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

VOF method

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

Like Tree10Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   January 23, 2009, 05:30
Default Sorry to dig in. As far as I c
  #41
Senior Member
 
Mark Couwenberg
Join Date: Mar 2009
Location: Netherlands
Posts: 130
Rep Power: 9
markc is on a distinguished road
Sorry to dig in. As far as I can see in e.g. interFoam there is only 1 U. The statement in the presentation is not implemented. And reading chpter 4 of PhD thesis of Rusche, this formulation is also not used. However, Rusche also describes a two-fluid approach, which more resembles the U statement.
Maybe another addition: it has also be proposed (e.g. by Jasak, Paterson) to damp the "air" side velocity by implementing a extra line in the U eqn: UEqn += gamma*fvm::div(rhoPhi, U);

Is this equivalent...? Im afraid not.

Interesting thread though.

Brgds,

Mark
markc is offline   Reply With Quote

Old   January 23, 2009, 05:31
Default Hi Sebastian: if you are in
  #42
Member
 
Patricio Bohorquez
Join Date: Mar 2009
Location: Jaén, Spain
Posts: 94
Rep Power: 9
pbohorquez is on a distinguished road
Hi Sebastian:

if you are interested in a formal deduction of the VOF method from the point of view of the two-fluid model, and its connection with the OF implementation, my thesis (pp 12-14, ...) might help you.

http://infoscience.epfl.ch/record/130534
pbohorquez is offline   Reply With Quote

Old   January 23, 2009, 10:05
Default @Patricio: Nice job on the th
  #43
egp
Senior Member
 
egp's Avatar
 
Eric Paterson
Join Date: Mar 2009
Location: Blacksburg, VA
Posts: 198
Blog Entries: 1
Rep Power: 10
egp is on a distinguished road
@Patricio: Nice job on the thesis! Looks very complete and of high quality. Thank you for posting it. I've already forwarded it to colleagues who are working on sediment transport.

@Everyone: Threads like this one would completely disappear if each of the distributed solvers had either a "theory paper" or a link to a published document. Since OpenCFD is not able, or interested, to do this, I would suggest that the community, and especially the Special Interest Groups (SIGs), take this on for the solvers in their interest areas.

"If you would not be forgotten as soon as you are dead and rotten, either write something worth reading or do things worth the writing"

-Benjamin Franklin
Annier likes this.
egp is offline   Reply With Quote

Old   January 23, 2009, 10:37
Default Hi @Patricio: I would like
  #44
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,693
Rep Power: 27
ngj will become famous soon enoughngj will become famous soon enough
Hi

@Patricio: I would like to take Eric's lead and say that it looks like interesting reading. I am going to consider sediment transport and morphology as well, so it is nice to see people succeeding in applying OF to such problems. Especially I am looking forward to be reading about your VOF approach on the sediment bed. Especially on how you managed to get the correct bed shear stress and details like that. (Though it is not directly related to this thread, thus not a question)

Have a good weekend,

Niels
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   June 23, 2009, 07:26
Default
  #45
Senior Member
 
isabel
Join Date: Apr 2009
Location: Spain
Posts: 171
Rep Power: 9
isabel is on a distinguished road
After reading this discussion, I still have some doubts about VOF in interFoam solver:

Wich equation gammaEqn.H solves? Perhaps this

d(gamma)dt+grad(gamma*U)=0

Where can I download the thesis "Computational Fluid Dynamics of dispersed Two-Phase Flows at High Phase Fractions"?

Last edited by isabel; June 23, 2009 at 11:38.
isabel is offline   Reply With Quote

Old   June 23, 2009, 10:14
Default
  #46
Senior Member
 
isabel
Join Date: Apr 2009
Location: Spain
Posts: 171
Rep Power: 9
isabel is on a distinguished road
In the interFoam solver, what these lines in the file gamma.Eqn.H mean?

surfaceScalarField phiGamma =
fvc::flux
(
phi,
gamma,
gammaScheme
)
+ fvc::flux
(
-fvc::flux(-phir, scalar(1) - gamma, gammarScheme),
gamma,
gammarScheme
);

Last edited by isabel; June 23, 2009 at 11:38.
isabel is offline   Reply With Quote

Old   June 23, 2009, 11:26
Default
  #47
Senior Member
 
isabel
Join Date: Apr 2009
Location: Spain
Posts: 171
Rep Power: 9
isabel is on a distinguished road
In the interFoam solver, where is defined the mass conservation equation? I am refering to:

divergence(U)=0
isabel is offline   Reply With Quote

Old   June 24, 2009, 07:25
Default
  #48
Senior Member
 
Tian
Join Date: Mar 2009
Location: Berlin, germany
Posts: 106
Rep Power: 9
tian is on a distinguished road
Hi Marc,

did you find a solution to damp the "air" side velocity? I tried the extra line also but without success. The velocity increase and to hold my courant numer the time step decrease to very small and make my simulation time very slow...

Thanks.

Bye
Thomas
tian is offline   Reply With Quote

Old   July 7, 2009, 13:26
Default
  #49
Member
 
Nuno Gomes
Join Date: May 2009
Location: Portugal
Posts: 39
Rep Power: 9
Dinocrack is on a distinguished road
Quote:
Originally Posted by isabel View Post

Where can I download the thesis "Computational Fluid Dynamics of dispersed Two-Phase Flows at High Phase Fractions"?
if you dont have it, here
http://powerlab.fsb.hr/ped/kturbo/Op...chePhD2002.pdf
Dinocrack is offline   Reply With Quote

Old   July 8, 2009, 12:21
Default
  #50
New Member
 
Suraj Deshpande
Join Date: Mar 2009
Location: Madison, WI, USA
Posts: 17
Rep Power: 9
suraj is on a distinguished road
Hello All,
I was looking at the way deltaN is defined. I did not understand the reason behind keeping deltaN a function of average mesh size (average(gamma.mesh().V()). I always thought that deltaN was a fixed small number required to keep nHatfv bounded, but as it turns out, it is not.

Thanks,
Suraj
suraj is offline   Reply With Quote

Old   January 7, 2010, 20:05
Default
  #51
Senior Member
 
Claus Meister
Join Date: Aug 2009
Location: Wiesbaden, Germany
Posts: 241
Rep Power: 9
idrama is on a distinguished road
Hey Seaga,

I read your post. Did you get any references about MULES?

Cheers,

Claus
idrama is offline   Reply With Quote

Old   June 24, 2010, 18:56
Default
  #52
Senior Member
 
santiagomarquezd's Avatar
 
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 430
Rep Power: 15
santiagomarquezd will become famous soon enough
Quote:
Originally Posted by eberberovic View Post
The time derivative is accounted for within the MULES solver. In the gammaEqn.H only explicit fluxes are calculated, which are needed in MULES.

The interface.nHatf() represents a cell face unit interface normal flux. It is evaluated from the dot product of the cell face surface vector and the interface unit normal calculated at the cell face:

nHatf_ = nHatfv & Sf,

where

nHatfv = gradGammaf/(mag(gradGammaf) + deltaN_).

and deltaN is a stabilization factor for the case of gradGammaf = 0.

For the full implementation look in src/transportModels/interfaceProperties/interfaceProperties.C

Regards.
Edin, I'm studying the interFoam solver now, based on the code cfd-online posts and particularly on your paper: "Drop impact onto a liquid layer of finite thickness: Dynamics of the cavity evolution". Actually I'm focused in time marching, MULES, etc.
I understood Eq. 30 as a time subdivision in order to improve convergence and stability. I had hoped to use this small step in an explicit time marching loop actualizing VOF field in every substep. Although a different thing is done, calculating flux subdivisions and finally summing all of them to recover the whole timestep flux (Eq. 31). I recognize you are right here, that's in the code, but I can't understand this step at all. Could you explain a bit this topic to me? Do you hava any external reference in books, papers, about this method?

Regards. Santiago.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D.
Research Scientist
Research Center for Computational Methods (CIMEC) - CONICET/UNL
Tel: 54-342-4511594 Int. 7032
Colectora Ruta Nac. 168 / Paraje El Pozo
(3000) Santa Fe - Argentina.
http://www.cimec.org.ar
santiagomarquezd is offline   Reply With Quote

Old   June 25, 2010, 07:11
Default
  #53
Senior Member
 
sega's Avatar
 
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 12
sega is on a distinguished road
Quote:
Originally Posted by idrama View Post
Hey Seaga,

I read your post. Did you get any references about MULES?

Cheers,

Claus
No, I have still no reference about MULES.
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!"
sega is offline   Reply With Quote

Old   June 28, 2010, 06:50
Default MULES solver in interFoam
  #54
Senior Member
 
Suresh kumar Kannan
Join Date: Mar 2009
Location: Luxembourg, Luxembourg, Luxembourg
Posts: 129
Rep Power: 9
kumar is on a distinguished road
Hello Edin Berberovic and santiago,
I have been following this post closely to understand the MULES and VOF methodology implemented in OpenFOAM.
I just got the paper Drop impact onto a liquid layer of finite thicknessynamics of the cavity evolution. Thanks santiago for mentioning it, since i have been looking for a paper which explains the MULES.
I want to confirm that the MULES concept explained in that paper is the one implemented in OF-1.5, in the interFoam solver
What about OF-1.6.x, in which the pressure difference is handled in a different way. So could anybody tell me what is the major difference between the MULES explained in the paper and the one currently in OF-1.6.x, interFoam solver.

regards
K.Suresh kumar
kumar is offline   Reply With Quote

Old   June 28, 2010, 08:33
Default
  #55
Senior Member
 
santiagomarquezd's Avatar
 
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 430
Rep Power: 15
santiagomarquezd will become famous soon enough
Kumar, Edin's paper is one of the most comprehensive papers about interFoam that I have found. It's true, it explains interFoam version 1.5 but the part about MULES is valid in 1.6.x also.
Changes in pressure treatment from pd to p are not affecting the MULES part, I've been studying MULES and it's important only in solving the non-linear advection equation (Eq. 15), in fact it is not mentioned in Edin's paper. Changes in pd affects only in mommentum equation formulation (Eq. 20).
Calling MULES is a strategy to solve Eq. 15, taking a look of alphaEqn.H we have,

Code:
00009     for (int aCorr=0; aCorr<nAlphaCorr; aCorr++)
00010     {
00011         surfaceScalarField phiAlpha =
00012             fvc::flux
00013             (
00014                 phi,
00015                 alpha1,
00016                 alphaScheme
00017             )
00018           + fvc::flux
00019             (
00020                 -fvc::flux(-phir, scalar(1) - alpha1, alpharScheme),
00021                 alpha1,
00022                 alpharScheme
00023             );
00024 
00025         MULES::explicitSolve(alpha1, phi, phiAlpha, 1, 0);
00026 
00027         rhoPhi = phiAlpha*(rho1 - rho2) + phi*rho2;
00028     }
by means of this solving and Eq. 31 a new flux is assembled in order
to solve the mommentum equation.
Hope these insights can be helpful, and will be valuable if other
foamers correct me and add more info. Please share your findings.

Regards
Pirlu likes this.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D.
Research Scientist
Research Center for Computational Methods (CIMEC) - CONICET/UNL
Tel: 54-342-4511594 Int. 7032
Colectora Ruta Nac. 168 / Paraje El Pozo
(3000) Santa Fe - Argentina.
http://www.cimec.org.ar
santiagomarquezd is offline   Reply With Quote

Old   October 5, 2010, 05:18
Default
  #56
Member
 
Edin Berberovic
Join Date: Mar 2009
Posts: 31
Rep Power: 9
eberberovic is on a distinguished road
Hi.

Sorry for not answering, I was far too busy in the previous months.

Regarding the sub-cycling in gammaEqn, I have no references on that, but it indeed does what you are writing, i.e. the gamma field is being updates in every sub-cycle time step (in MULES, explicitly or implicitly) and the total face-flux is accumulated for the momentum equation.

There are also no references on MULES, but it is basically an additional limiter, which is used to clip or cut off the superfluous fluxes. The face-flux calculated using any limited scheme is represented as a sum of the upwind-flux and the corresponding flux correction. Then the limiter lambda is calculated, according to the worst (limiting) cases of gamma being equal to the maximum/minimum from the cells surrounding the cell of interest. Its value is between 1 and 0, which means that the flux corrections are either left unchanged, or the superfluous flux corrections are partially clipped, or the flux corrections are completely cut off reducing the scheme to upwind.

Hope this helps,
Edin.
sharonyue, Pirlu and hchen like this.
eberberovic is offline   Reply With Quote

Old   October 5, 2010, 06:22
Default
  #57
Senior Member
 
isabel
Join Date: Apr 2009
Location: Spain
Posts: 171
Rep Power: 9
isabel is on a distinguished road
Hello everybody,

Can anybody send me the paper "Drop impact onto a liquid layer of finite thickness: Dynamics of the cavity evolution"?

Mi mail is lamasgaldo@yahoo.es
isabel is offline   Reply With Quote

Old   October 5, 2010, 06:36
Default
  #58
Member
 
Edin Berberovic
Join Date: Mar 2009
Posts: 31
Rep Power: 9
eberberovic is on a distinguished road
Hi Isabel,

I've just sent you the paper PRE 2009. There is one typo in it, namely Eq. (24) represents the face flux rather than velocity at the cell-face. Sorry for this, it went also unnoticed by the reviewers.

Edin.
eberberovic is offline   Reply With Quote

Old   October 5, 2010, 06:43
Default
  #59
Member
 
Edin Berberovic
Join Date: Mar 2009
Posts: 31
Rep Power: 9
eberberovic is on a distinguished road
Hi Isabel,

I've just sent you the paper PRE 2009. There is one typo in it, namely Eq. (24) represents the face flux rather than velocity at the cell-face. Sorry for this, it went also unnoticed by the reviewers.

Edin.
eberberovic is offline   Reply With Quote

Old   October 5, 2010, 09:11
Default
  #60
Senior Member
 
santiagomarquezd's Avatar
 
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 430
Rep Power: 15
santiagomarquezd will become famous soon enough
Edin,

Quote:
Originally Posted by eberberovic View Post
Hi.

Sorry for not answering, I was far too busy in the previous months.

Regarding the sub-cycling in gammaEqn, I have no references on that, but it indeed does what you are writing, i.e. the gamma field is being updates in every sub-cycle time step (in MULES, explicitly or implicitly) and the total face-flux is accumulated for the momentum equation.

There are also no references on MULES, but it is basically an additional limiter, which is used to clip or cut off the superfluous fluxes. The face-flux calculated using any limited scheme is represented as a sum of the upwind-flux and the corresponding flux correction. Then the limiter lambda is calculated, according to the worst (limiting) cases of gamma being equal to the maximum/minimum from the cells surrounding the cell of interest. Its value is between 1 and 0, which means that the flux corrections are either left unchanged, or the superfluous flux corrections are partially clipped, or the flux corrections are completely cut off reducing the scheme to upwind.

Hope this helps,
Edin.
thanks for your answer, I've been working in this solver for the last two months, lately Nisi is working with me too. We've found that MULES::limiter is based on Flux-Corrected Transport ideas, particularly this version is quite similar to the job of Zalesak (http://rsmas.miami.edu/personal/misk...FCT-JCPv31.pdf). In Zalesak job, lambdas are calculated once, in MULES::limiter this work is done iteratively. We've arrived to similar conclussions as yours, thanks for this confirmation.

Best.
Pirlu likes this.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D.
Research Scientist
Research Center for Computational Methods (CIMEC) - CONICET/UNL
Tel: 54-342-4511594 Int. 7032
Colectora Ruta Nac. 168 / Paraje El Pozo
(3000) Santa Fe - Argentina.
http://www.cimec.org.ar
santiagomarquezd 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
Comparing between the Fractional step method and the SIMPLE method ghlee Main CFD Forum 1 April 10, 2012 16:59
Finite volume method vs finite difference method? superfool Main CFD Forum 4 October 21, 2006 14:37
Pressure Correction method, Finite Volume Method Seeker01 Main CFD Forum 2 January 13, 2003 03:49
hess-smith method and fvm method yangqing FLUENT 0 March 20, 2002 20:25
Projection method and Block-off method Leo Main CFD Forum 0 June 14, 2001 07:22


All times are GMT -4. The time now is 23:02.