[hosseinfathi]

Dear Foamers

Recently, I am involved to a project which is the modeling of two phase flow in nanoscale in porous media. As we want to model the porous media in pore scale modeling we need to solve the two phase flow problem in this scale.

I want to use the interFoam solver. I think due to the unbalance artificial compression force with surface tension force in nano scale I have smearing interface instead of seeing a sharp one. (I should mention that I found sharp interface in micro scale!!!)

Does anybody know how to change something or use a parameter to observe a sharp interface in nano scale?

Moreover, I changed cAlpha to 20 and I found the sharp one, but illogical distribution of water.

I'll appreciate your helps.

Kind regards,
Hossein

[nero235]

Originally Posted by hosseinfathi

Dear Foamers

Recently, I am involved to a project which is the modeling of two phase flow in nanoscale in porous media. As we want to model the porous media in pore scale modeling we need to solve the two phase flow problem in this scale.

I want to use the interFoam solver. I think due to the unbalance artificial compression force with surface tension force in nano scale I have smearing interface instead of seeing a sharp one. (I should mention that I found sharp interface in micro scale!!!)

Does anybody know how to change something or use a parameter to observe a sharp interface in nano scale?

Moreover, I changed cAlpha to 20 and I found the sharp one, but illogical distribution of water.

I'll appreciate your helps.

Kind regards,
Hossein

Hello,

since the VOF solver uses an one-fluid approach, the code has to blend the alpha values from 1 to 0 and a value of 0.5 at the interface. Therefore there cannot be a "exactly" sharp interface. Maybe you have to look into other interface tracking techniques and solution approaches (multi-fluids ...).

Also, an cAlpha of 20 will produce unrealistic phenomena! I cannot suggest using values greater than 1.

How about a finer mesh?

Is it maybe a question about post-processing? Try to visualize the alpha field not as a scalar field of the whole domain from 0 to 1 in paraview. Instead just display only the values of the interface of 0.5.

Regards, Sebastian

[liquidspoon]

You may have some success using a different formulation for the surface tension force model (OpenFOAM only provides a single model).

We implemented the sharp surface tension force model of Raeini et al. (2012). This is computationally more expensive, but can help in certain flows. Our implementation is available in a modified two-phase solver we wrote (https://github.com/MahdiNabil/CFD-PC).

[thomasArk47]

Hello liquidspoon,

good job! and great to release it

I'm sure I will use it for my compagny
So I could give you feedback from a user point of view...

thanks.

[mkraposhin]

Also, problems can be in unit system

You can try to convert from default SI system to, for example, cm-g-sec.

We successfully solved such case by deriving our own unit system, in which all dimensions became of order of 1 (instead of 10^(-10))

[hosseinfathi]

Thank you Sebastian, liquidspoon, and mkraposhin for your comments.

I think all suggestions are helpful. I also changed the way of adding water in domain as a source term not as a flux on boundary. So I can achieve sharper interface.

Best regards,
Hossein

[AhmadZ]

Hello Guys,

I just passed through this post right now. I am wondering if it is possible to use InterFoam for nano-scale applications!. Is it realistic to use continuum physics (NSE) here?!.

Thanks

[nero235]

Originally Posted by AhmadZ

Hello Guys,

I just passed through this post right now. I am wondering if it is possible to use InterFoam for nano-scale applications!. Is it realistic to use continuum physics (NSE) here?!.

Thanks

Hey,

I really don't know. What does the literature say? Have you tried phase field methods in contrast to VoF?

Kind regards,

Sebastian

[liquidspoon]

I'm not sure what you mean by nano-scale applications. The continuum approximation is not appropriate for length scales <100s - 1000s of molecules.

Also, the surface tension force model in OpenFOAM will have issues with small length scales (literature discusses a critical cell capillary number).

[arjun]

Originally Posted by AhmadZ

Hello Guys,

I just passed through this post right now. I am wondering if it is possible to use InterFoam for nano-scale applications!. Is it realistic to use continuum physics (NSE) here?!.

Thanks

I think what you mean is that do you need extended navier stokes equations or not?

It is hard to tell, but i would feel that you would need extend version and not the one these solvers solve. I might be wrong so you would have to explore a bit more as this is very much problem dependent.

[AnasCFD]

Exactly, one needs here to use the Extended Navier Stokes equation (please see https://www.researchgate.net/publica...nnel_Gas_Flows and other publications of the coauthor Prof. Franz Durst) or Molecular Dynamics (available in OpenFoam).