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

Phase change with VOF

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   June 13, 2005, 07:16
Default Hi! I want to set up a comp
  #1
shu
New Member
 
Bitan SHU
Join Date: Mar 2009
Posts: 14
Rep Power: 8
shu is on a distinguished road
Hi!

I want to set up a computation region with two domains, one with the conductive heat transfer in the wall under the liquid, and the other with the conductive as well convective heat transfer in the liquid above the wall. My questions:

1. How can I set up these two domains? In the tutorial case "scalarTransportFoam/pitzDaily", it was only one domain.

2. What does the parameter "DT" mean in the following line
DT DT [0 2 -1 0 0 0 0] 0.01;
from the file ~/OpenFOAM/OpenFOAM-1.1/tutorials/scalarTransportFoam/pitzDaily/constant/transpo rtProperties? If it is kinematic viscosity (with the unit [m^2/s]), how can I introduce two different thermal conductivities?

3. Shall I create a new solver for the heat transfer equation with conductive and convective terms? The flow is laminar and unsteady.

4. Further, I will have a bubble on the wall in the liquid, which grows and detachs because of evaporation (pool boiling). To simulate such a problem, the source terms are needed in the mass-conservation equation, in the heat transfer equation, and in the VOF-equation too. Is it possible to do it with OpenFoam? (two phase, laminar flow)

Many thanks,

Bitan
shu is offline   Reply With Quote

Old   June 13, 2005, 16:26
Default It is possible to do all you r
  #2
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
It is possible to do all you require with OpenFOAM but it will require a substantial effort and you might want to consider arranging a support contract particularly if you would like OpenCFD to do some/all of the implementation for you.
henry is offline   Reply With Quote

Old   June 13, 2005, 22:47
Default Here's some help: 1) conjug
  #3
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,769
Rep Power: 21
hjasak will become famous soon enough
Here's some help:

1) conjugate heat transfer simulations in FOAM (as it stands) are not completely straightforward. There are several possible approaches, but you need to know what you are doing. There is no tutorial for this.

2) scalarTransportFoam only solves the standard transport equation for a scalar, given a prescribed velocity field. Thus, kinematic viscosity is not needed as the flow equations are not solved. DT that you mention is the diffusivity (conductivity) for the scalar you are solving for.

3) I would advise studying the tutorials and the code until you get a better grasp of your problem. You will then need to write your own solver, tailored to the problem you are trying to do.

4) Two-phase laminar solver with the VOF-like approach already exists in FOAM. It is called interFoam and there is a tutorial for it. In order to do the evaporation, you will need to add various terms to the original equations + solve for the heat transfer; in order to do that successfully, you will first need to understand the current implementation. That's where I would start.

Good luck,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   June 17, 2005, 07:09
Default Thank you very much for the an
  #4
shu
New Member
 
Bitan SHU
Join Date: Mar 2009
Posts: 14
Rep Power: 8
shu is on a distinguished road
Thank you very much for the answers and the advices!

To Henry:
I am not sure, if we have budget to give such a contract. But I will discuss it in my team.

To Hrvoje:
I have created a solver for the heat transfer equation with the convective and conductive terms. It works fine.
As the next step I will try to combine it with interFoam.

Has anyone set up two or more domains with the different properties, e.g. the thermal conductivities, or densities?

Bitan
shu is offline   Reply With Quote

Old   May 25, 2007, 03:13
Default Hallo Bitan, I am working on
  #5
New Member
 
Karl-Heinz Leitz
Join Date: Mar 2009
Posts: 16
Rep Power: 8
khleitz is on a distinguished road
Hallo Bitan,
I am working on a similar problem like you. I want so simulate the melting and evaporation of a solid. Therefore I have alread combined the lagragian heat transfer solver with interfoam. The melting works quite nice however I have no idea how to implement the evaporation. Did you have success in implementing the evaporation in the interfoam solver?
If yes, where do I have to add the source terms?
Best reagards,
Karl-Heinz
khleitz is offline   Reply With Quote

Old   May 29, 2007, 11:29
Default Hallo Karl-Heinz, I model t
  #6
shu
New Member
 
Bitan SHU
Join Date: Mar 2009
Posts: 14
Rep Power: 8
shu is on a distinguished road
Hallo Karl-Heinz,

I model the evaporation with some terms in all the conservation equations, i.e. mass, Navier-Stokes, energy, and VOF-equation. The terms is derived from the rate of evaporation which depends on the heat transfer at the phase interface and the latent heat.

However I have problem with the smeared phase interface described with VOF. Because in this zone the heat conductivity can not be determined correctly. And then false evaporation rate turns out. For this reason I am working on Level-Set-Method. Maybe this problem will not be so serious in case of melting, because the ratio of heat conductivities is smaller then that in case of evaporation.

Regards,
Bitan
shu is offline   Reply With Quote

Old   January 30, 2008, 23:55
Default I am new to OpenFoam. I am sol
  #7
New Member
 
RAJEEV R. KRISHNAN
Join Date: Mar 2009
Location: Bangalore, Karnataka, India
Posts: 2
Rep Power: 0
rajeevrkris is on a distinguished road
I am new to OpenFoam. I am solving for hot air flow (1000K) at a velocity of 5m/s on top of water (300K)flowing at 2 m/s in a converging duct. How shall I model evaporation of water into air stream using volume of fluid in interFoam? Can anybody help me out?
Thank you,
Rajeev Krishnan
rajeevrkris is offline   Reply With Quote

Old   February 1, 2008, 05:54
Default > Has anyone set up two or mor
  #8
kar
Senior Member
 
Kārlis Repsons
Join Date: Mar 2009
Location: Latvia
Posts: 111
Rep Power: 8
kar is on a distinguished road
> Has anyone set up two or more domains with the different properties, e.g. the thermal conductivities, or densities?

Looks like post from somebody who's done that would be appreciated! I'm also interested..
kar is offline   Reply With Quote

Old   February 1, 2008, 10:23
Default I have submitted a paper to th
  #9
shu
New Member
 
Bitan SHU
Join Date: Mar 2009
Posts: 14
Rep Power: 8
shu is on a distinguished road
I have submitted a paper to the conference CHT-08, in which a model for the phase change is described. To model the phase change some additional terms are introduced into the equations. Film boiling can be simulated successfully. It is based on interFoam.

Bitan
shu is offline   Reply With Quote

Old   July 21, 2008, 12:37
Default Hello Bitan Shu, I'm workin
  #10
New Member
 
arghaz
Join Date: Mar 2009
Location: France
Posts: 1
Rep Power: 0
arghaz is on a distinguished road
Hello Bitan Shu,

I'm working on modelling Film Boiling and I'm interested by your CHT-8 paper. Thus, can you send me an example.

Arghaz
arghaz is offline   Reply With Quote

Old   July 23, 2008, 10:18
Default Hi Arghaz, it would be a pl
  #11
shu
New Member
 
Bitan SHU
Join Date: Mar 2009
Posts: 14
Rep Power: 8
shu is on a distinguished road
Hi Arghaz,

it would be a pleasure for me to send you the paper. Please drop me an email: shubitan <at> gmx dot net

Bitan Shu
shu is offline   Reply With Quote

Old   February 10, 2009, 16:06
Default Hi Bitan Shu, what about co
  #12
Member
 
Nugroho Adi
Join Date: Mar 2009
Location: norway
Posts: 79
Rep Power: 8
mahaputra is on a distinguished road
Hi Bitan Shu,

what about condensation? phase change from steam (water vapour) into liquid phase ?

does your solver work for this case?

i have a problem within phase change with the multiphase flow.

could you please guide me to solve the problem?

and could you make a tutorial on internet for your case of film boiling?

kindly please help me

regards

Nugroho Adi
mahaputra is offline   Reply With Quote

Old   March 5, 2009, 15:22
Default Dear all, I want to simulate
  #13
Member
 
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 8
haghajani is on a distinguished road
Dear all,
I want to simulate Liquid Hydrogen release under high pressures, and am investigating if the multiphase solvers can helpful;

Liquid Hydrogen evaporates shortly (flash evaporation/boiling Temperature 20K) after releasing in to atmosphere and I am thinking to a solver based on "ras/interfoam" 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   April 17, 2009, 14:17
Default help plz
  #14
New Member
 
Karthik Shenoy
Join Date: Mar 2009
Posts: 8
Rep Power: 8
karthik is on a distinguished road
actually i plan to simulate phase change in centrifugal casting.
so basicall 3 phase
1>air that wil fil the rest of the domain and interact with the molten metal and involve in heat transfer
2>molten metal that will spin and develop its own flows
3>molten metal that wil interact with the mould and get transformed to solid

4>the solid rotating mould with the sourrounding atmosphere(dunno bout tis

an my self very confuse regarding the mesh and the models, relaxation etc)

so if any of u guys can enlighten me if this problem CAN ACTUALLY BE

SIMULATED
.i hav already obtained the fluid flow patterns alon in Fluidyn

unfortunatly fluidyn doesnot support heat transfer with phase change hence i

plan to use openFoam(i know verry little of foam)so plz help me out guys
karthik is offline   Reply With Quote

Old   June 16, 2009, 03:12
Default nucleate boiling
  #15
Senior Member
 
isabel
Join Date: Apr 2009
Location: Spain
Posts: 171
Rep Power: 8
isabel is on a distinguished road
I want to simulate nucleate boiling with OpenFOAM for my doctoral studies. Can anybody send me papers or information to lamasgaldo@yahoo.es
isabel is offline   Reply With Quote

Old   June 17, 2009, 13:51
Default
  #16
New Member
 
Karthik Shenoy
Join Date: Mar 2009
Posts: 8
Rep Power: 8
karthik is on a distinguished road
it can be done but am not sure of wat solver to use sorry
karthik is offline   Reply With Quote

Old   June 22, 2009, 11:03
Default
  #17
Senior Member
 
isabel
Join Date: Apr 2009
Location: Spain
Posts: 171
Rep Power: 8
isabel is on a distinguished road
I am studying interFoam solver and I have two doubts:

- What is pEqn.H ?
- Where is mass conservation equation defined? It would be gradient(u)=0
isabel is offline   Reply With Quote

Old   July 8, 2009, 00:25
Default
  #18
Senior Member
 
Sandy Lee
Join Date: Mar 2009
Posts: 207
Rep Power: 9
sandy is on a distinguished road
Quote:
Originally Posted by isabel View Post
I am studying interFoam solver and I have two doubts:

- What is pEqn.H ?
- Where is mass conservation equation defined? It would be gradient(u)=0
==================

To a phase change VOF problems, div(u) =? 0, I don't know too.

However, in the InterPhaseChangeFoam solver, div(u) = (1/rho1 - 1/rho2) * (mDotP[0] -mDotP[1]) * (p - pSat) = (vDotcP-vDotvP)*(p - pSat), so in pEqn.H of this solver, the source term of pdEqn become into (vDotcP-vDotvP) * (pd - pv[=rho*gh - pSat]), and the (vDotcP-vDotvP) * pd is implicitly solved as the Sp term of pdEqn and (vDotcP-vDotvP) * pv is a explcit term as the Su term of pdEqn. Am I right?

But, I don't know why this equation could not be solved convergently, after I activated the cavitation model to it and gammaEqn?

Who know the reason? Please help me out. Thanks a lot.

Last edited by sandy; July 20, 2009 at 00:34.
sandy is offline   Reply With Quote

Old   July 16, 2009, 06:23
Default
  #19
Senior Member
 
isabel
Join Date: Apr 2009
Location: Spain
Posts: 171
Rep Power: 8
isabel is on a distinguished road
Thank you very much, sandy. In the interPhaseChangeFoam, the terms vDotcP and vDotvP are divided by the pressure, so when you solve the continuity equation, you multiply for the pressure again to have the units 1/s.

Then, my equation which is

div(U) = source

in pEqn.H of the interPhaseChangeFoam solver would be typped as:

fvScalarMatrix pEqn
(
fvc::div(phi) - fvm::laplacian(rUAf,pd) - source
);


Am I wright?
isabel is offline   Reply With Quote

Old   July 16, 2009, 08:42
Default
  #20
Senior Member
 
Sandy Lee
Join Date: Mar 2009
Posts: 207
Rep Power: 9
sandy is on a distinguished road
Quote:
Originally Posted by isabel View Post
Thank you very much, sandy. In the interPhaseChangeFoam, the terms vDotcP and vDotvP are divided by the pressure, so when you solve the continuity equation, you multiply for the pressure again to have the units 1/s.

Then, my equation which is

div(U) = source

in pEqn.H of the interPhaseChangeFoam solver would be typped as:

fvScalarMatrix pEqn
(
fvc::div(phi) - fvm::laplacian(rUAf,pd) - source
);


Am I wright?
I think, in interphasechangefoam, the source term is that the terms vDotcP and vDotvP are divided by the rho (1/rho1 - 1/rho2), so

div(U? or phi)= source = (p - pSat) * ( vDotcP - vDotvP).

If it is "phi" but "U", whether or not we also need to interpolate RHS to the face? Why not?

Last edited by sandy; July 20, 2009 at 00:37.
sandy 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
phase change Robert FLUENT 6 May 2, 2009 06:17
Two phase flow with phase change Ahmad Al-Zoubi CFX 1 November 26, 2008 04:59
Phase Change ....!! prakash FLUENT 2 May 15, 2007 20:12
udf for phase change ranjit.prakash FLUENT 0 February 26, 2007 11:10
Phase change J.W.Ryu FLUENT 6 March 20, 2003 16:58


All times are GMT -4. The time now is 04:04.