[Bali]

Originally Posted by saj216

Sad news, your suggestions didn't work. The symmetryPlane BC on the base affects the axisymmetric setup and prevents it running. Do you have any other suggestions ?

Hi Sam,

sorry I am a little confused about your case. 1/4 of the bubble will be simulated. So why using axis-symmetry? when using the axis boundary, I think the wedge boundary condition might be more suitable. And I am still not sure your case is in 2d or 3d.

If you want to setup the single bubble growth case just like the default case in the solver, using the makeaxis tool, I guess you have to reconsider your geometry. Maybe You have to draw the bottom half of the structure as well if the symmetry boundary is conflict on the base.

sorry for my poor English.

Best

[saj216]

Your English is great, don't worry about it. It is a 2D axisymmetric simulation, i'm trying to replicate this scenario based on this paper (https://www.mdpi.com/1996-1073/10/3/272/htm).


initialising a thermal boundary layer at interface using funkySetFields

However, the BCs used for the solver used in this simulation does not work for mine.

Thanks for the help again.

[Bali]

Originally Posted by saj216

Your English is great, don't worry about it. It is a 2D axisymmetric simulation, i'm trying to replicate this scenario based on this paper (https://www.mdpi.com/1996-1073/10/3/272/htm).


initialising a thermal boundary layer at interface using funkySetFields

However, the BCs used for the solver used in this simulation does not work for mine.

Thanks for the help again.

oh, I've seen this paper before, the solver they used is the evapVOFHardt I think. But you can use the validation case for the interThermalPhaseFoam solver. In Kunkelmann's PhD dissertation this case could be found.

I am really busy these days, perhaps you should check Kunkelmann's dissertation, or just try the simulation in a 2d plane without wedge boundary first, determining the boundary conditions. The files you uploaded were not complete for running in OpenFOAM so I cannot give targeted advice.

funkysetfields is good for the temperature fields initialization but, I recommend you simplify the case by using the default setFields tool first. When everything is settled, use funkysetfields tool to obatin a better initial temperature field.

Besides, in this case spurious currents should be avoided, SST model in interThemalPhaseFoam or surface tension model in evapVOFHardt solver is better than the default CSF model in interFoam.

good luck

[saj216]

No problem, thanks for the advice . I did try to upload the complete file but it was too big.

[Bali]

Originally Posted by saj216

No problem, thanks for the advice . I did try to upload the complete file but it was too big.

Hi Sam, I find a case regarding single bubble growth in superheated liquid,which can be run with interThermalPhaseChangeFoam. 1/8 of the bubble is simulated without the wedge boundary. check it maybe it will inspire you.

good luck

[saj216]

Hello again,

Do you have the link for this?

[Bali]

Originally Posted by saj216

Hello again,

Do you have the link for this?

ha? I have uploaded it in the last reply. maybe pm me your email address so I can send it to you

[saj216]

Sorry I didn't notice. I'm a little tired . Thanks for all your help. If I find out why it didn't work i'll let you know.

[saj216]

I believe I have resolved this issue. It was the way in which i was treating the temperature in terms of my initialisation.

I do have another question regarding the setting of the reference temperature in the transport properties. I know it is part of the thermal energy transport equation in the governing equations. However, how exactly should this be treated in reference to a bubble?

[saj216]

Hey guys,

Does anyone know how to code for the bubble radius in postprocessing?

[Bali]

Originally Posted by saj216

Hey guys,

Does anyone know how to code for the bubble radius in postprocessing?

Hi Sam, if there is only one bubble in your case, you can use paraview to get the bubble diameter with respect to time easily. of course, write some codes in the controlDict file can plot the diameter when running the simulation.


functions
(
DataSummary
{
functionObjectLibs ("libutilityFunctionObjects.so");
type coded;
redirectType DataSummary;
outputControl timeStep;
outputInterval 10;
code
#{

//************************************************** *********************
//First get t and dt
scalar t = mesh().time().value();
// scalar dt = mesh().time().deltaTValue();
//************************************************** *********************

//************************************************** *********************
//Now get void fraction
const volScalarField& alpha1 = mesh().lookupObject<volScalarField>("alpha.phase1" );

const scalar V_Vapor = gSum( (1.0-alpha1.internalField()) * mesh().V() );
//************************************************** *********************
// Calculate the equilibrium diameter of the bubble
const scalar D_bubble = 2*cbrt(4*V_Vapor*3/4/3.141592654);
//************************************************** *********************
//Finally print out results:
//Now write out data:
if( Pstream::master() == true )
{
std:fstream fs;
fs.open ("Diameter.dat", std::fstream::app);
fs.precision(6);
fs << t << "\t" << D_bubble << "\t" << "\n" ;
fs.close();
}

#};

codeInclude
#{
#include <fstream>
#};
}


);

[saj216]

Hi Bali,

Thanks for the reply. Wow I should have realised that. My bad. The only problem is that I had to upgrade the solver to openfoam version 7 and I have not been able to run Data Summary in it . Sorry to ask but do you have any idea?

[Bali]

Originally Posted by saj216

Hi Bali,

Thanks for the reply. Wow I should have realised that. My bad. The only problem is that I had to upgrade the solver to openfoam version 7 and I have not been able to run Data Summary in it . Sorry to ask but do you have any idea?

I havent used of-7 but maybe add this line at the end of the controldict file is helpful

libs ("libutilityFunctionObjects.so");

[saj216]

It is already there, thanks for the help though. I had to do it so it can be used on a cluster. I wish I didn't have to. Such a pain to do.

Thanks again,

Sam

[saj216]

Hi again Bali, I reread your comments and you stated that you can get bubble radius as a function of time through paraview. Could you expand on how to achieve this. Step by step if possible . Thank

[Bali]

Originally Posted by saj216

Hi again Bali, I reread your comments and you stated that you can get bubble radius as a function of time through paraview. Could you expand on how to achieve this. Step by step if possible . Thank

Hi Sam, it is really simple, just do some volume integral with the volume fraction field. Assume that alpha = 0 is gas when alpha = 1 is liquid.

1. calculator. input 1-alpha.
2. open the spreadsheet view and ctrl+a all the cell data. use integrate variables to obtain the volume of the vapor gas.
3. select the integrated data in spreadsheet and use plot selection over time

[Naaren]

Originally Posted by Fahmida

I had to reduce the domain size and increase the evaporation threshold number although I am not clear enough how the evaporation number was effecting this issue.

Hi,
I am facing a similar issue of bubble size not growing when I go for a 3D geometry in this solver. I would be happy if you can share the evaporation threshold number which was used in your simulation.


Thank you,
M Naarendharan

[Naaren]

Hi everyone,
I have one more doubt. In a 2D Axisymmetric simulation, my bubble growth is proper, but when I go for a 3D simulation in a smaller domain, the bubble placed at the center moves towards a side wall and eventually hits the wall.

I am not sure about what is causing the movement of the bubble. I would be grateful if someone could help me with this issue.


Thanking you,
M Naarendharan

[Naaren]

I am still facing the issue. Any suggestions would be of great help.


Thank you,
M Naarendharan

[Naaren]

Hi,
I am still facing the issue. Any suggestions would be very much appreciated.


Thank you,
M Naarendharan