code_saturne User's Forum

Hello,

I have a question regarding utilizing CS to solve multiphase flows using a mixture model.

In fact, CS can solve multiphase flows using VOF, an interface-capturing model that combines some highly compressive NVD scheme with a artificial drift flux (cs_vof_deshpande_drift_flux) to compress the interface.

Is it possible to use the VOF model framework (void fraction transport and momentum equations) and incorporate an algebraic slip model to connect relative velocities between phases?

Thanks in advance.

Best regards,
Luciano.

Hello Luciano,

I guess this would be possible using the drift model. I have not gotten an answer yet from colleagues when relaying rhe question, so I'll ask again.

Best regards,

Yvan

Ok Yvan,

Thank you for your answer.

I will wait for any recommendations.

Best regards,
Luciano

Hello,

I actually did this in the past, with v5.
If you want a mixture two-phase model, the easiest way is just to add a transported scalar. You can add scalars directly in the GUI.
The scalar will represent your void fraction (or rather the mass fraction in CS).
Then, you can add a drift velocity to added scalar.

The VOF framework, from my point of view, is not adapted: in a mixture model you want your secondary phase to diffuse (i.e., being a dispersed phase), which will not be possible with the space scheme of the VOF in CS.

Hope this helps you.
Best regards,
Daniele

I forgot to add that of course you will then have to modify your properties (density, viscosity...) as a function of the scalar.
This could be done in the cs_user_physical_properties.f90 at the time, I don't know with the current version.
Best regards, Daniele

Thank you very much Daniele, for your answer on this topic.

My first attempt was to use the solution that you mentioned, but in my case, I have a mass transfer between phases, similar to a boiling or cavitation process.

It is not clear why you mention that it "will not be possible with the space scheme of the VOF in CS". It is about the compressive NVD scheme used by default with VOF?

Best regards,
Luciano

Hello Luciano,

Since you spoke about "slip model", I guessed you wanted to simulate some sort of dispersed phase inside a continuous field. Otherwise, if you use the VOF, the slip velocity is already solved, since the interface is sharp and you will have the gas velocity on one side and the liquid one on the other... This is why I wrote that the VOF is not the proper base to simulate this, but I actually don't know exactly what you want to simulate, so I can be wrong.
Regarding boiling/cavitation, I don't see the problem in doing that with an added scalar: you will just have to add a positive/negative source term to the scalar.
Keep in mind that if you want to solve the correct "drift flux model", there is one additional term appearing in the momentum equation resulting from summing the gas and liquid momentum equations (see Ishii), that you will need to write manually inside CS as source term.

I don't know if this helps...
Best regards,
Daniele

Hello Daniele,

You are correct, I want to solve a dispersed phase inside a continuous one. At the moment I use the core of the VOF implementation to modify the physical properties (density, viscosity, Cp) as a function of the void fraction. Also, I change/remove the interface-capturing model and the artificial drift-flux.

If I'm not wrong, finally I get a homogeneous mixture model. As you mentioned, if I need a drift/slip flux model (e.g. Schiller-Naumann ) between phases, I will have to add terms in the volume fraction transport equation as well as the momentum eq.

Regards,
Luciano