[nov.t]

Hello Foamers,

I am using multiphaseEulerFoam (ver. 2.2) for the multiphase jet flow.

I want to specify the continuous and dispersed phase in calculating the drag force between each phase.

I found that it is possible to determine the continuous/dispersed phase in twoPhaseEulerFoam (ver. 2.3) as follows (but this is the case of virtual mass force):

virtualMass
(
(water in air) // water droplets dispersed in air
{
type constantCoefficient;
Cvm 0.5;
}
);

http://www.openfoam.org/version2.3.0/multiphase.php

Is it possible to specify the phases in multiphaseEulerFoam 2.2.x ?
Please give me your knowledge.

Best regards,
nov.t

[dschmidt]

Hi nov.t,

as far as I know, the phases are read from the interface dict from left to right.

        
dragModel
        (
            const dictionary& interfaceDict,
            const phaseModel& phase1,
            const phaseModel& phase2
        );

so: (air water)
air=phase1
water=phase2


From e.g. SchillerNaumann drag you can see that phase1 is the dispersed phase, as its diameter is used for the calculation of Re (phase1_.d()).

  volScalarField Re(max(Ur*phase1_.d()/phase2_.nu(), scalar(1.0e-3)));

From the continuous phase (phase2,water) the kinematic viscosity is used (phase2_.nu()).


In short:
(air water) => (air in water)


Hope this clarifies it for you.

Regards,
Dominik

[nov.t]

Dear dschmidt,

Thank you for replying.

Is the phase1 always the dispersed phase?

When I used the "blended" type for the drag in transportProperties as following code, phase inversion is considered.

drag
(
    (air water)
    {
        type blended;

        air
        {
            type SchillerNaumann;
            residualPhaseFraction 0;
            residualSlip 0;
        }

        water
        {
            type SchillerNaumann;
            residualPhaseFraction 0;
            residualSlip 0;
        }

        residualPhaseFraction 1e-3;
        residualSlip 1e-3;
    }
)

So I think the drag force calculation was carried out for both cases. (If I was wrong, sorry.)
(case A: continuous = air, dispersed = water, and case B: continuous = water, dispersed = air)

Is there different type along with "blended" ?


Best regards,

nov.t

[dschmidt]

Yes, when using blended the solver automatically weights the drag forces based on the phase fraction, so both drag forces are calculated
and different models for each dispersed phase can be chosen.

return phase2()*dragModel1_->K(Ur) + phase1()*dragModel2_->K(Ur)

phase1() and phase2() are the phase fractions of each phase.

[nov.t]

Dear dschmidt,

Thank you for explaining the blended model, and I could understood about it.

However, I want to fix the two dispersed phases (air, oil) in the three-phase flow (continuous phase is water).

Present setting is as follows:

drag
(
    (air water)
    {
        type blended;

        air
        {
            type SchillerNaumann;
            residualPhaseFraction 0;
            residualSlip 0;
        }

        water
        {
            type SchillerNaumann;
            residualPhaseFraction 0;
            residualSlip 0;
        }

        residualPhaseFraction 1e-3;
        residualSlip 1e-3;
    }
 
   (oil water)
    {
        type blended;

        oil
        {
            type SchillerNaumann;
            residualPhaseFraction 0;
            residualSlip 0;
        }

        water
        {
            type SchillerNaumann;
            residualPhaseFraction 0;
            residualSlip 0;
        }

        residualPhaseFraction 1e-3;
        residualSlip 1e-3;
    }

   (oil air)
    {
        type blended;

        oil
        {
            type SchillerNaumann;
            residualPhaseFraction 0;
            residualSlip 0;
        }

        air
        {
            type SchillerNaumann;
            residualPhaseFraction 0;
            residualSlip 0;
        }

        residualPhaseFraction 1e-3;
        residualSlip 1e-3;
    }

);

To fix the dispersed phases definitely, I think blended model is not appropriate.
So I am finding the different approach without using the blended type.

thank you.

Best regards,

nov.t

[dschmidt]

 (dispersedPhase contPhase)
    {
        type SchillerNaumann;

        residualPhaseFraction 1e-3;
        residualSlip 1e-3;
    }

... set dispersedPhase & contPhase as needed: e.g. (air water) ... air dispersed in water.

[nov.t]

Dear dschmidt,

I understood, I realized it was simple problem... Thank you.

[vonboett]

Dear Foamers,

Is there a good validation case around for multiphaseEulerFoam?

[foamiste]

Dear vonboett,

Did you find any information about multiphaseEulerFoam?

[vonboett]

well at least some, the best overview for me was available here:
http://documents.mx/documents/cfd-si...ous-media.html

but there are others like "Numerical Investigation of Vertical Plunging Jet Using a Hybrid Multifluid–VOF Multiphase CFD Solver" by Olabanji Y. Shonibare and Kent E. Wardle (2015) or "Hybrid Multiphase CFD Solver for Coupled Dispersed/Segregated Flows in Liquid-Liquid Extraction" by Kent E. Wardle and Henry G. Weller (2015). My problem is that I implemented the transportModels so you can model Non-Newtonian rheologies, but I get a fluctuating interface between my air phase and my other components that is somehow oscillating in a way I do not observe with interFoam (or interMixingFoam). The dambreak test case works fine, (and the coupling to a lagrangian particle simulation in a way like in DPMFoam using kinematicCollidingCloud worked quite well, too) so the interface behavior is the only thing that worries me. I played around with the sigmas but the problem remained.

[nic92]

Hi guys,

I need to simulate a gas-oil-water flows, with gas the continuous phase, water and oil dispersed ones. After having a look at the code of multiphaseEulerFoam (specifically, UEqn), I think that the momentum exchange term among phases is counted for the dispersed phases and continuous and not between the dispersed phases. The influence of a disperse phase on the other one is negligible when I do not have a separation process, however in my case there is a time after which oil and water's domain is in contact and through this interface, mometum is surely exchange.
Do you agree with my conclusion concernig with this solver?

For example, in the twoPhaseEulerFoam, the drag term is counted as k_{d12}(U_1-U_2) for phase1 and k_{d21}(U_2-U_1) for phase2. In this way, both phases are treated without specifying which one is the dispersed or the continous one. On the other hand, in MFE, if 1 is the continuous phase and 2 and 3 the disperse ones, the drag term is counted as k_{d12}(U_1-U_2) and k_{d13}(U_1-U_3).

Thanks in advance.

[vonboett]

Wardle & Weller (2013):
"In this solver, calculation of the drag coefficient can be done by specifying a dispersed phase or by independent calculation with each phase as the “dispersed phase” and the overall drag coefficient applied to the momentum equations taken as the volume fraction weighted average of the two values. This is a so-called blended scheme which is a useful approximation for flows with regions in which either phase is the primary phase"

[nic92]

Thanks for your answer. I made a mistake.
Do you think that the same holds also for the virtual mass force?
I mean in twoPhaseEulerFoam the blending function is applied to each of the momentum exchange term. On the other hand in MFE, the blended function is applied only on the drag term.
Moreover, here the blended function is an average base on phase fraction, whereas in TFE the blended function is hyperbolic or linear.

Thanks in advance

[vishal3]

Originally Posted by nic92

Hi guys,

I need to simulate a gas-oil-water flows, with gas the continuous phase, water and oil dispersed ones. After having a look at the code of multiphaseEulerFoam (specifically, UEqn), I think that the momentum exchange term among phases is counted for the dispersed phases and continuous and not between the dispersed phases. The influence of a disperse phase on the other one is negligible when I do not have a separation process, however in my case there is a time after which oil and water's domain is in contact and through this interface, mometum is surely exchange.
Do you agree with my conclusion concernig with this solver?

For example, in the twoPhaseEulerFoam, the drag term is counted as k_{d12}(U_1-U_2) for phase1 and k_{d21}(U_2-U_1) for phase2. In this way, both phases are treated without specifying which one is the dispersed or the continous one. On the other hand, in MFE, if 1 is the continuous phase and 2 and 3 the disperse ones, the drag term is counted as k_{d12}(U_1-U_2) and k_{d13}(U_1-U_3).

Thanks in advance.

Dear nic92,

I am looking into the formulation details of the twoPhaseEulerFOam and come across this post. In OpenFOAM, the momentum transfer due to the drag force is defined in terms of k_{d13}(U_1-U_3). I was interested in knowing that what is the relationship between this term and drag coefficient. How drag coefficient is taken into account while solving this term?
I need the exact formulation for k, which includes drag coefficient.


Thanking you,

[vonboett]

there are many drag models, depending on your "phase particles" or other characteristics of you flow. They are in multiphaseEulerFoam/interfacialModels/dragModels.

You may find related drag models implemented in the lagrangian libraries, for solvers that couple continuous phase fluids solved by the Navier-Stokes eqns. with Lagrangian particle solvers, and maybe you find more comments about how the drag coefficients work searching among those solver discussions.

[bbita]

Dear Foamers,
I did some modelling for oil and water in a single tube with interFoam (with specific contact angle). I want to model the same thing with eulerFoam as it has momentum equation for both phases. In my problem, both phases are dispersed and I don't want to include any drag force for now. I appreciate your help.

[vonboett]

...well the phases are coupled by drag. Maybe what you are looking for is the mixed interFOAm/Euler OpenFOAM solver developed by:
Wardle, K. E. and Weller, H.: Hybrid Multiphase CFD Solver for Coupled Dispersed/Segregated Flows in Liquid-Liquid Extraction, Int. J.
Chem. Eng., p. 128936, doi:10.1155/2013/128936, 2013.

With that solver, I experienced some difficulties with the free surface though and it is not accounting for non-Newtonian rheologies, however, that was easy to implement, I can send you the code if you like. Still, one should carefully validate this solver before use because it has many parameters and one can easily get in a mess.

[bbita]

Dear Albrecht,

Sure, I will test the solver and let you know if it works for my case.

[MT Scelzo]

Originally Posted by vonboett

there are many drag models, depending on your "phase particles" or other characteristics of you flow. They are in multiphaseEulerFoam/interfacialModels/dragModels.

You may find related drag models implemented in the lagrangian libraries, for solvers that couple continuous phase fluids solved by the Navier-Stokes eqns. with Lagrangian particle solvers, and maybe you find more comments about how the drag coefficients work searching among those solver discussions.

Dear all,



I am checking the calculation of the drag force in
reactingTwoPhaseEulerFoam OF 4.0.



I am in the folder multiphase/reacitngEulerFoam/interfacialModels/dragModels/dragModel.


In dragModel.C, I don't see the density of the dispersed phase in the definition of K.


EDIT: It should not be there because it multiplies the momentum equation. The dimensions are consistent.

[vishalgarg474]

Why aren't there same blended libraries in multiphaseEulerFoam as twoPhaseEulerFoam?



As I understand they should both give same results when blending methods are used. But they do not.



I tried to look into the drag parameter coefficients and the values are different when I test the same case on twoPhaseEulerFoam and multiphaseEulerFoam.


Can somebody please shed some light on this?


Thank you