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

Multiphase flow and Phase change due to heat transferevaporation

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   March 6, 2009, 07:58
Default Dear all, Why there is no s
  #1
Member
 
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 9
haghajani is on a distinguished road
Dear all,

Why there is no solver in Multi-phase 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
haghajani is offline   Reply With Quote

Old   March 6, 2009, 10:57
Default If your simulation is incompre
  #2
Senior Member
 
mkraposhin's Avatar
 
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 330
Rep Power: 11
mkraposhin is on a distinguished road
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.opencloudconf.ru/en/oscome.html
mkraposhin is offline   Reply With Quote

Old   March 6, 2009, 13:07
Default Dear Matvej, Thank you for yo
  #3
Member
 
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 9
haghajani is on a distinguished road
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
haghajani is offline   Reply With Quote

Old   March 9, 2009, 04:32
Default interPhaseChangeFoam uses VOF
  #4
Senior Member
 
mkraposhin's Avatar
 
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 330
Rep Power: 11
mkraposhin is on a distinguished road
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.opencloudconf.ru/en/oscome.html
mkraposhin is offline   Reply With Quote

Old   March 9, 2009, 05:06
Default Dear Matvej, Thanks again for
  #5
Member
 
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 9
haghajani is on a distinguished road
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
haghajani is offline   Reply With Quote

Old   March 9, 2009, 05:37
Default i've sended materials to you b
  #6
Senior Member
 
mkraposhin's Avatar
 
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 330
Rep Power: 11
mkraposhin is on a distinguished road
i've sended materials to you by e-mail, they are from site

http://library.caltech.edu/
__________________
Winter OpenFOAM days in Moscow - http://www.opencloudconf.ru/en/oscome.html
mkraposhin is offline   Reply With Quote

Old   March 9, 2009, 05:45
Default I'm working on quasi-steady-st
  #7
Senior Member
 
mkraposhin's Avatar
 
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 330
Rep Power: 11
mkraposhin is on a distinguished road
I'm working on quasi-steady-state 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.opencloudconf.ru/en/oscome.html
mkraposhin is offline   Reply With Quote

Old   March 9, 2009, 06:24
Default Dear Matvej, Thanks for sendi
  #8
Member
 
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 9
haghajani is on a distinguished road
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 two-phase 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
haghajani is offline   Reply With Quote

Old   March 9, 2009, 07:34
Default I have received them, thanks
  #9
Member
 
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 9
haghajani is on a distinguished road
I have received them,
thanks
haghajani is offline   Reply With Quote

Old   March 9, 2009, 07:48
Default Oh! Sorry, i've done mistake,
  #10
Senior Member
 
mkraposhin's Avatar
 
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 330
Rep Power: 11
mkraposhin is on a distinguished road
Oh! Sorry, i've done mistake, when typing your e-mail address

please, check your mail now

well, your task is complex, both in geometry and mathematics.

In this case you can obtain trans-sonic 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.opencloudconf.ru/en/oscome.html
mkraposhin is offline   Reply With Quote

Old   March 9, 2009, 08:52
Default Dear Matvey, I have received
  #11
Member
 
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 9
haghajani is on a distinguished road
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 multi-step 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
haghajani is offline   Reply With Quote

Old   March 10, 2009, 12:47
Default hi, hamed! i think about Op
  #12
Senior Member
 
mkraposhin's Avatar
 
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 330
Rep Power: 11
mkraposhin is on a distinguished road
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 / break-up, 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) 2-eq RAS turbulence model
__________________
Winter OpenFOAM days in Moscow - http://www.opencloudconf.ru/en/oscome.html
mkraposhin is offline   Reply With Quote

Old   March 11, 2009, 08:56
Default Hi Matvey, Thanks for your su
  #13
Member
 
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 9
haghajani is on a distinguished road
Hi Matvey,
Thanks for your supportive comments,
To see the physics as simple as possible, the mean flow could be modelled using the three-dimensional 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 k-ε model, in which buoyancy effects were included.
....
develop-able!

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
haghajani is offline   Reply With Quote

Old   March 11, 2009, 15:13
Default Hi, Hamed! After reading yo
  #14
Senior Member
 
mkraposhin's Avatar
 
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 330
Rep Power: 11
mkraposhin is on a distinguished road
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.opencloudconf.ru/en/oscome.html
mkraposhin is offline   Reply With Quote

Old   March 11, 2009, 15:24
Default Hei Matvej Kraposhin , thanks
  #15
Member
 
Nugroho Adi
Join Date: Mar 2009
Location: norway
Posts: 79
Rep Power: 9
mahaputra is on a distinguished road
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??
mahaputra is offline   Reply With Quote

Old   March 13, 2009, 07:30
Default Dear Matvey, Thanks for you c
  #16
Member
 
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 9
haghajani is on a distinguished road
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
haghajani is offline   Reply With Quote

Old   March 13, 2009, 08:24
Default Hi, Hamed I'm trying to fin
  #17
Senior Member
 
mkraposhin's Avatar
 
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 330
Rep Power: 11
mkraposhin is on a distinguished road
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.opencloudconf.ru/en/oscome.html
mkraposhin is offline   Reply With Quote

Old   March 13, 2009, 08:30
Default Thank you, I'll keep trying t
  #18
Member
 
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 9
haghajani is on a distinguished road
Thank you,
I'll keep trying to build one!
haghajani is offline   Reply With Quote

Old   March 16, 2009, 11:47
Default cavitating solver is done
  #19
Senior Member
 
mkraposhin's Avatar
 
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 330
Rep Power: 11
mkraposhin is on a distinguished road
dear friends, you can find solver sources for OF 1.4.1 by link

http://www.os-cfd.narod.ru/small_fil...PimpleFoam.tgz

and solver equations by link

http://www.os-cfd.narod.ru/small_files/cav-English.odt

the model is one-phase turbulent flow of compressible fluid with cavitation, accounted with transport equation
mkraposhin is offline   Reply With Quote

Old   March 20, 2009, 11:45
Default
  #20
Member
 
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 9
haghajani is on a distinguished road
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?
haghajani is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


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 Al-Zoubi CFX 1 November 26, 2008 04:59
Two-phase flow in T-junction, multiphase of DPM? Tony FLUENT 2 July 8, 2008 01:26
how to deal with phase-change heat exchanger? cherry FLUENT 1 April 16, 2002 21:59


All times are GMT -4. The time now is 17:03.