CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Water drop falling too slow - Interfoam (http://www.cfd-online.com/Forums/openfoam-solving/111538-water-drop-falling-too-slow-interfoam.html)

danvica January 9, 2013 10:54

Water drop falling too slow - Interfoam
 
4 Attachment(s)
I wanted to sim the falling of a drop into water. Nothing complicated (!), I just followed the dam tutorial.

The problem is that the drop is falling too slow (from steady: 50mm in 1.2s) and the velocity is not increasing.

Please see enclosed pictures about alpha and U.

Here is checkmesh result:
Code:

Mesh stats
    points:          1520469
    faces:            4461972
    internal faces:  4430208
    cells:            1470988
    boundary patches: 3
    point zones:      0
    face zones:      0
    cell zones:      0
Overall number of cells of each type:
    hexahedra:    1448660
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:    22328
Checking topology...
    Boundary definition OK.
 ***Total number of faces on empty patches is not divisible by the number of cells in the mesh. Hence this mesh is not 1D or 2D.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
    Number of regions: 1 (OK).
Checking patch topology for multiply connected surfaces ...
    Patch              Faces    Points  Surface topology                 
    defaultFaces        15876    16169    ok (non-closed singly connected) 
    atmos              0        0        ok (empty)                       
    wall                15888    16181    ok (non-closed singly connected) 
Checking geometry...
    Overall domain bounding box (0 0 0) (0.2 0.2 0.2)
    Mesh (non-empty, non-wedge) directions (0 0 0)
    Mesh (non-empty) directions (0 0 0)
    All edges aligned with or perpendicular to non-empty directions.
    Boundary openness (2.34348e-015 2.34348e-015 -2.43385e-014) OK.
    Max cell openness = 1.71543e-016 OK.
    Max aspect ratio = 0 OK.
    Minumum face area = 6.93889e-007. Maximum face area = 1.11156e-005.  Face area magnitudes OK.
    Min volume = 5.7801e-010. Max volume = 3.70593e-008.  Total volume = 0.008.  Cell volumes OK.
    Mesh non-orthogonality Max: 25.2571 average: 3.5358
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.333721 OK.
    Coupled point location match (average 0) OK.
Mesh OK.

This are my BC:

U
Code:

dimensions      [0 1 -1 0 0 0 0];
internalField  uniform (0 0 0);
boundaryField
{
    atmos
    {
        type            pressureInletOutletVelocity;
        value          uniform (0 0 0);
    }
 
    wall
    {
        type            fixedValue;
        value          uniform (0 0 0);
    }
 
    defaultFaces
    {
        type            fixedValue;
        value          uniform (0 0 0);
    }
}

p_rgh

Code:

dimensions      [1 -1 -2 0 0 0 0];
internalField  uniform 0;
boundaryField
{
    atmos
    {
        type            totalPressure;
        p0              uniform 0;
        U              U;
        phi            phi;
        rho            rho;
        psi            none;
        gamma          1;
        value          uniform 0;
    }
 
    wall
    {
        type            buoyantPressure;
        value          uniform 0;
    }
 
    defaultFaces
    {
        type            buoyantPressure;
        value          uniform 0;
    }
}

alpha (to be modified with setfields):

Code:

dimensions      [0 0 0 0 0 0 0];
internalField  uniform 0;
boundaryField
{
    wall
    {
        type            zeroGradient;
    }
    atmos
    {
        type            inletOutlet;
        inletValue      uniform 0;
        value          uniform 0;
    }
    defaultFaces
    {
        type            empty;
    }
}

The box domain is 0.2x0.2x0.2m.
The water is a sphere with radius=8mm.

Flow is laminar.

g is defined as:

Code:


dimensions      [0 1 -2 0 0 0 0];
value          ( 0 0 -9.81 );

transportProperties is the tutorial one:

Code:

phase1
{
    transportModel  Newtonian;
    nu              nu [ 0 2 -1 0 0 0 0 ] 1e-06;
    rho            rho [ 1 -3 0 0 0 0 0 ] 1000;
    CrossPowerLawCoeffs
    {
        nu0            nu0 [ 0 2 -1 0 0 0 0 ] 1e-06;
        nuInf          nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;
        m              m [ 0 0 1 0 0 0 0 ] 1;
        n              n [ 0 0 0 0 0 0 0 ] 0;
    }
    BirdCarreauCoeffs
    {
        nu0            nu0 [ 0 2 -1 0 0 0 0 ] 0.0142515;
        nuInf          nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;
        k              k [ 0 0 1 0 0 0 0 ] 99.6;
        n              n [ 0 0 0 0 0 0 0 ] 0.1003;
    }
}
phase2
{
    transportModel  Newtonian;
    nu              nu [ 0 2 -1 0 0 0 0 ] 1.48e-05;
    rho            rho [ 1 -3 0 0 0 0 0 ] 1;
    CrossPowerLawCoeffs
    {
        nu0            nu0 [ 0 2 -1 0 0 0 0 ] 1e-06;
        nuInf          nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;
        m              m [ 0 0 1 0 0 0 0 ] 1;
        n              n [ 0 0 0 0 0 0 0 ] 0;
    }
    BirdCarreauCoeffs
    {
        nu0            nu0 [ 0 2 -1 0 0 0 0 ] 0.0142515;
        nuInf          nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;
        k              k [ 0 0 1 0 0 0 0 ] 99.6;
        n              n [ 0 0 0 0 0 0 0 ] 0.1003;
    }
}
sigma          sigma [ 1 0 -2 0 0 0 0 ] 0.07;


The sim is running without any problem. Courant Number is well respected and residuals are ok.

It seems phase2 is too viscous...

I'm sure it's a silly mistake of mine but where ? Please be kind if you know it :o

Thanks.

danvica January 10, 2013 09:02

Ok, it seems nobody is able to find the mistake ;)

In the meanwhile I enclose a video of the lazy drop

https://www.box.com/s/3vs4cfumt81rbl8mjjf9

Nice to see the surface tension working when the drop is approching the water.

Any idea ?

duongquaphim January 10, 2013 18:35

Did you by any chances made the bottom patch as a wall? That's might be the only reason I can think of.

Duong

danvica January 11, 2013 02:22

Thanks Duong !

In effect my problem is about boundaries.

I meshed the domain using my normal routine: CAD + blockMesh + SnappyHexMesh.

This is usually perfect for "complex" geometries but not in this case.

I don't know why but it seems SHM has problems when you try to mesh a box using another blockMesh-defined box with the same dimensions... it calculates the right mesh but with some missing boundaries.

Could I see the mistake before ? Yes, sure. See the checkmesh result I posted before:

Quote:

Checking patch topology for multiply connected surfaces ...
Patch Faces Points Surface topology
defaultFaces 15876 16169 ok (non-closed singly connected)
atmos 0 0 ok (empty)
wall 15888 16181 ok (non-closed singly connected)
defaultFaces should be empty and the others no ! The correct one is:

Quote:

Checking patch topology for multiply connected surfaces ...
Patch Faces Points Surface topology
defaultFaces 0 0 ok (empty)
atmos 8848 9081 ok (non-closed singly connected)
wall 23248 23481 ok (non-closed singly connected)

Why haven't I used blockMesh only to mesh such a simple case ? Well, I already have my habits...I'm lazy :p

Anyway a good lesson... read carefull everything !
Thanks again Duong to show me the light :)

Regards

danvica January 11, 2013 02:26

Well, another question would be: "How can some messing BC reduce the velocity of a falling drop without blowing out a simulation ?"

But this is out of my reach so far...

muhanad November 20, 2013 09:54

setting 2D sphere
 
well done!
My point is how to set a sphere using only setFields, i am planning to modify the dam break in interFoam to simulate a falling drop in solid surface a time and over a liquid as here the other time..

after that, how to assign proper boundary condition to the falling droplet?

moreover, shall i asign an initial velocity? i am assuming it falls freely under gravity effects and starts from say, 0 m/s


All times are GMT -4. The time now is 15:34.