# Modelling falling solid sphere using interFoam VOF model

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

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: 122
Rep Power: 9
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*0.1/3e-3=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] 1.0e-06;
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 ] 1e-10;
}

sigma           sigma [1 0 -2 0 0 0 0] 0.1;```
0/U
Code:
```    top
{
type            slip;
}
bottom
{
type            pressureInletOutletVelocity;
value           uniform ( 0 0 0 );
}
front
{
type            slip;
}
back
{
type            slip;
}
ambient
{
type            slip;
}
wall
{
type            slip;
}```
0/p_rgh

Code:
```boundaryField
{
top
{
type            fixedValue;
value           uniform 0;
}
bottom
{
type            buoyantPressure;
}
wall
{
type            buoyantPressure;
}
back
{
type            buoyantPressure;
}
ambient
{
type            buoyantPressure;
}
front
{
type            buoyantPressure;
}
}```
0/alpha1
Code:
```boundaryField
{
top
{
}
bottom
{
}
wall
{
}
back
{
}
ambient
{
}
front
{
}
}```
system/controlDict
Code:
```application     interFoam;

startFrom       startTime;

startTime       0;

stopAt          endTime;

endTime         100.0;

deltaT          1e-5;

writeInterval   1;

purgeWrite      0;

writeFormat     ascii;

writePrecision  6;

writeCompression uncompressed;

timeFormat      general;

timePrecision   6;

runTimeModifiable yes;```
system/fvSolution
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       1e-10;
relTol          0;
smoother        DICGaussSeidel;
nPreSweeps      0;
nPostSweeps     2;
nFinestSweeps   2;
cacheAgglomeration false;
nCellsInCoarsestLevel 10;
agglomerator    faceAreaPair;
mergeLevels     1;
}
tolerance       1e-10;
relTol          0;
maxIter         100;
}

"(p_rgh|Psi)"
{
solver          GAMG;
tolerance       1e-07;
relTol          0.01;
smoother        GaussSeidel;
cacheAgglomeration true;
nCellsInCoarsestLevel 10;
agglomerator    faceAreaPair;
mergeLevels     1;
}

"(p_rgh|Psi)Final"
{
\$p_rgh;
relTol          0;
}

"(Bf|U|T|k|epsilon|omega|R|omega)"
{
solver          GAMG;
tolerance       1e-07;
relTol          0.1;
smoother        GaussSeidel;
cacheAgglomeration true;
nCellsInCoarsestLevel 10;
agglomerator    faceAreaPair;
mergeLevels     1;
}

"(U|k)Final"
{
\$U;
relTol          0;
}
}

PIMPLE
{
momentumPredictor no;
nCorrectors     3;
nNonOrthogonalCorrectors 2;
nAlphaCorr      1;
nAlphaSubCycles 4;
cAlpha          1;
}

// ************************************************************************* //```
system/fvSchemes
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;
}

{
//    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;
}

{
default         corrected;
}

fluxRequired
{
default         no;
p_rgh;
pcorr;
alpha1;
}

// ************************************************************************* //```
Attached Images
 bubble.jpg (94.2 KB, 209 views)

 March 28, 2012, 07:54 #2 Senior Member   Olivier Join Date: Jun 2009 Location: France, grenoble Posts: 235 Rep Power: 9 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 ~1e-3) regards, olivier

April 2, 2012, 08:10
viscosity dependence
#3
Senior Member

Eelco van Vliet
Join Date: Mar 2009
Location: The Netherlands
Posts: 122
Rep Power: 9
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=1e-3 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 2e-3 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
Attached Images
 plotfall_boxg2_U_and_X_free.jpg (85.2 KB, 114 views) velandstream.jpg (90.3 KB, 176 views)

November 28, 2012, 04:57
#4
Senior Member

Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 667
Rep Power: 8
Quote:
 Originally Posted by eelcovv 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).
Quote:
 Originally Posted by eelcovv 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 ~1e-3)
Hi, if you want to simulate a perspex sphere droping in water, I dont know why you can change the nu of water, afaik,the nu of water is a constant if you dont considerate T or something.

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   Duong A. Hoang Join Date: Apr 2009 Location: Delft, Netherlands Posts: 92 Rep Power: 8 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: 4 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 : Refined Mesh for droplet fall Last edited by emirust; January 21, 2013 at 08:21.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post cuteapathy CFX 14 March 20, 2012 07:45 garima chaudhary FLUENT 1 July 20, 2007 08:37 Garima Chaudhary FLUENT 0 July 13, 2007 02:20 Manoj Kumar FLUENT 0 February 26, 2005 17:22 Chie Min CFX 5 July 12, 2001 23:19

All times are GMT -4. The time now is 17:58.

 Contact Us - CFD Online - Top