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 Tree9Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   March 7, 2005, 13:41
Default Hello, I am working on mod
  #1
Vinay Ramohalli Gopala (Gopala)
Guest
 
Posts: n/a
Hello,

I am working on modeling of mass-transfer between two immiscible liquids. Recently I started using OpenFoam.

I have tried some simple simulations by manipulating the dambreak problem,(for example a denser liquid drop falling in a less denser liquid and also the rayleigh-taylor instability problem).

I intend to use VOF for my project and it would be very helpful to know more about the method implemented in the present version of OpenFoam, i.e. is it CICSAM or a different one ?

Also I would like to know if the option in interFoam - movingMesh is the same as Adaptive grid refinement around the interFace ?

Thanks in advance.
  Reply With Quote

Old   March 7, 2005, 13:49
Default > i.e. is it CICSAM or a diff
  #2
Henry Weller (Henry)
Guest
 
Posts: n/a
> i.e. is it CICSAM or a different one

It's a new technique I developed a few years ago to resolve some of the fundamental problems of CICSAM and other traditional VOF interface compression methods. The differences have already been debated at length, have a look through previous threads on the subject.

> Also I would like to know if the option in interFoam -
movingMesh is the same as Adaptive grid refinement around
the interFace ?

No.
  Reply With Quote

Old   March 7, 2005, 21:24
Default I was wondering what's the ac
  #3
Ali (Ali)
Guest
 
Posts: n/a
I was wondering what's the actual and preferred expression for the compressive term in gamma equation and a very brief explanation of how it is derived. The formula for 'phir' in the code differs from what Henrik has mentioned in (Eq. (4.15)). In the code:

phir=cGamma()*mag(phi/mesh.magSf())*interface.nHatf()

while Henrik's suggests (if I have formulated it correctly):

phir=cGamma*nhatf*max(nhat * phi / mesh.magSf()**2 )

Are they really different (am I missing something) and if yes, which one is better?


2) where is the smoothing function for 'gamma' in interFoam? Does it have a significant effect on VOF performance or just affects surface tension prediction?

thanks
  Reply With Quote

Old   March 8, 2005, 03:58
Default I have tried various options
  #4
Henry Weller (Henry)
Guest
 
Posts: n/a
I have tried various options for the compression term in the gamma equation and the one I recommend is the one that is currently in interFoam. It is not derived, it is selected and there are other choices. If you would like to find out which option is best for you try them out on your case.

There is no "smoothing" function for gamma in interFoam, it was found to be detrimental to the overall performance of the interface capturing.
  Reply With Quote

Old   March 9, 2005, 15:49
Default Hi Henry, Can I get any ref
  #5
New Member
 
Vinay Ramohalli Gopala
Join Date: Mar 2009
Location: Netherlands
Posts: 13
Rep Power: 8
gopala is on a distinguished road
Hi Henry,

Can I get any references for the VOF method you have implemented ?

Thanks
gopala is offline   Reply With Quote

Old   March 9, 2005, 15:56
Default Sorry, I haven't written many
  #6
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
Sorry, I haven't written many papers; it's too time consuming and stops me doing the interesting work.
henry is offline   Reply With Quote

Old   March 9, 2005, 16:55
Default There is a decent description
  #7
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
There is a decent description of the implemented Interface-Capturing Methodology (probably a bit out of date now) in a PhD Thesis by dr. Henrik Rusche:

Computational Fluid Dynamics of Dispersed Two-Phase Flows at High Phase Fractions, Henrik Rusche, Imperial College of Science, Technology & Medicine, December 2002.

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

Old   March 9, 2005, 17:00
Default That describes an old version
  #8
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
That describes an old version of my method, not the one currently in interFoam.
henry is offline   Reply With Quote

Old   December 15, 2008, 09:44
Default I'm currently having a look in
  #9
Senior Member
 
sega's Avatar
 
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 11
sega is on a distinguished road
I'm currently having a look into the gammaEqn.H from OF 1.4.1

Well, some parts look like the equation (4.15) from Rusches PhD thesis.

But still I'm not sure about some issues:

- Where is the time derivative of gamma?
- What is interface.nHatf()? Is it the normal vector to the cell face?
- What doese MULES::explicitSolve01(gamma, phi, phiGamma) mean?

Thanks so far!
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!"
sega is offline   Reply With Quote

Old   December 15, 2008, 10:30
Default Dear Sebastian, the time de
  #10
caw
Member
 
Christian Winkler
Join Date: Mar 2009
Location: Mannheim, Germany
Posts: 63
Rep Power: 8
caw is on a distinguished road
Dear Sebastian,

the time derivative is not there because of the usage of MULES. Look at OpenFOAM-1.5.x\src\finiteVolume\fvMatrices\solvers\MULES\MU LES.H for details:

" MULES: Multidimensional universal limiter with explicit solution.
Solve a convective-only transport equation using an explicit universal
multi-dimensional limiter.
Parameters are the variable to solve, the normal convective flux and the
actual explicit flux of the variable which is also used to return limited
flux used in the bounded-solution. "

Best regards
Christian
caw is offline   Reply With Quote

Old   December 15, 2008, 12:19
Default The time derivative is account
  #11
New Member
 
Edin Berberovic
Join Date: Mar 2009
Posts: 29
Rep Power: 8
eberberovic is on a distinguished road
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.
eberberovic is offline   Reply With Quote

Old   December 16, 2008, 05:15
Default Hi, I have two questions rela
  #12
mer
Member
 
merrouche djemai
Join Date: Mar 2009
Location: ain-oussera, djelfa, algeria
Posts: 46
Rep Power: 8
mer is on a distinguished road
Hi,
I have two questions related to the interFoam solver:

1) I used the utility "barycenter" posted by Sebastian. It works fine with axisymmetric cases. In 2D or 3D cases and using the utility, it doesn't work (the position of the bubble is in decrease when time increase). Is there a signification for that?
I find also that the position of the bubble increase when the value of Min(gamma) is negative. Is there a relation with Min(gamma) and the barycenter of the bubble?!

MULES: Solving for gamma
Liquid phase volume fraction = 0.99921 Min(gamma) = -2.20718e-11 Max(gamma) = 1

2) I want to switch to OF-1.5. In the file interFoam.C there is an additional line comparing to OF-1.4.1:

p = pd + rho*gh;

Is it a construction of the pressure p field or what? if yes, how can I get values of this field for different times.

Best regards
mer is offline   Reply With Quote

Old   December 16, 2008, 05:47
Default Hi, I have two questions rela
  #13
mer
Member
 
merrouche djemai
Join Date: Mar 2009
Location: ain-oussera, djelfa, algeria
Posts: 46
Rep Power: 8
mer is on a distinguished road
Hi,
I have two questions related to the interFoam solver:

1) I used the utility "barycenter" posted by Sebastian. It works fine with axisymmetric cases. In 2D or 3D cases and using the utility, it doesn't work (the position of the bubble is in decrease when time increase). Is there a signification for that?
I find also that the position of the bubble increase when the value of Min(gamma) is negative. Is there a relation with Min(gamma) and the barycenter of the bubble?!

MULES: Solving for gamma
Liquid phase volume fraction = 0.99921 Min(gamma) = -2.20718e-11 Max(gamma) = 1

2) I want to switch to OF-1.5. In the file interFoam.C there is an additional line comparing to OF-1.4.1:

p = pd + rho*gh;

Is it a construction of the pressure p field or what? if yes, how can I get values of this field for different times.

Best regards
mer is offline   Reply With Quote

Old   December 16, 2008, 12:54
Default Thanks so far for your respons
  #14
Senior Member
 
sega's Avatar
 
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 11
sega is on a distinguished road
Thanks so far for your responses.
I will try to get them step by step (and respond if there are any questions).

First of all:
Is there a reference for MULES in some kind of citable form?
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!"
sega is offline   Reply With Quote

Old   December 16, 2008, 14:57
Default Dear Edin. Thanks for your
  #15
Senior Member
 
sega's Avatar
 
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 11
sega is on a distinguished road
Dear Edin.

Thanks for your response.
I have read your answer carefully and looked the code up.

But I still have some questions related to the code.
Is this the correct analytical representation of the code?


I'm not sure what to do with the deltaN.
In the code it's calculated like this:
1e-8/average(gamma.mesh().V()), 1/3)

What does gamma.mesh().V() mean?

See you (maybe at SLA ...)
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!"
sega is offline   Reply With Quote

Old   December 17, 2008, 06:19
Default Sebastian, I will come up t
  #16
New Member
 
Edin Berberovic
Join Date: Mar 2009
Posts: 29
Rep Power: 8
eberberovic is on a distinguished road
Sebastian,

I will come up to you. The coefficient cGamma is not in the analytical transport equation, but it is used in modeling the relative velocity.

gamma.mesh().V(), for a non-moving mesh simply takes the volumes of control cells throughout the domain, so the average of it to the power of 1/3 gives a representative cell dimension (lenght).

Regards.
eberberovic is offline   Reply With Quote

Old   December 17, 2008, 10:38
Default Dear Edin. Thanks for your
  #17
Senior Member
 
sega's Avatar
 
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 11
sega is on a distinguished road
Dear Edin.

Thanks for your answere.
So, the equation will take this form?


zhernadi, Pirlu and duan like this.
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!"
sega is offline   Reply With Quote

Old   December 18, 2008, 23:28
Default On a side comment, I plan on u
  #18
New Member
 
Robert Manning
Join Date: Mar 2009
Posts: 12
Rep Power: 8
bobatpurdue is on a distinguished road
On a side comment, I plan on using interFoam to do 2-D flows. Does anyone know how to implement proper BC?
bobatpurdue is offline   Reply With Quote

Old   December 24, 2008, 04:59
Default Hello All, One new question
  #19
Senior Member
 
Mark Couwenberg
Join Date: Mar 2009
Location: Netherlands
Posts: 130
Rep Power: 8
markc is on a distinguished road
Hello All,

One new question related to VOF solvers (interFoam).
I modelled a ship sailing in a basin with water and air. The watersurface at the Inlet and internal has been set at Z=4 m. After a few seconds of physical time (so not CPU time) the solver crashes on very low deltaT. Looking the results in paraview one can see what happens:


The picture shows the outlet of the domain. It looks like the watersurface is attracted towards Z=0 at the outlet patch. Maybe it might eventually go down further, provided that the solver should not crash.
However, after that I translated the geometry such that the initial waterlevel is at Z=0 and kept the rest unchanged. Than the solution runs smooth as expected.
BC's on the outlet:
gamma and U: zeroGradient
pd: fixedValue uniform 0

My questions:
- is there any mechanism that forces a surface towards Z=0?
- Has the problem described here something to do with continuity and/or mass conservation?
- I set BC's on the top of the domain at fixedValue (vesselspeed) for U and zeroGradient for pd, this to reduce strong air vortices which influence solution stability. Should I better set the BC's on the top at atmosphere?

Hope someone can shine his/hers light, not because I got stuck (I found a work around) but out of curiousity,

Brgds,

Mark

Mark
markc is offline   Reply With Quote

Old   December 24, 2008, 06:22
Default If this is an outlet than mayb
  #20
Senior Member
 
sega's Avatar
 
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 11
sega is on a distinguished road
If this is an outlet than maybe the water is simply "leaking" out of it.
Maybe you can try fixedValue 0 for U at the out- and inlet?
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!"
sega 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 20:55.