CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Water drop falling too slow - Interfoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 9, 2013, 10:54
Default Water drop falling too slow - Interfoam
  #1
Senior Member
 
Daniele Vicario
Join Date: Mar 2009
Location: Novara, Italy
Posts: 142
Rep Power: 8
danvica is on a distinguished road
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

Thanks.
Attached Images
File Type: jpg pict_alpha0.jpg (30.8 KB, 55 views)
File Type: jpg pict_alpha1270.jpg (31.2 KB, 54 views)
File Type: jpg pict_u200.jpg (30.3 KB, 44 views)
File Type: jpg pict_u1270.jpg (31.0 KB, 40 views)
__________________
Daniele Vicario

blueCFD2.1 - Windows 7
danvica is offline   Reply With Quote

Old   January 10, 2013, 09:02
Default
  #2
Senior Member
 
Daniele Vicario
Join Date: Mar 2009
Location: Novara, Italy
Posts: 142
Rep Power: 8
danvica is on a distinguished road
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 ?
__________________
Daniele Vicario

blueCFD2.1 - Windows 7
danvica is offline   Reply With Quote

Old   January 10, 2013, 18:35
Default
  #3
Member
 
Duong A. Hoang
Join Date: Apr 2009
Location: Delft, Netherlands
Posts: 92
Rep Power: 8
duongquaphim is on a distinguished road
Send a message via Yahoo to duongquaphim
Did you by any chances made the bottom patch as a wall? That's might be the only reason I can think of.

Duong
duongquaphim is offline   Reply With Quote

Old   January 11, 2013, 02:22
Default
  #4
Senior Member
 
Daniele Vicario
Join Date: Mar 2009
Location: Novara, Italy
Posts: 142
Rep Power: 8
danvica is on a distinguished road
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

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

Regards
__________________
Daniele Vicario

blueCFD2.1 - Windows 7
danvica is offline   Reply With Quote

Old   January 11, 2013, 02:26
Default
  #5
Senior Member
 
Daniele Vicario
Join Date: Mar 2009
Location: Novara, Italy
Posts: 142
Rep Power: 8
danvica is on a distinguished road
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...
__________________
Daniele Vicario

blueCFD2.1 - Windows 7
danvica is offline   Reply With Quote

Old   November 20, 2013, 09:54
Default setting 2D sphere
  #6
New Member
 
Muhanad Fakhri
Join Date: Sep 2012
Posts: 7
Rep Power: 4
muhanad is on a distinguished road
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
muhanad is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
question about simulation of falling water film mengyue1 FLUENT 2 March 30, 2014 10:16
Modelling falling solid sphere using interFoam VOF model eelcovv OpenFOAM Running, Solving & CFD 5 January 16, 2013 03:37
interFoam Average velocity of water only! dsanza OpenFOAM 4 September 7, 2011 10:16
Problems with BCs in muliphase flow with water falling from a reservoir Paul_l FLUENT 2 March 11, 2011 05:59
uptodate water distribution network fredius,magige,tanzanian,(e.a) Main CFD Forum 0 January 27, 2002 08:10


All times are GMT -4. The time now is 03:44.