[paul]

Hello everyone,

Does anyone have an documentation (ie. journals/theses) on the twoPhaseEulerFoam solver?

Thank you in advance,

Paul Lucente

[alberto]

Hello Paul,
the solution algorithm is explained in Henrik Rusche's Ph.D. thesis:

http://powerlab.fsb.hr/ped/kturbo/Op...chePhD2002.pdf

The algorithm was actually developed for bubble flow, and the resulting solver was bubbleFoam, of which twoPhaseEulerFoam is an extension.

If you need more information, ask here :-)

Regards,
A.

[paul]

Alberto,

I'm having problems with the particle-particle magnitude force (PPMagf) equation, which is in the alphaEqn.H file.

I am very new with this software as well as this type of fluid dynamics. I'm using the bed example and changing it to a liquid-solid settling model. When I include the packing limiter I get a Floating exception error (I'm assuming a division by zero). When I turn the packing limiter off the solids fraction rises above the packing limit and in some other locations I also get a negative solids fraction.

Do you have any suggestions?

Thank you,
Paul

[minzhang]

Hello Paul,

I am wondering whether you worked your problem out at the end, and whether you could direct me to your papers/thesis for reference.

Here, I want to use twoPhaseEulerFoam to simulate a solid/liquid slurry transport in long horizontal pipes like in this reference.
Yang, Yan, Haoping Peng, and Chuang Wen. "Sand transport and deposition behaviour in subsea pipelines for flow assurance." Energies 12.21 (2019): 4070.

Your valuable comments would be greatly appreciated!

Thanks!
Min

Originally Posted by paul

Alberto,

I'm having problems with the particle-particle magnitude force (PPMagf) equation, which is in the alphaEqn.H file.

I am very new with this software as well as this type of fluid dynamics. I'm using the bed example and changing it to a liquid-solid settling model. When I include the packing limiter I get a Floating exception error (I'm assuming a division by zero). When I turn the packing limiter off the solids fraction rises above the packing limit and in some other locations I also get a negative solids fraction.

Do you have any suggestions?

Thank you,
Paul

[alberto]

Dear Paul,
I know these problems, and only a significant change in the solution algorithm can reduce them reliably. You can find some more information about this searching the discussion board, and in the MFIX documentation www.mfix.org.

About your case, if you need to simulate settling, there is also another solver in openFOAM: settlingFoam. Some theoretical background is here:

http://powerlab.fsb.hr/ped/kturbo/Op...BrennanPhD.pdf

With kind regards,
Alberto

[paul]

Sorry about all these questions.

The kineticTheoryModel.C file refers to a paper (ie. Line 226 - "particle pressure - coefficient in front of Theta (Eq. 3.22, p. 45)). I was wondering if you happen to know what paper they are refering to.

Thank you again,

Paul

[alberto]

Hello Paul,
that annotation just means you calculate the "coefficient" of the granular pressure you have to put in the term:

fvm::SuSp(-((PsCoeff*I) && dU), Theta_)

of the transport equation for the granular temperature.

The coefficient is simply Ps/Theta_, because Theta_ is already present in the SuSp, as a separate argument, being the variable you solve for.

With kind regards,
Alberto

[paul]

Hello Alberto,

I'm still curious to know what paper they are refering to. I've tried searching for this bed example on the internet I haven't been able to find it. I'm curious because there a few other references to this paper in that same kineticTheoryModel.C file.
Basically I would like to get a better understanding of the solution steps.

Thank you again,

Paul

[alberto]

The reference is Berend Van Wachem Ph.D. thesis I think, who is a professor at Chalmers University now.

With kind regards,
Alberto

[juho]

Alberto,

You said it would need a significant change in the solution algorithm to overcome the overpacking problems.

Have you outlined what the significant change should be? Even roughly?

I have to use a very small timestep to keep the packing under alphaMax. Down to 1e-6s, whitch makes the calculation impossibly slow.

Even with the packing limiter enabled it will overpack. I've actually got the limiter kicking in at 1e-2 before the alphaMax to get slightly longer steps.

In the kineticTheory.C the call for G0 is limited by min(alpha,alphaMax - 1e-2). I tried a limit of (alphaMax - 1e-3), but it made things even worse.

Juho

[alberto]

Hello Juho,

the problems you're facing are due to the explicit treatment of the granular pressure in the current solver.

To my knowledge, there are mainly two approaches used to stabilize the solution when the particle phase reaches the packing limit, at least in well known codes (FLUENT, MFIX, ...).

The first one is to make the particulate phase incompressible when the packing is reached, which means you solve a pressure equation for the particulate phase too. You then use the granular pressure predicted by the kinetic theory when the flow is not packed, and the pressure given by the pressure equation when the flow is packed.

The second solution is the one adopted in MFIX (see details in their documentation on www.mfix.org, or in Mathijs Goldschmidt, "Hydrodynamic Modelling of Fluidised Bed Spray Granulation", Twente University Press), where a particle phase fraction correction equation is used instead of the continuity equation for the particulate phase, to sensitize it to the granular pressure.

Both these algorithms are based on SIMPLE, with internal iterations to be able to apply under-relaxation. Probably the first one is the less intrusive to implement, but you need to find a way to workaround the singularity in the pressure equation you have when the particulate phase fraction tends to zero.

If you need further information, just ask or drop an email.

Regards,
Alberto

[juho]

Thank you!

I'll look into those to see if I get a handle on how to implement them. Studying MFIX documentation ja transientSimpleFoam at the moment. I may have to bother you again...

Although at the moment there's no overpacking in areas of interest with timestep of 3e-5s.

Regards,
Juho

[sradl]

Dear Foamers,

I found some inconsistencies between the actual OpenFOAM implementation (TwoPhaseEulerFoam as well as bubbleFoam) and the PhD Thesis of Rusche. It is about the treatment of pressure.

In the PhD of Rusche he discusses on p. 121 the boundary conditions for pressure at walls. He states that he removes the hydrostatic pressure from the total pressure to simplify the pressure boundary condition, i.e., to use zeroGradient. By doing so, the gravity term in the continuous phase equation vanishes (his Eqn. 3.71) and the pressure is replaced by the "modified mixture pressure" p* = p - rho_b . g . x.

However, in the current OF implementations the gravity term is still included (not in UEqn.H but later in the pEqn.H where it is added via the phiDrag-terms). Also, the results include the hydrostatic pressure, but still are using the zeroGradient BC for pressure.

So I have the following questions:

- why the current implementation works with zeroGradient BC, as it should not.

- Rusche's definition of p* = p - rho_b . g . x is generally not applicable to a mixture, as the pressure gradient is proportional to rho_b . g . eps_b. So I don't see the rationale why p* is defined as it is.

I'd appreciate any clarification on this,

br
Stefan Radl

[Edy]

Hi Sefan Radl,

I am actually quite confused about the implementation of the pressure in twoPhaseEulerFoam which is different than what Rusche explains in his thesis.

If "p" in the solver represents the modified pressure, why then gravity still appears (as a term transfered from the UEqn.H to the pEqn.H)?

I hope that you found the answer to this question after this long time and that you'll be able to help me.

Thanks in advance!
Best,

Edy

[alberto]

bubbleFoam / twoPhaseEulerFoam do not solve for the modified pressure, but for the actual pressure. You can easily obtain the pressure equation used in the code dividing each continuity equation by the corresponding phase material density and summing them up.

Further information here: http://openfoamwiki.net/index.php/Bu...ssure_equation

Best,

[Edy]

Hi Alberto,

Thanks a lot for your answer and link. I just started using OF and there are still many things that are unclear to me...

Your link was quite useful and now I understand, i think, the role of the pressure equation. However i still have few questions :

1) Tell me if I am wrong but the terms to be transfered to the pressure equation are the one in which appears a gradient term, cause letting gradient terms in the RHS of the momentum equation would cause numerical calculation problems such as oscillations and loss of continuity. Am i right? Then I understand why the pressure gradient and the turbulent dispersion force (in which appears grad(alpha)) are transfered, but why the gravity g too??

2) Since twoPhaseEulerFoam considers the actual pressure, the BC at the wall should not be zeroGradient, right? I think I'd better use buoyantPressure, but then I have an issue concerning the density to use. The wall is ,in my case, heated and void fraction can be relatively high, so taking the liquid density does not appear as the best solution to me. Perhaps to take a kind of mixture density would be more appropriate. I do not really know how this BC patch works...

I would be very grateful if you could provide some insight into these two issues.
Thanks a lot!

Best regards,

/Edouard

[alberto]

Originally Posted by Edy

The pressure equation. However i still have few questions :

1) Tell me if I am wrong but the terms to be transfered to the pressure equation are the one in which appears a gradient term, cause letting gradient terms in the RHS of the momentum equation would cause numerical calculation problems such as oscillations and loss of continuity. Am i right? Then I understand why the pressure gradient and the turbulent dispersion force (in which appears grad(alpha)) are transfered, but why the gravity g too??

The gravity term, as well as the explicit part of the drag term are "transferred to the pressure equation" since they are included in the interpolation formula to stabilize the numerical procedure when there are sharp changes in the volume fraction. Some Author called this "improved Rhie-Chow interpolation".

2) Since twoPhaseEulerFoam considers the actual pressure, the BC at the wall should not be zeroGradient, right? I think I'd better use buoyantPressure, but then I have an issue concerning the density to use. The wall is ,in my case, heated and void fraction can be relatively high, so taking the liquid density does not appear as the best solution to me. Perhaps to take a kind of mixture density would be more appropriate. I do not really know how this BC patch works...

The buoyantPressure BC is exactly a zeroGradient BC if p is not p_rgh. You might want to take a look at the code.

Best,

[Edy]

Hi Alberto,

Thanks again for taking some time and answer my questions!

Ok, so transferring the explicit part of the drag term to the pEqn will stabilize the procedure. I am trying to understant all that because I am modeling a two phase Eulerian model for nucleate subcooled boiling. And therefore I have additional terms in my momentum equations due to phase change. But I dont know if they should be kept there or transfered to the pEqn... How to guess that transferring some terms will stabilize the procedure?

Do you have any advice?

Anyway, thanks a lot, your previous posts have been quite helpful.

Best,

/Edouard

[alberto]

What is the form of these terms? Do they change quickly with the phase fraction?

Best,

[Edy]

Hi,

Woaw, that s a quick reply !

Well, i have two terms :
- one due to evaporation at a heated wall, which is calculated using Kurul and Podowski model, and it is absolutely independent on the phase fraction
- one due to condensation in the bulk, which is directly proportional to the void fraction.

Best,

/Edouard