[Jahir]

Hello.


As you all know, the implementation of cases that go beyond what the tutorials offer is a bit complicated sometimes. I started using interFoam last year and it's mostly worked out well, but I'm not sure I'm using the boundary condition my model requires.


In short, I'd like to know if this is the best way to approach outlets that are open to both fluids (n \cdot T = nP_{atm}). This are the files contained in the 0 directory:


alpha.water

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  8
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      alpha.water;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 0 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    inlet
    {
        type            fixedValue;
        value           uniform 1;
    }

    walls
    {
        type            zeroGradient;
    }

    outlet
    {
        type            zeroGradient;
        value           uniform 0;
    }

    atmosphere
    {
        type            inletOutlet;
        inletValue      uniform 0;
        value           uniform 0;
    }
}

// ************************************************************************* //

U

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  8
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    inlet
    {
        type            flowRateInletVelocity;
        volumetricFlowRate constant 10.7;
    }

    walls
    {
        type            noSlip;
    }

    atmosphere
    {
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
    }

    outlet
    {
        type            inletOutlet;
        inletValue      uniform (0 0 0);
        value           $internalField;
    }
}


// ************************************************************************* //

p_rgh

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  8
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [1 -1 -2 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    atmosphere
    {
        type            totalPressure;
        p0              uniform 0;
    }

    ".*"
    {
        type            fixedFluxPressure;
        value           uniform 0;
    }
}

// ************************************************************************* //

I tried with totalPressure for the p_rgh condition at the outlets but it crashed. Since my goemetry is too big I can't say for certain that these are wrong, but I'm not sure these are the best BCs I could use for my simulation. I also checked the veolcities (and volumetric flows) at these boundaries and I think the values are too small.


Thank you very much in advance!

[Alczem]

Hey,


What are you trying to simulate? An open channel? Can you share a picture of your geometry?

[Jahir]

Originally Posted by Alczem

Hey,


What are you trying to simulate? An open channel? Can you share a picture of your geometry?

It's a tank meant for separating water and sediment. To the left is the inlet and there are 4 outlets that are on the right side.

[Alczem]

Hey,


My usual setup for this kind of simulation is the following:

• Initialise the water field with setFields at the proper height
• Add a hRef file in constant/ with the height corresponding to the water level
• For alpha.water and U at the inlet, use variableHeightFlowRate and variableHeightFlowRateInletVelocity
• For the outlets, inletOutlet and pressureInletOutletVelocity are ok
• totalPressure should work at the outlets

This usually works for my cases. hRef is necessary if your water level is different from z=0m. It represents the waterlevel outside the domain (= beyond the outlet, there is still water and not void) if that makes sense, and prevents the water from "falling" at the outlet.