

October 16, 2014, 02:51 

#10 
Senior Member
Cees Haringa
Join Date: May 2013
Location: Delft
Posts: 607
Rep Power: 0 
Maybe you can contact the authors of that paper?


October 16, 2014, 03:01 

#11 
New Member
Mechanical Engineer
Join Date: Sep 2014
Posts: 11
Rep Power: 11 
I have just found it.
Cell zone condition>mark Fixed Values and then put values of x and y velocities to zero Thanks for your support CeesH. 

October 16, 2014, 03:04 

#12 
Senior Member
Cees Haringa
Join Date: May 2013
Location: Delft
Posts: 607
Rep Power: 0 
Haha, no need to thank me, in the end you found it
Thanks for sharing the solution! 

January 30, 2015, 12:45 

#13 
Senior Member
Join Date: May 2011
Posts: 231
Rep Power: 16 
Hi All,
I am simulating gassolid flow with two fluid approach and I am trying to have 20% mass loading of the particle at the inlet. as it is same inlet for both phases area is not important... my air density is 1.2 kg/m3, velocity is 9.3 m/s. solid density is 2500 kg/m3 , I think velocity must be calculated but I am not sure or I can use 9.3 for solid as well? how I can calculate the uniform volume fraction of the solid at inlet while assuming constant particle to gas velocity ratio? is there any idea? thanks in advance! 

January 31, 2015, 05:50 

#14 
New Member
Mechanical Engineer
Join Date: Sep 2014
Posts: 11
Rep Power: 11 
Hi Kanarya,
I couldn't understand your question. Is it fluidized bed or fixed bed? Is solid phase fixed or being fluidized inside the domain? what do you mean by 20% loading? you used the word 'particle', are you using DPM in Eulerian phase? 

January 31, 2015, 05:58 

#15 
Senior Member
Join Date: May 2011
Posts: 231
Rep Power: 16 
Thanks for the answer. It is eulerian simulation and it is fluidised inside. And I want to have 20% solid mass loading at inlet because of that I need to calculate uniform solid volume fraction do you know how to do it?


January 31, 2015, 09:14 

#16 
New Member
Mechanical Engineer
Join Date: Sep 2014
Posts: 11
Rep Power: 11 
Hi Kanarya,
first find volume fraction of both the fluid and the solids by multiplying respective mass flow with respective density, thus you will have some number less than 1 for volume fraction (vof) of solids, then try this Try boundary conditions (phase solids) > inlet> edit> multiphase> enter vof for solids.. I hope this will work. 

January 31, 2015, 11:14 

#17  
Senior Member
Join Date: May 2011
Posts: 231
Rep Power: 16 
Hi, thanks again but I could not get it.could you please write it in a maths way (formula with alpha and U and so on)thanks
Quote:


January 31, 2015, 13:50 

#18 
New Member
Mechanical Engineer
Join Date: Sep 2014
Posts: 11
Rep Power: 11 
Hi Kanarya,
It was already very simple... but let me put it in simpler way. 1). First multiply mass flow rate of solid by density of solids and thus find volume flow rate of solids. 2) . Then multiply mass flow rate of fluid by density of fluid and thus find volume flow rate of fluid. 3) Then in order to know volume fraction of solids, divide solid volume flow rate that you found in step 1 by the summation of volume flow rates that you found in step 1 and step 2. 4). the number you will get from step 3 will be less than 1. 5). put the number you get in step 4 in the boundary conditions>inlet>(phase) solids> multiphase> volume fraction Hope you understood this time. 

February 6, 2015, 04:05 

#19 
New Member
Join Date: Sep 2014
Posts: 3
Rep Power: 11 
hi mechanical engineer..
can you show me your grid please.. i am new in fluent and interesting in case of multiphase.. i want to simulate flow in a tank, and i think your case will help me in understanding my case. 

September 12, 2017, 04:12 
solid volume fraction

#20 
New Member
Mohamed Yahya
Join Date: Jun 2015
Posts: 2
Rep Power: 0 
Hi every one
I'm using Euler Euler Multiphase flow (Interphase) between two types of glass particles. From your comments I'm able to calculate volume fraction but what's the best value of solid volume fraction which I get it from Ansys Fluent 

Tags 
eulerian, multiphase, volume fraction 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Multiphase flow (Eulerian) modeling  Umesh  FLUENT  5  December 29, 2014 10:06 
[blockMesh] nonorthogonal faces and incorrect orientation?  nennbs  OpenFOAM Meshing & Mesh Conversion  7  April 17, 2013 05:42 
Multiphase Settling in 2D Container  Volume Fraction?  Hawkeye  FLUENT  1  March 29, 2012 12:03 
air bubble is disappear increasing time using vof  xujjun  CFX  9  June 9, 2009 07:59 
fluent add additional zones for the mesh file  SSL  FLUENT  2  January 26, 2008 11:55 