[Maryam1988]

Dear Foamers,

I have a problem while solving alpha equation using MULES algorithm in multiphaseEulerFoam. In some cases of mine I received alpha more than 1 and sometimes less than zero . How is it possible since I specified psiMin and psiMax to be 0 and 1.

Is there anybody who knows the reasons? Could you help me to fix the problem?
I already checked my initial and boundary conditions

Thanks alot

[TobiF]

Hey Maryam1988,
I'm facing an similar problem here. I want to simulate solid phase in gas phase but cannot manage to set the final phasefractions the right way.

Did you manage to set values for alpha.min and alpha.max for each phase? Is this even possible?

Any help would be great!

Regards Tobias

[kwardle]

What kind of mesh are you using? I have found that phase fraction boundedness is much improved in multiphaseEulerFoam when using a clean all hex mesh rather than poly or tet.

[TobiF]

Hey Kent,
I'm using a clean hex mesh created with blockMesh at the moment.

My problem was that I used a wrong type for drag force setup.
SchillerNaumann could not calculate the right phasefraction while simulation solidphase with two different fluid phases in my case.

Now, using Gidaspow, everthing is looking fine.

I could not see any problems depending on mesh quality/mesh type till now, but maybe I'll face this prob when using meshes created with shm.

Will let you know!

Regards Tobi

[kwardle]

Yes, selection and setup of drag formulation is also sensitive for this solver. It sometimes experiences instabilities for regions where the dispersed phase fraction or the relative velocity go to zero. This is why there are extra parameters in the setup in transportProperties for residualPhaseFraction and residualSlip. You can have a look at how these are included in the code. I think the default in most of the tutorials is 1e-3 for both, but in some cases increasing the value of residualPhaseFraction to 5e-3 improved stability.

[TobiF]

Hello Kent,

it seems that you have experience simulating with multiEuler?
So maybe you can help me with another problem coming up at the moment.

I'm simulating with Gidaspow-drag force and want to calculate solid material (spheres with 1mm diameter) falling into water.

I set the residual phasefraction between solid and water as
0.65 for the solid phase (65% solid and 35% water)

But at the moment when the solid phase hits the bottom wall, solidphasefraction goes up 0.9, but it should stay at 0.65.

Is it possible to set this phasefraction the right way?

Any hint would be great
Regards
Tobi

[kwardle]

Originally Posted by TobiF

Is it possible to set this phasefraction the right way?

As I said above, the parameters residualPhaseFraction and residualSlip are intended to be numerical crutches only to help the coupled formulation keep numerical stable. They were not intended to provide constraints on phase fraction in the way you are attempting. Have a look at the code, they are not included in the calculation of the actual phase fractions or velocities, ONLY in the calculation of the drag force itself.

If the solids are settling in your system, then it is not surprising that the volume fractions at the bottom would be higher than in the bulk.

[TobiF]

Thanks for your reply,

if these parameters are just for stability, is it even possible to set an alpha.min oder alpha.max for the different phases?

If I want to simulate real particle behavior, phasefractions higher 0.6 or even 0.7 aren't realistic, so I set these values with setFields at the beginning.

I've tried different particle-solvers with good results but as the meshes are getting more complex and particle numbers are rising simulations take much too long.

(next step should be combination with dynamic meshes - here you have, depending on included particle classes problems with automapping)

[kwardle]

You are referring to something like a maximum packing fraction. No, at the moment that part was never implemented as the target for the development was initially liquid-liquid-gas flows and not solids. It may be that a piece of packing limiter code is still hanging out in the solver folder, but it is not used. The standard solver would have to be modified to include this. Should not be terribly difficult.

[TobiF]

Hello Kent,
thanks for your answer!!
Yes, you're right - this is exactly what I wanna do.

Do you know if this function was implemented in some older versions of OF?

And may it be possible to use fvOptions for such a limiter function?

Regards Tobi

[kwardle]

fvOptions will not work with the phase fractions. Yes, you should be able to find packingLimiter.H file in some previous versions of twoPhaseEulerFoam. You may be able to borrow something from here. The solution of the volume fraction equations is done in multiphaseSystem/multiphaseSystem.C in multiphaseEulerFoam so you probably have to implement your max volume fraction there.

[TobiF]

Thanks Kent for that reply.

I will have a look on it the next days and let you know in I get it working!

Regards Tobi

[bbita]

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. I appreciate your help.

[kwardle]

Originally Posted by bbita

In my problem, both phases are dispersed.

Unless you have a third phase, I am not clear how both can be dispersed.
Perhaps you mean that there are regions where the phases are inverted (one dispersed in the other)? The current solver is not able to capture phase inversion. You can use a so-called 'blended' drag formulation which essentially computes the drag force with a volume fraction weighted average of treating each phase being dispersed. This is intended to capture the case where there are regions where one phase is dispersed and regions where it is continuous. However, this does NOT capture viscosity changes which could be significant as you go through phase inversion depending on what type of phases and flow you have.

[bbita]

Dear Kent,

Thanks for your note. In my problem, I have static water and oil inside a capillary tube. By defining the contact angle and running interFoam, I could see the formation of the curvature due to wettability. In interFoam, I only needed to enter viscosity, density, and contact angle. I tried to model the same thing with eulerFoam but the interface doesn't have the same shape.

[kwardle]

If you mean twoPhaseEulerFoam, this does not have any interface or interfacial tension so this problem is not right for that solver. If you mean multiphaseEulerFoam, you can specify an interFoam-like compressed interface with surface tension, but for two phases only, there would be no advantage over interFoam. In fact, with multiphaseEulerFoam there are some other threads here that talk about problems with interfacial tension implementation in certain versions.
The problem you describe seems to be best captured with interFoam. Why are you even trying to use "eulerFoam"?

[bbita]

Dear Kent,

The oil I modelled has a very high viscosity and therefore there is a huge difference between viscosity of oil and water. It seems interFoam cannot capture this system (alpha.water is higher than one in some specific area!!) I thought maybe multiphaseEulerFoam can model this system. I appreciate your suggestions.

[kwardle]

multiphaseEulerFoam will not do better on this problem. A couple things to consider:
- Be careful on your mesh. Clean hex mesh will be required and you will need high resolution in the interface region to capture curvature.
- If you are getting issues with unbounded volume fraction be sure to check that there are no other problems with your setup such as inconsistent boundary conditions or sub-optimal settings in fvSchemes
- Compressive schemes like used in interFoam may not be the best choice if your problem is interfacial tension driven. (Also make sure cAlpha = 1 and not greater as in some of the tutorials, this will only make interface numerical problems worse.) Not sure what version of OF you are using, but I did notice in the recent release of v1706 (ESI version from openfoam.com) there is implemented an interface reconstruction scheme (similar to PLIC in Fluent). Solver is called interIsoFoam. This MAY do better on this problem, but it could also be more sensitive to mass loss. I have not studied the specifics of the implementation so I am not sure how they have tackled this aspect.

Good Luck!

[bbita]

Dear Kent,

Many thanks for your suggestions. I am using the last version of OpenFoam (v1706). I will come back to you with the results.

[bbita]

Dear Kent,

I checked the points you mentioned, in addition to interIsoFoam and interDyMFoam and none of them works. I also activate momentum predictor as suggested on another thread and it doesn't work as well. I am not sure if VOF method is appropriate in systems with a high viscosity difference.