
[Sponsors] 
October 24, 2011, 08:14 
Slurry (sand water) flow in twoPhaseEulerFlow possible?

#1 
New Member
Jochem van den Bosch
Join Date: Oct 2011
Location: Rotterdam, The Netherlands
Posts: 20
Rep Power: 7 
Hi everybody,
As a part of my MSc. thesis I am trying to model a slurry flow (sand/water) in OpenFOAM (for different geometries). I heard that i could best use the twoPhaseEulerFlow solver for this problem, however I have found only examples regarded pneumatic conveying in combination for this solver. Can this solver also be used for a liquid/solid interface. Some specifics of my research are: Turbulent flow (Re>>2300) Pipe flow Sand (2600kg/m^3), water mixture Concentrations ranging from 10 to 40% Medium fine sand, d50 approximately 300600 micrometer I am particularly interested in the pressure drop allong the length of the pipe. Is the twoPhaseEulerFlow the right solver to use and do you think I would have to adjust this solver. If it is not the one to use, which one should I use. Thanks so much in advance!!! Best regards! 

October 26, 2011, 11:27 

#2 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
Yes, it should work. The code might present some instability if particles pack. Please, search the forum for discussions on the topic.
__________________
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 27, 2011, 03:21 

#3 
New Member
Jochem van den Bosch
Join Date: Oct 2011
Location: Rotterdam, The Netherlands
Posts: 20
Rep Power: 7 
Hi Alberto. Thanks for your response. I did some research (mostly on this forum) and for now I've decided to go with settlingFoam instead of twoPhaseEulerFoam, since the first is based on the driftflux model, which I already have some experience with (is taught by my university). Also packing might occur (not sure). settlingFoam seems more appropiate for this task (although it doesn't provide means to simulate a sliding bed...).
Do you know of any thesis' that use settlingFoam to simulate slurry flow. Thanks in advance & best regards, 

October 27, 2011, 14:26 

#4 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
OK. Just keep in mind that the algebraic slip model (mixture model) is valid for relatively low particle concentrations and it might have limitations on the Stokes number.
BTW, I am working on slurry flow with my (heavily) modified version of twoPhaseEuler, and it is working fairly well.
__________________
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 31, 2011, 05:25 

#5 
New Member
Jochem van den Bosch
Join Date: Oct 2011
Location: Rotterdam, The Netherlands
Posts: 20
Rep Power: 7 
Hi Alberto, thanks for your tips. About the mixture model for low concentration, my professor (Cees van Rhee) used this model in het PhD thesis (on the sedimentation process in a trailing suction hopper dredger) succesfully for concentrations up to 40% (sand in water). What are your thoughts about this (what do you consider a high concentration?)?
Best regards, ps. what kind of slurry flow are you working on, sand/water? And openchannel flow or pipeflow? 

October 31, 2011, 11:46 

#6 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
Hi Jochem,
as long as the hypotheses behind the model are satisfied, you can use it. Remember that the mixture model is derived making quite strong assumptions:  Local equilibrium among the phases, which limits the validity to low Stokes numbers  Mixture hypothesis, which limits the property ratio of the phases When it comes to fluidparticle flows, the mixture model is suggested in case the particle loading is "low". How low depends on the flow conditions, but since you do not consider particleparticle interactions, I would say ~10%. You find applications with much higher concentrations, however. There are doubts on the validity of the model under those conditions however. I deal with slurry flow in ducts (high St number). 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. 

December 18, 2015, 08:09 

#7 
Member
Ali
Join Date: Oct 2013
Location: Scotland
Posts: 55
Rep Power: 5 
Hi both,
In regards to the original question, is there an EulerEuler solver available for particle/fluid flow? I'm using twoPhaseEulerFoam, but I don't like how I have to include temperature. The openFoam website says the model is incompressible, but it clearly isn't. Any help is appreciated! regards 

December 26, 2015, 00:03 

#8 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
This has been addressed in reactingTwoPhaseEulerFoam (OF 3.0.x or dev from the Foundation). You can set phases to be isothermal, and the energy equation won't be solved.
The model can be compressible or incompressible, depending on how you set the thermodynamic properties of the phases (see fluidisedBed tutorial, where the solid phase is incompressible).
__________________
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. Last edited by alberto; December 26, 2015 at 00:05. Reason: Added consideration on compressibility 

January 5, 2016, 09:58 

#9 
Member
Ali
Join Date: Oct 2013
Location: Scotland
Posts: 55
Rep Power: 5 
Thanks for your reply Alberto. I'm using 2.3.x, so I’ll upgrade.
I'm planning on combining this solver with DPMFoam, have you heard of anything else like this? Combining two solvers I mean... For example solver A running in the top of the domain, and solver B running in the bottom of the domain. I think it will be tricky, but not impossible. Your help is appreciated! regards 

March 18, 2016, 12:27 

#10  
Senior Member
Ruben Di Battista
Join Date: May 2013
Location: Milan
Posts: 111
Rep Power: 6 
Quote:
How do I set the phases isothermal? I tried to set up the diameterModel as isothermal and minIter for the energy equation to 0 but it stills continue to solve energy for both phases. 

March 24, 2016, 08:23 

#11 
Member
Ali
Join Date: Oct 2013
Location: Scotland
Posts: 55
Rep Power: 5 
Ruben, see below:
http://www.cfdonline.com/Forums/ope...tml#post580432 

March 30, 2016, 05:27 

#12  
Senior Member
Ruben Di Battista
Join Date: May 2013
Location: Milan
Posts: 111
Rep Power: 6 
Quote:


November 15, 2016, 22:27 

#13 
New Member
Bryant
Join Date: Mar 2015
Posts: 6
Rep Power: 4 
Hi everyone,
I'm interested in the topic of particle/fluid flow. Now I want to simulate the dry particle (above water surface in the beginning) flows into water. Is it possible to use twoPhaseEulerFoam to simulate this phenominon? For this problem, I want to capture the free surface of particle flow and water flow, and ignore the effect of the air. Thanks in advance! BR 

November 16, 2016, 11:35 

#14  
Senior Member
Ruben Di Battista
Join Date: May 2013
Location: Milan
Posts: 111
Rep Power: 6 
Quote:


November 16, 2016, 20:33 

#15 
New Member
Bryant
Join Date: Mar 2015
Posts: 6
Rep Power: 4 
Hi Ruben,
Thanks for your quick reply. VOF is indeed a good way for freesurface problem. But I want to simulate the interactions between particle and fluid, and use Kinetic theory to simulate interactions between particles. So I want to make some modifications based on interfoam or twoPhaseEulerFoam. Do you think which is easier to implement, 1) Adding KT part into interFoam or 2) Adding a freesurface capturing part into twoPhaseEulerFoam? Thanks 

November 17, 2016, 13:09 

#16  
Senior Member
Ruben Di Battista
Join Date: May 2013
Location: Milan
Posts: 111
Rep Power: 6 
Quote:
By the way I would choose the starting solver on the base of which of the two phenomenon is more important to your case. 

November 19, 2016, 19:26 

#17  
Member
Patricio Bohorquez
Join Date: Mar 2009
Location: Jaén, Spain
Posts: 95
Rep Power: 10 
Quote:
Bohorquez, P. Finite volume method for falling liquid films carrying monodisperse spheres in Newtonian regime. AIChE Journal, 58: 2601–2616, 2012 PDF doi:10.1002/aic.13863 

November 30, 2016, 10:16 
multiphase flow in cyclone

#18 
Member
ali
Join Date: Jul 2016
Posts: 70
Rep Power: 2 
Dear All,
I want to simulate multiphase flow of cyclone in OpenFOAM. I am working on slurry flow that its parameters are as fallows: Particle size distribution= <70 micron %solid of slurry= 7075% %water of slurry= 2530% When flow is pumped to cyclone, Air core is created inside cyclone. There are 3 type phase in cyclone: particle + water + air. 1 What solver is suitable for this flow? twophaseEulerFoam? or settlingFoam? or ...? 2 For example If twophaseEulerFoam solver is Ok, How will I enter the Lagrangian (particle) phase? Please guide about the folders (0 , constant , system) and their parameters. 3 I will use Mixture model, Is there the model in twophaseEulerFoam solver? Thanks in advance. Ali 

December 1, 2016, 10:05 

#19  
Senior Member
Ruben Di Battista
Join Date: May 2013
Location: Milan
Posts: 111
Rep Power: 6 
Quote:
There is not an "above all" solver. It depends on how do you want to model the different phases and on how high is the concentration of each of them. Did you check the solvers list? There is driftFluxFoam that, as it is written there, Quote:
To understand how the folders are organized, check the tutorial folder of OpenFOAM. 

December 1, 2016, 17:33 

#20 
Member
ali
Join Date: Jul 2016
Posts: 70
Rep Power: 2 
Thanks for your reply, I will to use twophaseEulerFoam solver with two phases [air + slurry] but the slurry contains water and fine particles (<70 micron)...!
Now, 1 how do I import the particles here so the solver can solve it? 2 Which solver can you suggest for this case? Thanks, Ali 

Tags 
pipe flow, sand & water, slurry flow, turbulent flow, twophaseeulerfoam 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Flow meter Design  CD adapco Group Marketing  CDadapco  3  June 21, 2011 08:33 
Can OpenFOAM generate flow at the speed of light?  Michel_sharp  OpenFOAM  6  October 24, 2009 04:09 
mass flow in is not equal to mass flow out  saii  CFX  2  September 18, 2009 08:07 
What is the difference between liquid reactive flow and gas reactive flow?  James  Main CFD Forum  6  May 15, 2009 12:14 
transform navierstokes eq. to eulereq.  pxyz  Main CFD Forum  37  July 7, 2006 08:42 