CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   Droplet break-up in a t-junction (http://www.cfd-online.com/Forums/openfoam/94039-droplet-break-up-t-junction.html)

deifobe November 3, 2011 12:51

Droplet break-up in a t-junction
 
1 Attachment(s)
Hi foamers,
I try to simulate slug flow-droplet break-up in a t-junction to compare the results to those obtained with Comsol, but the simulation result is very different, the break-up in openFoam simulation is further, also the drop form and and the detach time
is very different but I don't understand what i do wrong. Any suggestion?
I use interfoam solver, this is my BC:
-0/alpha1
inletWater
{
type fixedValue;
value uniform 1;
}
inletOil
{
type fixedValue;
value uniform 0;
}
bottom
{
type symmetryPlane;
}
outlet
{
type zeroGradient;
}

walls
{
type constantAlphaContactAngle;
theta0 135;
limit gradient;
value uniform 0;
}
- 0/p_rgh
inletOil
{
type zeroGradient;
}

inletWater
{
type zeroGradient;
}

walls
{
type fixedFluxPressure;
adjoint no;
}
bottom
{
type symmetryPlane;
}
outlet
{
type fixedValue;
value uniform 0;
}
-0/U
inletWater
{
type flowRateInletVelocity;
flowRate 5.555e-11;
value uniform (0 0 0);
}
inletOil
{
type flowRateInletVelocity;
flowRate 1.111e-10;
value uniform (0 0 0);
}
walls
{
type fixedValue;
value uniform (0 0 0);
}

bottom
{
type symmetryPlane;
}
outlet
{
type zeroGradient;
}
Attachment 9856

olivierG November 3, 2011 13:13

hello,

Can you give your fvScheme / fvSolution, or better, the case with mesh ?

Anyway, i would first change your 0/p_rgh like:
- inletOil / inletWater: outletInlet
- walls : buoyantPressure
- outlet : totalPressure

for alpha1: are you sure about 135 ? (seem big, maybe the tetha definition is not the same as comsol)

for U
- outlet : try inletOutlet or pressure(Normal ?)InletOutletVelocity

regards,
olivier

deifobe November 3, 2011 17:03

Thanks a lot for your reply! I tried your BC but result is a continuos flow but, as you say,
the problem seems to be contact angle, I will have to find and compare this angle definition in OpenFoam and in Comsol.
Thank you again.

kwardle November 4, 2011 10:27

Judging from your image, you are using a very coarse mesh. Unless you are trying to compare each code's results on the same mesh, you will want to use a much finer mesh to get anything right. Also, what kind of mesh is it? You should be able to easily use hex (blockMesh) for your geometry. You may also want to take a look at varying the cAlpha parameter in fvSolution--a value larger than 1 may result in some strange things on the interface which affect the accuracy. You have also not said what the dimensions of your problem are--different physics will affect the results depending on the scale. For example, if this is a micro channel flow (or even just 'milli' channel), then surface tension and wall contact angle will be much more important.


All times are GMT -4. The time now is 21:44.