
[Sponsors] 
Multiphase flow and Phase change due to heat transferevaporation 

LinkBack  Thread Tools  Display Modes 
March 6, 2009, 07:58 
Dear all,
Why there is no s

#1 
Member
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 10 
Dear all,
Why there is no solver in Multiphase flow solver series, capable of handling phase change due to evaporation? I want to simulate high pressures release of Liquid Hydrogen, which evaporates shortly (flash evaporation/its boiling Temperature is 22K), after releasing in to atmosphere and am investigating if the multiphase solvers can be helpful; I am thinking to "interfoam" based solver capable of handling with two phase flow + evaporation. Would you please let me know, where/How I should modify, if the idea feasible? Any other suggestion, I will be thankful; Hamed Aghajani hamed (dot) aghajani (at) gmail (dot) com 

March 6, 2009, 10:57 
If your simulation is incompre

#2 
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 330
Rep Power: 12 
If your simulation is incompressible, then, i think, you must try interPhaseChangeFoam. This solvers includes base model for phase change mechanism
__________________
Winter OpenFOAM days in Moscow  http://www.isprasopen.ru/en/conf/cfd.html 

March 6, 2009, 13:07 
Dear Matvej,
Thank you for yo

#3 
Member
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 10 
Dear Matvej,
Thank you for your reply, do you have experience with interPhaseChangeFoam? Could you please let me know How I should start with? Any, Tutorial? and any comments on, where i should change to introduce evaporation? Best, Hamed 

March 9, 2009, 04:32 
interPhaseChangeFoam uses VOF

#4 
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 330
Rep Power: 12 
interPhaseChangeFoam uses VOF method with surface capture, like in interFoam.
and phase kinetic is done by using fraction (void or liquid) transport. f.e., for volume void fraction we can write ddt(gamma) + div(U * gamma) = Production  Annihilation Production and Annihilation terms are often based on local pressure, normalised by infinity parameters and uses empirical constants. for example such model (based on cavitation number) Production_{Vapor} = Evaporation = Max((PSat  P)/{rho * UInf^2/2} * C1,0) Annihilation_{Vapor} = Condensation = Max((P  PSat)/{rho * UInf^2/2} * C2,0) where P, PSat  local pressure, saturation pressure, rho  local density, UInf  inf. velocity, C1,C2  empirical constants If you are intersted, i can gave links to literature (articles and dissertation) in pdf
__________________
Winter OpenFOAM days in Moscow  http://www.isprasopen.ru/en/conf/cfd.html 

March 9, 2009, 05:06 
Dear Matvej,
Thanks again for

#5 
Member
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 10 
Dear Matvej,
Thanks again for your kind reply, I would be thankful if you send me the links. Email: hamed.aghajani@gmail.com h.aghajani@kingston.ac.uk After your comment, I found a tutorial on "Solve Cavitating flow around a 2D hydrofoil using a user modified version of interPhaseChangeFoam", after reading, it may arise some questions to me which I'll share with you, later. TA! Hamed 

March 9, 2009, 05:37 
i've sended materials to you b

#6 
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 330
Rep Power: 12 
__________________
Winter OpenFOAM days in Moscow  http://www.isprasopen.ru/en/conf/cfd.html 

March 9, 2009, 05:45 
I'm working on quasisteadyst

#7 
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 330
Rep Power: 12 
I'm working on quasisteadystate homogeneous model of cavitation.
i think, for your case you need energy conservation equation and equation of state?
__________________
Winter OpenFOAM days in Moscow  http://www.isprasopen.ru/en/conf/cfd.html 

March 9, 2009, 06:24 
Dear Matvej,
Thanks for sendi

#8 
Member
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 10 
Dear Matvej,
Thanks for sending the links, but I didn't received anything on my emails! Regarding my case, High pressure release of liquid Hydrogen, yeah!, I need to include the equations you mentioned. In a realistic simulation of the release of a cryogen (liquid Hydrogen),the initiating event could be a pipeline rupture or the catastrophic failure of a storage tank, the pressure relief from system to atmospheric pressure results in spontaneous vaporization of a certain fraction of the liquid (flash vaporization). Depending on leak location and thermodynamic state of the cryogen (7bar,20 K), a twophase jet is being created, leading to the formation of aerosols which vaporize in the air without touching the ground. The liquid gas eventually reaching the ground accumulates and forms a pool which expands, depending on spilled volume and release rate, radially away from the releasing point. Best, Hamed hamed.aghajani@gmail.com H.Aghajani@kingston.ac.uk 

March 9, 2009, 07:34 
I have received them,
thanks

#9 
Member
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 10 
I have received them,
thanks 

March 9, 2009, 07:48 
Oh! Sorry, i've done mistake,

#10 
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 330
Rep Power: 12 
Oh! Sorry, i've done mistake, when typing your email address
please, check your mail now well, your task is complex, both in geometry and mathematics. In this case you can obtain transsonic velocities, thus you must use different pressure equation, am i wrong? Vapour material is compressible and you to account changes in density... I think, your algo should be something between cavitatingFoam, rasInterFoam, interPhaseChangeFoam and rhoPimpleFoam. i'm working on problem, near to your (evaporation of liquid with temperature near Tsat due to sudden pressure loss, Ma number for vapour could be more then 0.5)
__________________
Winter OpenFOAM days in Moscow  http://www.isprasopen.ru/en/conf/cfd.html 

March 9, 2009, 08:52 
Dear Matvey,
I have received

#11 
Member
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 10 
Dear Matvey,
I have received the Thesis and the paper; :) Actually the physics is complicated. I started working with openFoam, 5 month ago, first i tried combustion solvers, reactingFoam, to model the formation of Gas Hydrogen combustible cloud due to dispersion.while after evaporation, we have a combustible Hydrogen cloud! After it, I tried dieselFoam, why I supposed can capture aerosols/droplets of liquid Hydrogen by applying breakup models on it. no remarkable success in this approach! Diesel foam injects the liquid, and I couldn't apply any breakup model on continuous liquid jet/core!, this solver has evaporation model, as well. Then I came to the point to examine Multiphase solvers! I have no idea what shall I do? I just run the tutorial of compressibleLes/interFoam, twoliquidMixingFoam and twoPhaseEuelerFoam before opening this Thread. My idea was to a multistep development compressibleLesinterFoam, it is my first manipulation in source code of openFoam,by adding energy equation into it see what happens!!! Anyway, The solver should be compressible, as you mentioned, and consider the energy eq., as well. would you please let me know, why a cavitation model should be included? Do you have any suggestion, on which of your mentioned solvers, I should base solver development Thanks a lot for your time, Yours, Hamed 

March 10, 2009, 12:47 
hi, hamed!
i think about Op

#12 
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 330
Rep Power: 12 
hi, hamed!
i think about OpenFOAM solvers in a such way: 1) First, i need to understand, what goes in reality, how it looks and what physics lies behind process 2) then, i need to obtain equations for main variables, which describes state of system 3) last, i can solve equations with solvers (OpenFOAM functionality) regarding our task: 1) If you are interested in simple phase change, which will be indicated only by density variations due to changes in main variables, then you can use homogeneous approach  transport equation for void (or liquid) fraction, energy conservation equation, momentum conservation equation and mass conservation 2) If you need turbulence, then you need to insert turbulence model 3) If you need to account for effects of surface, dividing two phases, then you need surface capturing approach 4) If we need to account for such advanced effects as interphase friction, evaporation, bubble coagulation / breakup, then we need something more complex cavitation mechanism is similar to evaporation, it is based mainly on local negative pressure values. for example, for my tasks, options 1) + 2) are enough. So, if you know all about equations and algorithms, that stays behind solvers you mentioned, then you can decide which of them are needed and which of them  not. I can tell you more about my approach: 1) single momentum equation: ddt(rho U) + div(rho U U)  div (rho Reff) = grad(p) 2) single mass equation: ddt(rho) + div(rho U) 3) transport equation for gamma (mass vapor fraction) ddt(rho gamma) + div (rho U gamma)  laplacian(DgammaEff, gamma) = Prod_gamma  Annih_gamma 4) barotropic relation for density in liquid and vapour: rho = psi * p + (1  gamma) * rhol0, where psi  compressibility (d rho)/(d p), or 1/(c^2) rhol0 = rho_liq_Sat  psi*pSat 5) linear equation for psi: psi = psiv*gamma + (1  gamma)*psil 6) 2eq RAS turbulence model
__________________
Winter OpenFOAM days in Moscow  http://www.isprasopen.ru/en/conf/cfd.html 

March 11, 2009, 08:56 
Hi Matvey,
Thanks for your su

#13 
Member
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 10 
Hi Matvey,
Thanks for your supportive comments, To see the physics as simple as possible, the mean flow could be modelled using the threedimensional transient, fully compressible conservation equation for mixture mass, mixture momentum, mixture enthalpy and hydrogen mass fraction. Mixture mass (continuity equation): ∂ρ/∂t+(∂ρu_i)/(∂x_i )=0 Mixture Momentum: (∂ρu_i)/∂t+(∂ρu_j.u_i)/(∂x_j )=∂P/(∂x_i )+ρg_i+∂/(∂x_j )((μ+μ_t)((∂u_i)/(∂x_j )+(∂u_j)/(∂x_i ))) Hydrogen mass fraction (liquid plus vapour): (∂ρq_l)/∂t+(∂ρu_j q_l)/(∂x_j)=∂/(∂x_j)((ρd+μ_t/〖Sc〗_t)(∂q_l)/(∂x_j)) Mixture enthalpy: ∂ρH/∂t+(∂ρu_j H)/(∂x_j )=∂P/(∂x_j )(μ_t/〖Pr〗_t ∂H/(∂x_j ))+∂P/∂t+∂/(∂x_j )(λ ∂T/(∂x_j )+ρdH_i (∂q_i)/(∂x_j )) Where, 1/ρ=(q_1V/ρ_1V)+(q_1L/ρ_1L)+(q_2/ρ_2), 1=q_1+q_2, q_1=q_1V+q_1L Turbulence could be modelled using the kε model, in which buoyancy effects were included. .... developable! Have you added new equations to a solver? I tried to follow guideline available for icoFoam, to add energy eq to interFoam, no success yet! could you please share your experience? Best, Hamed 

March 11, 2009, 15:13 
Hi, Hamed!
After reading yo

#14 
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 330
Rep Power: 12 
Hi, Hamed!
After reading your equations, i think, that it's better to use interPhaseChangeFoam model with energy equation, which may be easily implemented in OpenFOAM: phiv = phi / fvc::interpolate(rho) ht = h + magSqr(U) / 2.0 fvm::ddt(ht) + fvm::div(phiv, ht)  fvm::laplacian(D_t, h) = S_h...... But i can't understand (sorry)  how many liquids do you want to use? 1) liquid Hydrogen 2) vaporized Hydrogen 3) Air 4) = Air + H_l + H_v N liquids  N equations of state? i can"t understand last equation 1/ρ=(q_1V/ρ_1V)+(q_1L/ρ_1L)+(q_2/ρ_2), 1=q_1+q_2, q_1=q_1V+q_1
__________________
Winter OpenFOAM days in Moscow  http://www.isprasopen.ru/en/conf/cfd.html 

March 11, 2009, 15:24 
Hei Matvej Kraposhin , thanks

#15 
Member
Nugroho Adi
Join Date: Mar 2009
Location: norway
Posts: 79
Rep Power: 10 
Hei Matvej Kraposhin , thanks for the invitation
hi Hamed, im working on the phase change as well, but on the opposite change (vapour to liquid) i just want to ask in here, if is there somebody who has some experience and can give a simple example on how to put thermophysical properties to ex: compressibleLesFoam solver or how to put additional phase properties to the coodles solver? why in the compressibleLesFoam, it uses LES model from the incompressible flow?? 

March 13, 2009, 07:30 
Dear Matvey,
Thanks for you c

#16 
Member
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 10 
Dear Matvey,
Thanks for you comments, I am trying to run a case by interPhaseChangeFoam according to the tutorial I found! Do you have a case, which works OK with solver? I updated the transportproperties file but i got problems in system/fvSolution. Thanks again, Hamed 

March 13, 2009, 08:24 
Hi, Hamed
I'm trying to fin

#17 
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 330
Rep Power: 12 
Hi, Hamed
I'm trying to finish solver, which i described on this thread  rhoPimpleFoam + phase change, when i'll done it, i'll post link to download files. case for interPhaseChangeFoam? no, i don"t have a case
__________________
Winter OpenFOAM days in Moscow  http://www.isprasopen.ru/en/conf/cfd.html 

March 13, 2009, 08:30 
Thank you,
I'll keep trying t

#18 
Member
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 10 
Thank you,
I'll keep trying to build one! 

March 16, 2009, 11:47 
cavitating solver is done

#19 
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 330
Rep Power: 12 
dear friends, you can find solver sources for OF 1.4.1 by link
http://www.oscfd.narod.ru/small_fil...PimpleFoam.tgz and solver equations by link http://www.oscfd.narod.ru/small_files/cavEnglish.odt the model is onephase turbulent flow of compressible fluid with cavitation, accounted with transport equation 

March 20, 2009, 11:45 

#20 
Member
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 10 
Thanks for posting CavitatingPimpleFoam
after coping to applications/solvers/multiphase/..., and running "wmake" to compile it; got the following message; Making dependancy list for source cavitatingPimpleFoam.C make: *** No rule to make target `/home/.../src/OpenFOAM/lnInclude/cpuTime.H, needed by `baroThermo/baroThermo.dep'. stop. would you please let me know, what the source of error is? 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Modelling Supersonic TwoPhase Flow with Phase Change  wes  OpenFOAM Running, Solving & CFD  8  April 26, 2016 07:21 
About phase change heat and mass transfer  Michael  FLUENT  2  February 13, 2011 02:49 
Two phase flow with phase change  Ahmad AlZoubi  CFX  1  November 26, 2008 04:59 
Twophase flow in Tjunction, multiphase of DPM?  Tony  FLUENT  2  July 8, 2008 01:26 
how to deal with phasechange heat exchanger?  cherry  FLUENT  1  April 16, 2002 21:59 