[bouhoura]

Hello,


I am trying to simulate film boiling using OF+ original solvers that can model phase change in VOF (interCondensatingEvaporatingFoam and icoReactingMultiphaseInterFoam) in order to compare them and choose the best one for my application.


Film boiling case is a famous validation case to compare phase change models, it looks like the figure below and you expect bubbles to grow from the vapour/gas film and reach the top.

From Samkhaniani, 2017

The fluid properties used are from The evaluation of the diffuse interface method for phase change simulations using OpenFOAM, Samkhaniani, 2017. Mesh is structured.


I had no problem setting up and running the case with icoReactingMultiphaseInterFoam.

Film boiling in icoReactingMultiphaseInterFoam

However, with interCondensatingEvaporatingFoam, I cannot get any bubble growing as if the two fluids were mixing. I used the exact same fluid properties, boundary condition and initialization as with icoReactingMultiphaseInterFoam. I tried different meshes, fluid properties, fvSchemes/fvSolution but I always get this weird mixing.

Film boiling in interCondensatingEvaporatingFoam at different times

Do you have any idea on how to keep the interface between gas and liquid or maybe have any experience into modeling this in OpenFoam (eventually with this solver) ?

I know there are also community solvers as phaseChangeHeatFoam, evapVOFHardt or interThermalPhaseChangeFoam but I'd like to see if this one can work with this case.



I attached the case if you want to dig into it.


Thanks in advance,
Antoine

[lgs19960514]

Hi Antoine,

I am also working on the 2d film boiling in OpenFOAM. But I am facing some problem when I using icoReactingMultiphaseInterFoam. I couldn't get a continuous film when the bubbles were generated and detached from the film, the film broke.



Did you see this problem when you are running your case? How did you fix that? Or could you share me with your setup of this case?

Many thanks,
Frank

[bouhoura]

Hi Frank,


I have never seen this behavior in any of my simulations. To me it looks like an initialization problem, how do you initialize your case ? What's the BC at the top ?
I took the time to do a clean case that you can find here : https://bitbucket.org/abouhours/test-cases/ whether with the Lee model or the Schrage model.

The case is based on Welch, A Volume of Fluid Based Method for Fluid Flows with Phase Change. The latent heat is changed to H=100kJ/kg for icoReactingMultiphaseInterFoam.





Antoine

[lgs19960514]

Originally Posted by bouhoura

Hi Frank,


I have never seen this behavior in any of my simulations. To me it looks like an initialization problem, how do you initialize your case ? What's the BC at the top ?
I took the time to do a clean case that you can find here : https://bitbucket.org/abouhours/test-cases/ whether with the Lee model or the Schrage model.



Antoine

Thanks for your advice. I will check the BC. Thanks for your sharing your cases~~

[hayat elb]

Originally Posted by bouhoura

Hi Frank,


I have never seen this behavior in any of my simulations. To me it looks like an initialization problem, how do you initialize your case ? What's the BC at the top ?
I took the time to do a clean case that you can find here : https://bitbucket.org/abouhours/test-cases/ whether with the Lee model or the Schrage model.

The case is based on Welch, A Volume of Fluid Based Method for Fluid Flows with Phase Change. The latent heat is changed to H=100kJ/kg for icoReactingMultiphaseInterFoam.





Antoine

thanks for sharing, For the test-cases/ icoReactingMultiphaseInterFoam/StefanCase_Lee/constant/phaseProperties. How did you calculate the acommodataion coefficient C?

massTransferModel
(
(water to gas)
{
type Lee;
C 2000;
Tactivate 373.15;
}

[bouhoura]

This coefficient is usually a empirical coefficient (see the litterature associated with the Lee model). You adjust it to fit the empirical results or to maintain a constant temperature at the interface.
You can find some values of this coefficient in the literature for particular cases, type of flow,...

Antoine

[lgs19960514]

I found a Chinese paper that tells how to select a proper coefficient for Lee model. If you can understand Chinese you can have a look: http://hit.alljournals.cn/hitxb_cn/c...r_id=12&falg=1

The main idea is that when c→∞ the results will be more accurate but may cause divergence. You can try to use this range :[10^3 10^5].

Cheers,
Frank

[hayat elb]

Originally Posted by bouhoura

This coefficient is usually a empirical coefficient (see the litterature associated with the Lee model). You adjust it to fit the empirical results or to maintain a constant temperature at the interface.
You can find some values of this coefficient in the literature for particular cases, type of flow,...

Antoine

thanks for replying
I want to simulate evaporation and condensation of water. How can I simulate evaporation and condensation process using Lee Model in Openfoam?

Thanks,
Hayat

[thintn222]

Hi, bouhoura

I also tried the 2d film for interCondensatingEvaporatingFoam and also got the weird output. Have you figured out what is going on with this solver.

Thank you so much, i would be really appreciated with your help

[Lorenzo210]

Hi Bouhoura,
I know you posted the question more than one year ago, but maybe I can help anyone who had the same issue.

First of all, I'm working with interCondensatingEvaporatingFoam in OF v2012. In this version there are no issue about interface diffusion (or, at least, I never have any problem).

I used to work with OF v1812, and I remember I had a similiar problem in my simulations. I tried to run an adiabatic simulation ( damBreak from interFoam laminar tutorials) and compare results with interFoam. Surprisingly, interCondensating wasn't able to mantain a sharp interface, and so advancing in time the alpha.water diffused more and more.

Looking into the source code of the solver, I found that the correction of the interface in interCondensating was declared inside createFields.H, whereas interFoam has a line code in the main application file interFoam.C.

So, to overcome this issue, I added "interface.correct();" in line 124 in interCondensatingEvaporatingFoam.C (see the attached image).

It seems to work fine with my simulations, but I don't know if the solver is the same in of v1906.

And be careful: interCondensating has a tutorial called "condensatingVessel", here in fvSolution the "compression" factor for alpha.water is set to zero, you should set this parametre to one in order to avoid the interface diffusion (the parametre is called "cAplha"). If you don't modify this value the results won't change.

Finally, my suggestion is to update to newer version of OpenFOAM (which has no problem about interface compression), or at least to try adding that line in the main .C of the solver. (EDIT: first thing to do is control the cAplha value in fvSolution, and eventually change it.)

PS: I downloaded the case "film_boiling_Lee2D" inside icoReactingMultiphaseInterFoam from https://bitbucket.org/abouhours/test-cases/. I made the proper changes in order to run it with interCondensatingEvaporatingFoam in OF 2012 and I found some good results (see attached images). I mean, I don't know if it is physically correct because I used random transport properties, but at least the interface is not diffused). The images refer to a time step equal to 0.1s and 0.2s.

Here there are the chages in the folder:
-added phaseChangeProperties in constant;
-added transportProperties in constant;
-added ThermophysicalProperties in constant;
-modified fvSchemes and fvSolution in system;
-Changed the name of the application in controlDict file in system.

Lorenzo

[Muyiwa]

Please can anyone help me with how to write an OpenFOAM code in controlDict to obtain vapor phase velocity in interCondensatingEvaporatingFoam, interFoam or other solvers.

[Nikhil2511]

Hi Lorenzo,


Can you please share the film boiling case for interCondensatingEvaporatingFoam?


Thank you