Slurry (sand water) flow in twoPhaseEulerFlow possible?
 

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 300-600 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!

Yes, it should work. The code might present some instability if particles pack. Please, search the forum for discussions on the topic.

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 drift-flux 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,

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.

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 open-channel flow or pipeflow?

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 fluid-particle 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 particle-particle 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,

Hi both,

In regards to the original question, is there an Euler-Euler 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

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).

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

Dear @alberto,
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.

Ruben, see below:
http://www.cfd-online.com/Forums/ope...tml#post580432

Thank you. I also managed to make it shutting down even with bare twoPhaseEulerFoam and reported it in the thread you're quoting. =)

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

I believe that if you're interested to the free surface twoPhaseEulerFoam is not the right solver. I would choose using VOF (e.g. interFoam).

Hi Ruben,

Thanks for your quick reply. VOF is indeed a good way for free-surface 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 free-surface capturing part into twoPhaseEulerFoam?

Thanks

Well, that's an hard question. Maybe more expert people will be more useful than me. In any case if I remember well in the Rusche thesis twoPhaseEulerFoam solver is based on there was also a chapter on the interface capturing.

By the way I would choose the starting solver on the base of which of the two phenomenon is more important to your case.

I did it using the mixture or drift-flux theory some years ago. What you want to do is not easy. See some details in my paper:

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

multiphase flow in cyclone
 

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= 70-75%
%water of slurry= 25-30%
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

Well, you have multiple phases. How do you want to treat those phases? You talk about "Lagrangian", then about "mixture model", than about "twoPhaseEulerFoam" that is, as the name says, an Eulerian solver. It (and the more powerful brother multiplePhaseEulerFoam) treat the different phases as Eulerian fields.

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,

.

To understand how the folders are organized, check the tutorial folder of OpenFOAM.

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