
[Sponsors] 
March 27, 2012, 10:52 
Modelling falling solid sphere using interFoam VOF model

#1 
Senior Member
Eelco van Vliet
Join Date: Mar 2009
Location: The Netherlands
Posts: 123
Rep Power: 11 
Sponsored Links
I have been trying to model a falling perspex sphere in water using interFoam. I figured that choosing a large surface tension and dynamic viscosity would allow to represent the perspex sphere by the second liquid phase: the high surface tension should ensure a spherical shape and the high dynamic viscosity should prevent internal fluid circulations in the sphere. With my first attemp I find that the terminal falling velocity is way too small compared to what I expect. I assume a 3 mm sphere (density 2200 kg/m3) in water (1000 kg/m3), hence I expect to find a velocity of about 0.33 m/s However, I find a velocity of about 1 mm/s, which is an order 100 too small. Please find attached a view on the velocity field and pressure distribution over the particle (bubble). My quesions are: 1) Is it in priciple allowed to use VOF for falling object such as small particles? 2) Has anybody simulated solid spheres with VOF ? 3) Could anybody comment on my numerical settings? My impression is that the difficulty is the large pressure inside of the bubble due to the 2*sigma/R bubble pressure. I have choosen sigma as small as possible (0.1 N/m) in order to keep the internal bubble pressure as low as possible. Nevertheless, for R=3 mm this would still lead to a P=2*0.1/3e3=67 N/m. The hydrostatic pressure over the bubble (which takes care of the buyancy force) is 30 Pa. The pressure I find in the bubble is actually higher than anticipated: about 400 Pa. Perhaps the large pressure drop over the bubble interface give problems ? Well, anyway, in case anybody can say anything sensible about it. Please let me know. I will include a summary of my numerical and physical settings below. Some remarks: I have already varried some things. I checked a different gradScheme interpolation (see fvSchemes): cellMDLimited insteat of Gauss lnear. I have varied the resolution already. This mesh already uses 0.5 mlj cells. The grid was made with blockMesh and some grid refinement in the bubble areay with snappyHexMesh. Also I have tried a large surface tenstion (1 N/m), but none of it leads to a higher falling velocity Well. That's it. Any suggestions appreciated! Regards Eelco constant/transportProperties Code:
phase1 { transportModel Newtonian; nu nu [0 2 1 0 0 0 0] 1.0e06; rho rho [1 3 0 0 0 0 0] 1000; sigmaC sigmaC [1 3 3 0 0 2 0 ] 22; } phase2 { transportModel Newtonian; nu nu [0 2 1 0 0 0 0] 1; rho rho [1 3 0 0 0 0 0] 2200; sigmaC sigmaC [1 3 3 0 0 2 0 ] 1e10; } sigma sigma [1 0 2 0 0 0 0] 0.1; Code:
top { type slip; } bottom { type pressureInletOutletVelocity; value uniform ( 0 0 0 ); } front { type slip; } back { type slip; } ambient { type slip; } wall { type slip; } Code:
boundaryField { top { type fixedValue; value uniform 0; } bottom { type buoyantPressure; } wall { type buoyantPressure; } back { type buoyantPressure; } ambient { type buoyantPressure; } front { type buoyantPressure; } } Code:
boundaryField { top { type zeroGradient; } bottom { type zeroGradient; } wall { type zeroGradient; } back { type zeroGradient; } ambient { type zeroGradient; } front { type zeroGradient; } } Code:
application interFoam; startFrom startTime; startTime 0; stopAt endTime; endTime 100.0; deltaT 1e5; writeControl adjustableRunTime; writeInterval 1; purgeWrite 0; writeFormat ascii; writePrecision 6; writeCompression uncompressed; timeFormat general; timePrecision 6; runTimeModifiable yes; Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.0.0   \\ / A nd  Web: www.OpenFOAM.com   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { pcorr { solver PCG; preconditioner { preconditioner GAMG; tolerance 1e10; relTol 0; smoother DICGaussSeidel; nPreSweeps 0; nPostSweeps 2; nFinestSweeps 2; cacheAgglomeration false; nCellsInCoarsestLevel 10; agglomerator faceAreaPair; mergeLevels 1; } tolerance 1e10; relTol 0; maxIter 100; } "(p_rghPsi)" { solver GAMG; tolerance 1e07; relTol 0.01; smoother GaussSeidel; cacheAgglomeration true; nCellsInCoarsestLevel 10; agglomerator faceAreaPair; mergeLevels 1; } "(p_rghPsi)Final" { $p_rgh; relTol 0; } "(BfUTkepsilonomegaRomega)" { solver GAMG; tolerance 1e07; relTol 0.1; smoother GaussSeidel; cacheAgglomeration true; nCellsInCoarsestLevel 10; agglomerator faceAreaPair; mergeLevels 1; } "(Uk)Final" { $U; relTol 0; } } PIMPLE { momentumPredictor no; nCorrectors 3; nNonOrthogonalCorrectors 2; nAlphaCorr 1; nAlphaSubCycles 4; cAlpha 1; } // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.0.1   \\ / A nd  Web: www.OpenFOAM.com   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { // default CrankNicholson 1; default Euler; } gradSchemes { // default Gauss linear; default cellMDLimited Gauss linear 1.0; div(rho*phi,U) Gauss linearUpwind cellLimited Gauss linear 1; } divSchemes { div(rho*phi,U) Gauss limitedLinearV 1; div(phi,alpha) Gauss vanLeer; div(phirb,alpha) Gauss interfaceCompression; } laplacianSchemes { default Gauss linear corrected; laplacian(gamma,Psi) Gauss harmonic uncorrected; } interpolationSchemes { default linear; // gamma Gauss harmonic uncorrected; } snGradSchemes { default corrected; } fluxRequired { default no; p_rgh; pcorr; alpha1; } // ************************************************************************* // 

Sponsored Links 
March 28, 2012, 07:54 

#2 
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 266
Rep Power: 11 
hello,
You should try with a smaller viscosity ratio, 1e6 is too much and may give youstrong parasitic current/numerical artefacts ... so try a a viscosity ratio of 1e3. (i.e nu2 ~1e3) regards, olivier 

April 2, 2012, 08:10 
viscosity dependence

#3 
Senior Member
Eelco van Vliet
Join Date: Mar 2009
Location: The Netherlands
Posts: 123
Rep Power: 11 
Hi Olivier
Thanks for the remark. It indeed appears that the ratio nu_fluid/nu_bubble was choosen too large. I have run a few cases with varying bubble viscosity. Ideally the bubble viscosity is as large as possible (to mimic a solid sphere). For lower viscosities you can anticipate a different drag coefficient of the bubble, given by Cd=(16/Re)*((1+(3mu_p)/(2*mu_f))/(1+mu_p/mu_f)) (analytical solution for Rep<1 by Hadammard,1911) For mu_p<<mu_f this give Cd=16/Re (stokes flow of gas bubble) and for mu_p>>mu_f this gives Cd=24/Re (stokes flow for particle). Clearly, I am not in Stokes regime, nevertheless, if I use this relation I would say that for my choise of nu_p=1e3 m2/s > mu_p=rho*nu_p=2.2 Pa s I am in the limit of spherical particles as Cd > 24/Re. Well, I run a few values of nu_p; attached the graph of the position X_p and velocity U_p of each value, incl the analytical solution for a true spherical particle. As you can see, now indeed I am in the right ball park. My previous value of nu_p (of 0.01 m2/s) gave way too low terminal falling speed, but as soon you go below 2e3 m2/s for the kinematic viscity (i.e. take nu_p/nu_f < 1000), the terminal rising speed is reasonably well predicted. My only concern now is that the terminal falling velocity is very sensitive to the exact choise of nu_p, whereas the values taken should all be in the limit that Cd> 24/Re, hence still lead to the same terminal falling velocity. Perhaps this is due to differences in the deformation of the sphere. I will check the influence of the surface tension. But anybody with further suggestions: any comments appreciated:) Regards Eelco 

November 28, 2012, 04:57 

#4  
Senior Member
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 754
Rep Power: 10 
Quote:
Quote:
by the way, you sphere is so small, have you ever tried a larger diameter? such as 1cm steel ball? 

November 28, 2012, 06:06 

#5 
Member

Hi Eelco,
There is a group in Sweden performing quite a lot of simulations on settling of solid particles using VOF. Here is one of their paper: A novelmultiphase DNS approach for handling solid particles in a rarefied gas H. Ströma, b, , , S. Sasicc, , B. Anderssona, b, http://dx.doi.org/10.1016/j.ijmultip...ow.2011.03.011 Cheers, Duong 

January 16, 2013, 03:37 

#6 
Member
Join Date: Sep 2012
Posts: 30
Rep Power: 6 
Hey Eelcov,
You mention you perform a grid refinement in the region close to the bubble with snapphyHexMesh. How exactly are you doing this? Thanks! Edit: more infor can be found : http://www.cfdonline.com/Forums/ope...pletfall.html Last edited by emirust; January 21, 2013 at 08:21. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
error message  cuteapathy  CFX  14  March 20, 2012 07:45 
plz rply urgent regrding vof model for my system  garima chaudhary  FLUENT  1  July 20, 2007 08:37 
urgent query regarding vof model plz rply  Garima Chaudhary  FLUENT  0  July 13, 2007 02:20 
Modelling flow around a ship's hull using vof  Manoj Kumar  FLUENT  0  February 26, 2005 17:22 
CFX4.3 build analysis form  Chie Min  CFX  5  July 12, 2001 23:19 
Sponsored Links 