CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

[interCondensatingEvaporatingFoam] Film boiling - mixing problem

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree7Likes
  • 2 Post By bouhoura
  • 1 Post By bouhoura
  • 2 Post By lgs19960514
  • 2 Post By Lorenzo210

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   December 4, 2019, 04:47
Default [interCondensatingEvaporatingFoam] Film boiling - mixing problem
  #1
New Member
 
Antoine B
Join Date: Sep 2019
Location: Lyon
Posts: 3
Rep Power: 5
bouhoura is on a distinguished road
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
Attached Files
File Type: zip film_boiling2D.zip (17.6 KB, 104 views)
bouhoura is offline   Reply With Quote

Old   January 30, 2020, 02:11
Default
  #2
New Member
 
Join Date: Dec 2018
Posts: 4
Rep Power: 6
lgs19960514 is on a distinguished road
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
lgs19960514 is offline   Reply With Quote

Old   February 6, 2020, 04:36
Default
  #3
New Member
 
Antoine B
Join Date: Sep 2019
Location: Lyon
Posts: 3
Rep Power: 5
bouhoura is on a distinguished road
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
arman3939 and silviliril like this.

Last edited by bouhoura; February 6, 2020 at 08:23. Reason: Add a reference
bouhoura is offline   Reply With Quote

Old   February 6, 2020, 04:44
Thumbs up
  #4
New Member
 
Join Date: Dec 2018
Posts: 4
Rep Power: 6
lgs19960514 is on a distinguished road
Quote:
Originally Posted by bouhoura View Post
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~~
lgs19960514 is offline   Reply With Quote

Old   April 11, 2020, 19:10
Default
  #5
New Member
 
hayat EL BAAMRANI
Join Date: Nov 2017
Posts: 9
Rep Power: 7
hayat elb is on a distinguished road
Quote:
Originally Posted by bouhoura View Post
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;
}
hayat elb is offline   Reply With Quote

Old   April 13, 2020, 06:28
Default
  #6
New Member
 
Antoine B
Join Date: Sep 2019
Location: Lyon
Posts: 3
Rep Power: 5
bouhoura is on a distinguished road
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
hayat elb likes this.
bouhoura is offline   Reply With Quote

Old   April 13, 2020, 06:54
Default
  #7
New Member
 
Join Date: Dec 2018
Posts: 4
Rep Power: 6
lgs19960514 is on a distinguished road
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
arvindpj and hayat elb like this.
lgs19960514 is offline   Reply With Quote

Old   April 13, 2020, 11:44
Default
  #8
New Member
 
hayat EL BAAMRANI
Join Date: Nov 2017
Posts: 9
Rep Power: 7
hayat elb is on a distinguished road
Quote:
Originally Posted by bouhoura View Post
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
hayat elb is offline   Reply With Quote

Old   April 16, 2020, 10:47
Default
  #9
New Member
 
John
Join Date: Mar 2019
Posts: 26
Rep Power: 5
thintn222 is on a distinguished road
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
thintn222 is offline   Reply With Quote

Old   February 9, 2021, 03:55
Default
  #10
New Member
 
Lorenzo
Join Date: Apr 2020
Location: Italy
Posts: 28
Rep Power: 4
Lorenzo210 is on a distinguished road
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
Attached Images
File Type: jpg Result_02.JPG (14.3 KB, 77 views)
File Type: jpg Result_01.JPG (15.4 KB, 75 views)
File Type: jpg interCondensatingEvaporatingFoam.C mod.JPG (22.9 KB, 68 views)
raj kumar saini and arvindpj like this.
Lorenzo210 is offline   Reply With Quote

Old   February 19, 2021, 00:39
Default Vapor phase velocity
  #11
New Member
 
Muyiwa
Join Date: Feb 2020
Posts: 11
Rep Power: 4
Muyiwa is on a distinguished road
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.
Muyiwa is offline   Reply With Quote

Old   January 7, 2023, 16:13
Default
  #12
New Member
 
Nikhil Chitnavis
Join Date: Sep 2019
Location: India
Posts: 15
Rep Power: 5
Nikhil2511 is on a distinguished road
Hi Lorenzo,


Can you please share the film boiling case for interCondensatingEvaporatingFoam?


Thank you

Last edited by Nikhil2511; January 11, 2023 at 03:47.
Nikhil2511 is offline   Reply With Quote

Reply

Tags
film boiling, mixing interface, openfoam 1906, phase change

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
RPI Wall Boiling Problem aliemadi CFX 4 September 1, 2018 22:14
Tank Mixing Problem davidleinster CFD Freelancers 6 June 18, 2013 11:50
Problem on Fluent Tutorial: Horizontal Film Boilig Feng FLUENT 2 April 13, 2013 06:34
VOF problem, liquid film thickness Pedro24 FLUENT 0 May 13, 2009 06:57
multiphase mixing Problem with MRF model in MixSim Srinivas FLUENT 0 October 17, 2005 07:35


All times are GMT -4. The time now is 06:04.