# VOF method

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

 March 7, 2005, 12:41 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.

 March 7, 2005, 12:49 > 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.

 March 7, 2005, 20:24 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

 March 8, 2005, 02:58 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.

 March 9, 2005, 14:49 Hi Henry, Can I get any ref #5 New Member   Vinay Ramohalli Gopala Join Date: Mar 2009 Location: Netherlands Posts: 13 Rep Power: 16 Hi Henry, Can I get any references for the VOF method you have implemented ? Thanks

 March 9, 2005, 14:56 Sorry, I haven't written many #6 Senior Member   Join Date: Mar 2009 Posts: 854 Rep Power: 21 Sorry, I haven't written many papers; it's too time consuming and stops me doing the interesting work.

 March 9, 2005, 15:55 There is a decent description #7 Senior Member   Hrvoje Jasak Join Date: Mar 2009 Location: London, England Posts: 1,899 Rep Power: 32 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

 March 9, 2005, 16:00 That describes an old version #8 Senior Member   Join Date: Mar 2009 Posts: 854 Rep Power: 21 That describes an old version of my method, not the one currently in interFoam.

 December 15, 2008, 08:44 I'm currently having a look in #9 Senior Member     Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 19 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!"

 December 15, 2008, 09:30 Dear Sebastian, the time de #10 Member   Christian Winkler Join Date: Mar 2009 Location: Mannheim, Germany Posts: 63 Rep Power: 16 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

 December 15, 2008, 11:19 The time derivative is account #11 Member   Edin Berberovic Join Date: Mar 2009 Posts: 31 Rep Power: 16 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. amolrajan likes this.

 December 16, 2008, 04:15 Hi, I have two questions rela #12 Member   merrouche djemai Join Date: Mar 2009 Location: ain-oussera, djelfa, algeria Posts: 46 Rep Power: 16 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

 December 16, 2008, 04:47 Hi, I have two questions rela #13 Member   merrouche djemai Join Date: Mar 2009 Location: ain-oussera, djelfa, algeria Posts: 46 Rep Power: 16 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

 December 16, 2008, 11:54 Thanks so far for your respons #14 Senior Member     Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 19 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!"

 December 16, 2008, 13:57 Dear Edin. Thanks for your #15 Senior Member     Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 19 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!"

 December 17, 2008, 05:19 Sebastian, I will come up t #16 Member   Edin Berberovic Join Date: Mar 2009 Posts: 31 Rep Power: 16 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. amolrajan likes this.

 December 17, 2008, 09:38 Dear Edin. Thanks for your #17 Senior Member     Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 19 Dear Edin. Thanks for your answere. So, the equation will take this form? zhernadi, Pirlu, amolrajan and 2 others like this. __________________ Schrödingers wife: "What did you do to the cat? It's half dead!"

 December 18, 2008, 22:28 On a side comment, I plan on u #18 New Member   Robert Manning Join Date: Mar 2009 Posts: 12 Rep Power: 16 On a side comment, I plan on using interFoam to do 2-D flows. Does anyone know how to implement proper BC?

 December 24, 2008, 03:59 Hello All, One new question #19 Senior Member   Mark Couwenberg Join Date: Mar 2009 Location: Netherlands Posts: 130 Rep Power: 16 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

 December 24, 2008, 05:22 If this is an outlet than mayb #20 Senior Member     Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 19 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!"