[msabger]

Hi

I've already posted in the "OpenFOAM Running / Solving / CFD" section about this issue, but I'm starting to think that may be there is a bug in the interMixingFoam.

I tried to test the interMixingFoam solver when studing gravity currents. So I took the tutorial example but changing the initial alpha fields. The initial condition is a horizontal free surface, and two separated phases, with different densities (I attach the whole example).

I expected to see the gravity currents due the difference in density, but both liquid phases behave as they have the same properties.

What could it be wrong?

Thanks!

Martin

[mattijs]

We've finally got a proper bug reporting system :-)
Please report any OpenFOAM bugs on http://www.openfoam.com/bugs.

[nbadano]

Dear Martin,

There's indeed a bug in interMixingFoam. The solvers incorrectly assigns the properties of phase 2 to phase 3, so both are identical, preventing the development of any density current.

I found the bug in threePhaseMixture.C, located under /opt/openfoam171/applications/solvers/multiphase/inaMixingFoam/incompressibleThreePhaseMixture/

In lines 79 to 88 you should replace this piece of the constructor code:

    nuModel3_
    (
        viscosityModel::New
        (
            "nu3",
            subDict(phase2Name_),
            U,
            phi
        )
    ),

by this:

    nuModel3_
    (
        viscosityModel::New
        (
            "nu3",
            subDict(phase3Name_),
            U,
            phi
        )
    ),

After that, just recompile the solver with wmake.

I was able to run your test case without any problem after this modification. It works beautyfully. I've uploaded a couple of pics of the resulting alpha3.


Hope this helps.

Best regards!

Nicolas

[nbadano]

Although we never actually reported the bug officially, it seems to be corrected in the last 1.7.x version of OpenFOAM!

Nicolas

[sarahk]

Hey guys,

i know my probelm doesnt fit that well in this Thread, but as you used interMixingFoam already i thought you might be able to help me

i have a huge vessel with a tap (an electrical arc furnace). So, inside i have steel, slag and air. And i wanna simulate at wich level the slag flows into the tap. and I dont want steel and slag to mix (D=0, am i right??).

my bc´s:
phase 2 and 3 are slag and steel.
the field has a really small velocity in -y
g (0 -9,81 0) at beginning.

what happens is, that Foam stops after the first time step (0,005) and i have a velocity from 600 m/s at the Outlet.

Any Ideas?

Thanks in advance

Sarah

[nbadano]

Hey Sarah,

I don't really know much about metallurgy but; do slag and steel behave as separate phases (with sharp interface maintained by surface tension)?? If that's the case I think you should use multiphaseInterFoam instead of interMixingFoam. multiphaseInterFoam solves for n inmiscible phases. Maybe D=0 is not very interMixingFoam friendly!

On the other hand, 600 m/s in 0.005 secs sounds like an inconsistency in BCs or a mesh problem (any bad elements according to checkMesh?). Can't really pinpoint anything more concrete without having a look at the actual case directory.

Hope this helps!

Best regards

Nico

[sarahk]

HEy Nico,

thanks i´ll give multiphaseInterFoam a try

the Mesh is ok (i did the calculation in fluent before), but i think it really has a problem with the D=0, and how you use the phases. I changed steel against air (just to try it) and it worked much better (solution was senseless, anyway )

do you if there is still a bug in gravity? When i checked my Solutions i had air blowing through the tap in the steel, without patching any velocity ...

Greetings,

Sarah