
[Sponsors] 
December 21, 2012, 09:23 
compressible flow with phase change

#1 
Senior Member
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 7 
Dear friends!
I made model for compressible, twophase flow with phase change due to temperature and/or pressure variation, which is based on interFoam (VOF). If you are intersted in using it, you can download it by this link (with tutorials). Solver was done for OF2.1.0 and 1.6ext Equations description located here I need your advices and feed back. I would like to put this solver in OpenFOAM  but this can take some time. And, of course, excuse me my "great" russian english Some nice pictures: 

April 25, 2013, 05:54 

#2 
New Member
Coral.Qing
Join Date: Apr 2013
Posts: 2
Rep Power: 0 
thx, i will try it if i can figure out it


April 29, 2013, 11:47 

#3 
Senior Member

Hi Matvey,
thanks for share your solver! I have some questions: 1) have you implemented the Singhal model ?? In your opinion is it difficult to do it!? 2) Can I use the solver without the hydrostatic part of the pressure (rho * g *h)? Thanks Regards Marco 

July 26, 2013, 13:45 

#4 
Member
Jace
Join Date: Oct 2012
Posts: 71
Rep Power: 5 
Hi,
when I tried to run the steamjet tutorial, it complains about not having the nuSgsUSpaldingWallFunction, and I couldn't find such wall function anywhere in my OpenFOAM source either, can someone point to me where to get a copy of it? if it's out there at all. thanks! Last edited by zhengzh5; July 26, 2013 at 14:50. 

August 6, 2013, 13:31 

#5  
Senior Member
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 7 
Quote:
2) Yes, just set g = (0 0 0) 

August 6, 2013, 13:32 

#6  
Senior Member
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 7 
Quote:


August 6, 2013, 13:43 

#7  
Senior Member
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 7 
Quote:
Solver code has been changed. Also, system of equations changed too. Latest description of the test cases and description you can find here! Today this solver works well with two type of problem: 1) Cavitation (water) 2) Flashing of water in the adiabatic conditions Again, solver is available only for OpenFOAM 2.1.0, but i hope to port it to OF2.2.X, OF1.6ext 

August 6, 2013, 14:12 

#8  
Senior Member

Quote:
Hi, here is the link, where you can download the description of the model: http://fluidsengineering.asmedigital...icleid=1429576 The model includes also the gas cavitation! You cannot find the full description of the model with the gas mass transfer (one more transport equation)! If you give to me your mail I will send to you it! thank you for sharing your work Best Regards Marco 

August 7, 2013, 04:06 

#9 
Senior Member
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 7 

August 7, 2013, 04:13 

#10 
Senior Member
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 7 
I think, it can be a problem. If gas volume fraction is small enough, and it's density is comparable to density of vapour, then we can neglect influence of the gas on the flow. So we can decouple gas fraction transport from the liquid/vapour transport.
But, if the gas volume fraction is large, then we need a coupled solution, and this can be a slightly more complex case 

August 7, 2013, 12:59 

#11  
Senior Member
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 7 
Quote:
Source code and short description located here But now i have 2 questions: 1) Dimensions of equation (15) are different from (13). Does it mean that constant Ce should have dimensions [meter/second]? [(eq.13)]=kg/(meter^3 secod) 2) In equations (15) and (16) we can see mass fractions (Fv and Fl), but in our model we are solving for volume fraction. Why did you commented corresponding terms rho2/rho and rho1/rho ? 

August 7, 2013, 13:38 

#12  
Senior Member

Quote:
Great! First of all! I already validate the Singhal mass transfer model , so we can trust about the implementation! Answer 1) The dimension of the constants actually is [meters/seconds]. This is due to an author's trick! Answer 2) To implement the Singhal model I follwed the Tobias Huuva Thesis (this thesis is too long to send but I will send tomorrow just the Sighal Model page)! He replaces the mass fraction with the vapour one. The reason is that the transport equations of Singhal are written for the mass fractions so Singhal needs to scale the vapour fractions! The transport equations in OpenFoam are already written for the vapour fracions so you do not need to scale them! Fhurter improvements: 1) I have already implemented th Zwart model link: http://www.google.de/url?sa=t&rct=j&...50310824,d.Yms It is the Ansys cavitation model and I already validated this implementation..if you want I can send to you tomorrow! 2) What is a real improvement (which noone has already done) is to take in account for the Gas Cavitation (from equation 24 to equation 30 in Sighal's lecture )! It becomes very important in the past few years (for example for mineral oil applications)! But your model needs to be 4 phases (with condensable and non condesable gas vapour and liquid) and you must add two new transport eqautions. If you want to implement it I can share to you my knowledge (the Singhal model is not clear deriveted and I already made some new impromvents in the mass transfer rates)! Let me know (by mail too for the two improvments) regards Marco 

August 7, 2013, 14:08 

#13  
Senior Member
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 7 
Quote:
1) Av*rhov=rhom*Fv (Av  vapour volume fraction, rhov  vapor density, rhom  mixture density, Fv  mass vapour fraction) then ddt(Fv*rhom)+div(Fv*rhom*U)=ddt(Av*rhov) + div(Av*rhov*U) so, OpenFOAM formulation for Av transport is the same as in Singhal paper 2) Fv in eq, (15) comes from eq. (13) where Av*rhov/rhom=Fv, isn't it? Please, tell me where am i wrong? 

August 7, 2013, 16:16 

#14  
Senior Member
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 7 
Quote:
Also, can you propose your test cases for this models? 

August 8, 2013, 06:24 

#15  
Senior Member

Quote:
Hi, I already sent to you an mail! Regarding the test case, I have also an hydraulic resistence with mineral oil. Moreover, I am preparing an hydraulic valve with cavitation (the geometry looks like really cool).. but it takes time to be ready! Regards Marco 

August 9, 2013, 10:46 

#16 
Senior Member
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 7 
Hi, i made update to the solver it is available at the same address
Test cases for the hemispherical body with the Zwart and the Singhal models are still running. Some notes on the implementation of volume fraction transport in OpenFOAM. 1) It is formulated in volume fluxes, but it derived from mass fluxes: ddt(alpha_l * rho_l) + div(alpha_l * rho_l * U) = m_l ddt(alpha_l) + div(alpha_l U_l) = m_l/rho_l + (alpha_l/rho_l)*DDt(rho_l) when fluid is incompressible and flow is isothermal, last term is zero, then we have: ddt(alpha_l) + div(alpha_l U_l) = m_l m_l  is the sum of m^+ and m^ of the Singhal model. In OpenFOAM m_l is represented by method mDotAlphal. That's why i think that we need to scale terms in Singhal model when switching from the mass fraction to the volume fraction 2) In Singhal model pressure difference is calculated as: dP=pSat + c*k  p, but OpenFOAM interPhaseChangeFoam solver do not contain term "c*k" in the equation for pressure. And there is no such term in my model. That's why i don't include 0.5*0.39*rho_l*k when i estimate mass evaporation term. If you want to insert this term in the model (interPhaseChangeFoam or compressibleMixingPhaseChangeFoam), then you need to change equation for pressure to obtain mass and momentum continuity About NCG. I think, i can add transport equations for the noncondensible gas in the model in three step: 1) Simple transport of the volume gas fraction without accounting for it's influence on the total mass of the system (alpha_g <= 1.0e5 or another small value) 2) Transport of the volume gas fraction without desorption or absorption 3) And if two previous models will work, i can try to implement model with desorption and absorption If you are still interested, it will be nice to run test cases, which you had proposed by email 

August 9, 2013, 11:44 

#17 
Senior Member

Hi Matvej,
1) I will try to validate the model without scaling as well! The point is that it is not clear how Singhal has derivated it. I mean, where exactly he intoduces this scaling. 2) I totally agree with you. I choose to change the all mass transfer models with the 'k' term (as well as for the pressure equation) . Because I think that turbulence effects on cavitation too! About NCG. I think that your three steps are right. Just some considerations: 1) You must account for other two phases (dissolved and undissolved) so the transport equations which you were speaking about (in your second point) are two. This is because there is a big diference between vapor and gas. "Dissolved vapor" is the liquid. Dissolved gas has the same property of the liquid but it is not he liquid. You must take in account its fraction in the multiphase..also because it is the limit of the fraction of released undissolved gas ! 2) The absorpiton and desorption rates of Singhal show not a very good agreement with experiment. We are developing our own rates. If you are intrested I can (will) provide to you these two OpenFoam files as I did for Singhal (the same framework of the vapour cavitation) 3) I will send to you a presentation about the implementation of NCG in Ansys. Finally, I understood that you want to upload your solver in OpenFoam. A very good test case could be the valve which I spoke about. The geomety is not easy but it presents (experimentally) both gas and water cavitation. So it could be cool to have this test case. I will manage to do it when your solver is ready. During this time I try to get familiar with your implementation and I prepare the mesh. I am so sorry that I wrote to much! Anyway, your work is great Regards Marco 

September 13, 2013, 16:09 
Version 210 not available anymore?

#18 
New Member
Join Date: Sep 2013
Posts: 9
Rep Power: 3 
Hi Matvej
I would really like to use your solver, but I only have the versions 2.1.1, 2.2.0 and 2.2.1 on my computer. The others seem to be not available anymore as ubuntu deb packs from the openfoam site. Is there any chance to use it? For 2.1.1 I get the message: > FOAM FATAL IO ERROR: [0] keyword div(phi,psiphase1) is undefined in dictionary "/home/mkoch/MasterArbeit/0010vers211phasechangeFoam_try/processor0/../system/fvSchemes::divSchemes" thanks! 

September 14, 2013, 07:42 

#19 
New Member
Join Date: Sep 2013
Posts: 9
Rep Power: 3 
Ah sorry, it works now. I just used my old Dictionaries which were not suitable.
Another Question: what is beta for simpleLiquid? is it the del rho/del T in the EOS? 

September 16, 2013, 17:09 

#20  
Senior Member
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 7 
Quote:
I'm sorry for the late response! Today i'm working on the new version of this solver. The system of equations has been rewritten totally, so, please, wait about 24 weeks. Of course, i will made versions for OF2.1.X and OF2.2.X Changes are very significant, 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Multiphase flow and Phase change due to heat transferevaporation  haghajani  OpenFOAM Running, Solving & CFD  86  April 9, 2013 03:49 
phase change modeling  Danial Q  Main CFD Forum  0  April 5, 2012 02:14 
Modelling Supersonic TwoPhase Flow with Phase Change  wes  OpenFOAM Running, Solving & CFD  6  August 12, 2009 09:13 
low speed compressible flow  lily  CFX  2  November 16, 2005 06:15 
Two phase flow models  Atholl  Main CFD Forum  2  May 7, 2002 04:49 