
[Sponsors] 
Modelling falling solid sphere using interFoam VOF model 

LinkBack  Thread Tools  Search this Thread  Display Modes 
March 27, 2012, 11:52 
Modelling falling solid sphere using interFoam VOF model

#1 
Senior Member
Eelco van Vliet
Join Date: Mar 2009
Location: The Netherlands
Posts: 124
Rep Power: 16 
Dear Foamers,
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; } // ************************************************************************* // 

March 28, 2012, 08:54 

#2 
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 272
Rep Power: 15 
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, 09:10 
viscosity dependence

#3 
Senior Member
Eelco van Vliet
Join Date: Mar 2009
Location: The Netherlands
Posts: 124
Rep Power: 16 
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: Beijing, China
Posts: 787
Rep Power: 14 
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: 11 
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. 

August 7, 2021, 22:52 
Modelling A solid particle dropping into a Tank

#7 
New Member
Arnold
Join Date: Aug 2021
Posts: 2
Rep Power: 0 
Hello ever one,
Could you please let me know how I can model a solid drop into a tank? Which solver do you recommend? I have three phase of solid gas and liquid. Interfoam works? what about VOF? 

Thread Tools  Search this Thread 
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 09:37 
urgent query regarding vof model plz rply  Garima Chaudhary  FLUENT  0  July 13, 2007 03:20 
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 13, 2001 00:19 