|
[Sponsors] |
Bubble is not increasing in size in Nucleate boiling |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
December 8, 2019, 22:56 |
|
#21 | |
New Member
Bali
Join Date: Oct 2018
Posts: 14
Rep Power: 8 |
Quote:
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 |
||
December 8, 2019, 23:32 |
|
#22 |
Member
Sam
Join Date: May 2019
Posts: 64
Rep Power: 7 |
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. |
|
December 9, 2019, 00:35 |
|
#23 | |
New Member
Bali
Join Date: Oct 2018
Posts: 14
Rep Power: 8 |
Quote:
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 |
||
December 9, 2019, 00:44 |
|
#24 |
Member
Sam
Join Date: May 2019
Posts: 64
Rep Power: 7 |
No problem, thanks for the advice . I did try to upload the complete file but it was too big.
|
|
December 9, 2019, 00:53 |
|
#25 | |
New Member
Bali
Join Date: Oct 2018
Posts: 14
Rep Power: 8 |
Quote:
good luck |
||
December 9, 2019, 00:55 |
|
#26 |
Member
Sam
Join Date: May 2019
Posts: 64
Rep Power: 7 |
Hello again,
Do you have the link for this? |
|
December 9, 2019, 00:57 |
|
#27 |
New Member
Bali
Join Date: Oct 2018
Posts: 14
Rep Power: 8 |
||
December 9, 2019, 00:59 |
|
#28 |
Member
Sam
Join Date: May 2019
Posts: 64
Rep Power: 7 |
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.
|
|
January 3, 2020, 15:37 |
|
#29 |
Member
Sam
Join Date: May 2019
Posts: 64
Rep Power: 7 |
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? |
|
June 2, 2020, 16:14 |
|
#30 |
Member
Sam
Join Date: May 2019
Posts: 64
Rep Power: 7 |
Hey guys,
Does anyone know how to code for the bubble radius in postprocessing? |
|
June 3, 2020, 05:49 |
|
#31 | |
New Member
Bali
Join Date: Oct 2018
Posts: 14
Rep Power: 8 |
Quote:
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> #}; } ); |
||
June 3, 2020, 06:12 |
|
#32 |
Member
Sam
Join Date: May 2019
Posts: 64
Rep Power: 7 |
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? |
|
June 3, 2020, 06:17 |
|
#33 | |
New Member
Bali
Join Date: Oct 2018
Posts: 14
Rep Power: 8 |
Quote:
libs ("libutilityFunctionObjects.so"); |
||
June 3, 2020, 06:21 |
|
#34 |
Member
Sam
Join Date: May 2019
Posts: 64
Rep Power: 7 |
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 |
|
June 3, 2020, 07:52 |
|
#35 |
Member
Sam
Join Date: May 2019
Posts: 64
Rep Power: 7 |
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
|
|
June 3, 2020, 08:47 |
|
#36 | |
New Member
Bali
Join Date: Oct 2018
Posts: 14
Rep Power: 8 |
Quote:
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 |
||
November 10, 2020, 03:00 |
|
#37 | |
New Member
M Naarendharan
Join Date: Aug 2020
Posts: 21
Rep Power: 6 |
Quote:
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 |
||
November 11, 2020, 14:25 |
Movement of BUbble
|
#38 |
New Member
M Naarendharan
Join Date: Aug 2020
Posts: 21
Rep Power: 6 |
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 |
|
November 18, 2020, 04:22 |
|
#39 |
New Member
M Naarendharan
Join Date: Aug 2020
Posts: 21
Rep Power: 6 |
I am still facing the issue. Any suggestions would be of great help.
Thank you, M Naarendharan |
|
November 25, 2020, 23:29 |
|
#40 |
New Member
M Naarendharan
Join Date: Aug 2020
Posts: 21
Rep Power: 6 |
Hi,
I am still facing the issue. Any suggestions would be very much appreciated. Thank you, M Naarendharan |
|
Tags |
bubble, nucleate boiling |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Why pressure is increasing when Degassing BC is used for a pool boiling case? | soumitra2102 | CFX | 5 | August 4, 2020 07:21 |
TwoPhaseEulerFoam - Bubble diameter size Problem | BlnPhoenix | OpenFOAM Running, Solving & CFD | 8 | September 17, 2019 16:59 |
How to make UDFs for Nucleate Pool Boiling Simulation? | SIKJAE | Fluent UDF and Scheme Programming | 1 | August 4, 2018 08:07 |
OpenFOAM UpdateCoeffs Nucleate Wall Boiling | suneth.warna | OpenFOAM Programming & Development | 0 | July 31, 2016 18:42 |
Flow boiling & bubble formation | Venkat | CFX | 1 | July 23, 2009 10:20 |