[mike.franky]

Hello,

I have recently started using OpenFOAM. Specifically, I am trying to model a multiphase/multicomponent bubble column-like problem. It seems to me that the multiphaseEulerFoam solver is perfectly suitable for this task. However, I have a couple of questions.

First, for the calculation of the interphase interactions, the Eulerian model assumes that each phase forms bubbles of a constant diameter. In the absence of any experimental data, is there any empirical model that we can use to calculate this diameter?

My second question regards the compressibility of each phase. The documentation states that the solver is for compressible fluid phases (http://cfd.direct/openfoam/user-guide/standard-solvers/). Glancing at the code however, I can see that the energy (or temperature) equation is not solved. Am I missing something?

Finally, commercial software packages often consider a multiphase model called the mixture model (or at least that is what ANSYS is calling it). This is much more efficient than its Eulerian counterpart and might be suitable for my case. Does OpenFOAM have something equivalent?

Thanks in advance for any help

Mike

[kwardle]

Mike,
1. You are correct that the solver as released can handle a constant diameter only. There is a diameterModel class to add in other models and there is one that can handle size changes of bubbles due to external pressure changes. There are numerous equations in literature for estimating bubble size from properties and flow conditions. Not sure on accuracy. Probably more reliable is taking a case which the bubble size is 'known' to start.

2. multiphaseEulerFoam does not include compressibility. Depending on the version of OF you are using, twoPhaseEulerFoam might.

3. One of the main features of multiphaseEulerFoam is to enable euler-euler multiphase (momentum equation per phase with inter-phase drag) along with a VOF-style sharpened interface where this is needed. Fluent's 'mixture model' is a single shared momentum equation with a slip velocity to account for drag between phases. This is only appropriate for certain kinds of problems as the Fluent manual can tell you.

Hope that helps.
-Kent

[mike.franky]

Hi Kent,

Thanks for your reply. It is indeed very useful.

Regarding the diameter model, I see that I can use the isothermalDiameter model. To use this do I simply specify it in the transportProperties dictionary? Looking at the code I understand that there is no need for programming and recompiling the solver.

As for the compressibility, is it possible to adjust the code to be compressible (i.e. following a similar approach to the twoPhaseEuler solver) or is this a much more complicated task?

Thanks again for your help
Mike

[kwardle]

Addition of compressibility would be much more involved as it requires insertion of density as a variable and rearranging how the PDE is written and solved. You can take a look at an earlier version of twoPhaseEulerFoam and compare with recent to get an idea.
It is reasonably straightforward to implement a Boussinesq approximation density variation into multiphaseEulerFoam to account for natural convection flows where density variation throughout the system is not small but the difference is critical to the physics.

[openfoammaofnepo]

My understanding for the compressibility included in multiphaseEulerFoam is because they include "p = p_rgh + rho*gh;". the hydrodynamics and the thermodynamics are not decoupled. So the compression would also lead to the change of the density. However, since the temperature is solved in that solver, so the change of T would not.

[juho]

You may also want to check out the new reactingTwo/MultiphaseEulerFoam solvers:

https://github.com/OpenFOAM/OpenFOAM...ctingEulerFoam

[mike.franky]

Thank you all for your help.

openfoammaofnepo, so the multiphaseEulerFoam solver is in fact compressible? Thinking about it, the isothermal diameter model must also include compressibility effects since the bubbles expand and contract with pressure.

Juho the solver you suggested looks very interesting. Does it have any documentation?

[syavash]

Originally Posted by kwardle

Mike,
1. You are correct that the solver as released can handle a constant diameter only. There is a diameterModel class to add in other models and there is one that can handle size changes of bubbles due to external pressure changes. There are numerous equations in literature for estimating bubble size from properties and flow conditions. Not sure on accuracy. Probably more reliable is taking a case which the bubble size is 'known' to start.

2. multiphaseEulerFoam does not include compressibility. Depending on the version of OF you are using, twoPhaseEulerFoam might.

3. One of the main features of multiphaseEulerFoam is to enable euler-euler multiphase (momentum equation per phase with inter-phase drag) along with a VOF-style sharpened interface where this is needed. Fluent's 'mixture model' is a single shared momentum equation with a slip velocity to account for drag between phases. This is only appropriate for certain kinds of problems as the Fluent manual can tell you.

Hope that helps.
-Kent

Dear Kent,

I was wondering if the multiphaseEulerFoam is suitable for an application that I study:

The problem consists of air-water-solid phases, such that the solid particle are substantially larger than the cell size. This has led me to believe that the Euler-Lagrange method, as implemented in DPMFoam cannot be considered for my problem.
On the other hand, I think the VOF is essential to capture the air-solid, air-water, and water-solid interfaces. In short, the solid particles are to be carried by a mixture of air-water, with the gravity force active.
Now, the question is can I utilize multiphaseEulerFoam for this problem, or should I consider another approach??

I'd really appreciate your help on this matter.

Kind regards,
syavash