Problem with InterFoam.
 

Hi， I am trying to simulate a liquid droplet emerging from a pore on bottom of a cubic channel using interFoam(1.6.x). Gas was introduced from one side. But I didnot find any droplet at all, the total volume fraction of water did not change much (kept very small, e.g 1e-5).

Then I tried to increase the liquid velocity (from 0.1 to 1m/s), now I can get a droplet, the volume fraction was more than 0.1(makes sense). I was really confused by this result. Is there any limitation of InterFoam? Thanks a lot!


btw: fvscheme and fvsolution are the same as dambreak
=======0/alpha======
{
water_inlet
{
type fixedValue;
value uniform 1;
}
outlet
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}
gas_inlet
{
type fixedValue;
value uniform 0;
}
wall
{
type constantAlphaContactAngle;
theta0 140;
thetaA 170;
thetaR 90;
uTheta 1;
value uniform 1;
}
======0/U========
{
water_inlet
{
type fixedValue;
value uniform (0 0 0.0625);
}
outlet
{
type inletOutlet;
value uniform (0 0 0);
inletValue uniform ( 0 0 0 );
}
gas_inlet
{
type fixedValue;
value uniform (0 10 0);
}
wall
{
type fixedValue;
value uniform (0 0 0);
}
}
======0/p========
boundaryField
{
water_inlet
{
type zeroGradient;
}
outlet
{
type fixedValue;
value uniform 0;
}
gas_inlet
{
type zeroGradient;
}
wall
{
type zeroGradient;
}
}

I have done a similar work in my bachelor thesis.
The simulation was done by injecting a continous gas flow into a stagnant liquid.

During the simulation I encountered severe problems with "small" inflow rates.
It was evident that there was some loss of mass, as the liquid volume fraction was not changing although gas was flowing into the domain.

My "explanation" to this observation was the influence of parasitic currents in the proximity of the interface which was very close to the inflow in my case.

If the magnitude of the parasitic currents and the inflow velocity are close to each other (as it was in my case) some kind of interaction is highly probable!

Thank you for your reply!

I used Fluent before, and these never happened even the flow rates was much lower. However, I really wanna use OPENFOAM for my research, is there any way to deal with that?

by the way, I am not quite understand the term "parasitic current", could you give me more explanation? Thanks a lot!

"Parasitic currents" are known as unphysical velocity fields in the proximity of a resting interface. Theoretically all velocities should be zero in a flow field if the interface is not moving. Yet you will allways examine a velocity field if you use the CSF-Model (Continuum-Surface-Modell) for the representation of surface-tension which is used in interFoam.

Have a look at this picture of a static drop which shows parasitic currents:

http://www.familie-gatzka.de/openfoa...teCurrents.png

The CSF-model itself is introduced by Brackbill & al. "A Continuum Method for modeling Surface Tension" Journal of Compuational Physics, 100:335-354, 1992. The reasons of parasitic currents and its effects on the flow are discussend there.

The term "parasitic currents" was first introduced by Lafaurie et. al. "Modelling Merging and Fragmentation in Multiphase Flow with SURFER". Journal of Computational Physics. 113:134-147, 1994.

You will find a whole bunch of papers about this problem and even here it was discussed just yesterday:
http://www.cfd-online.com/Forums/ope...-currents.html

The magnitude of the parasitic currents scale with the fluid properties and with the "quality" of the solver. Please refer for the literature above for more details.

So maybe you will be able to simulate your cases with some restrictions on the fluid properties.

Really thanks your kind help. Seems I have a lot to learn :)