[dachs]

Hi Foamers,


I have the following Problem, i want to simulate the oil flow through a pipe, where the fluid come in contact with three rotating clyinders. I use the interFoam Solver. My BC for each rotating surface is:

0/U


roller
    {
    type            rotatingWallVelocity;        
    origin          (0 -0.0832 0);         
    axis            (0 0 1);
    omega           -98;         
    }





0/p_rgh


roller
        {
        type            fixedFluxPressure;
        value           uniform 0;
     }




0/nut


roller
        {
        type            nutkWallFunction;
    value        uniform 0;
     }




0/k


roller
    {
    type            kqRWallFunction;
    value        uniform 0;
     }


0/epsilon


roller
    {
    type            epsilonWallFunction;
    value           $internalField;
    }




0/alpha.oil
roller
    {
    type            zeroGradient;
    }

running this code will lead to the error Message:

--> FOAM FATAL ERROR:
Continuity error cannot be removed by adjusting the outflow.
Please check the velocity boundary conditions and/or run potentialFoam to initialise the outflow.
Total flux              : 2.22507e-308
Specified mass inflow   : 3.98506e-18
Specified mass outflow  : 4.06142e-18
Adjustable mass outflow : 0

Can anyone tell me what is wrong with my BC? All the other walls that are displayed are defined as walls and not as patches.


Mesh.jpgPhases.png

[tomf]

Hi,

It seems like you have no inlets or outlets and the solver therefore does not know a reference pressure to set.

You probably need to define a pRefCell or pRefPoint with a pRefValue in your fvSolution file (in the PIMPLE subDict). An example may be found in $FOAM_TUTORIALS/multiphase/interFoam/laminar/sloshingTank2D, copied here:

PIMPLE
{
    momentumPredictor no;
    nCorrectors     2;
    nNonOrthogonalCorrectors 0;
    correctPhi      no;
    pRefPoint       (0 0 0.15);
    pRefValue       1e5;
}

Good luck,
Tom