[AnjaMiehe]

Hello everybody,

I encounter problems in simulating some kind of pipe flow. My solution domain is given in domain.jpg and the boundaries are:

• inlet: pressure inlet
• inflow walls: no-slip walls
• air gap: no-slip wall
• rolls: rotating walls
• moving sheet: moving walls
• outlet: velocity outlet (block profile)

Using any of the solvers simpleFoam, icoFoam, pisoFoam or pimpleFoam, I get the result shown in velo_pimple.png. The figure shows, that the main stream attaches to the lower roll which is slightly nearer to the inlet region than the upper role.

As I want to continue with a second phase inside this domain, I recalculated it using interFoam. Unfortunately, I obtain the result shown in figure velo_inter.png. The stream is not attaching. I do not really understand the difference. My case setup is:

alpha1

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      alpha;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [ 0 0 0 0 0 0 0 ];

internalField   uniform 0;

boundaryField
{
    roll_down
    {
        type            zeroGradient;
    }
    roll_up
    {
        type            zeroGradient;
    }
    air_cooling
    {
        type            zeroGradient;
    }
    gap
    {
        type            zeroGradient;
    }
    die
    {
        type            zeroGradient;
    }
    outlet
    {
        type            zeroGradient;
    }
    inlet
    {
        type            fixedValue;
        value           uniform 0;
    }
    frontAndBackPlanes
    {
        type            empty;
    }
}
// ************************************************************************* //

p

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform 0;

boundaryField
{
    roll_down
    {
        type            zeroGradient;
    }
    roll_up
    {
        type            zeroGradient;
    }
    air_cooling
    {
        type            zeroGradient;
    }
    gap
    {
        type            zeroGradient;
    }
    die
    {
        type            zeroGradient;
    }
    outlet
    {
        type            zeroGradient;
    }
    inlet
    {
        type            fixedValue;
        value           uniform 0;
    }
    frontAndBackPlanes
    {
        type            empty;
    }
}
// ************************************************************************* //

U

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    location    "0";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform ( 0.0358 0 0 );

boundaryField
{
    roll_down
    {
        type            rotatingWallVelocity;
        origin          ( 0 -0.4225 0 );
        axis            ( 0 0 1 );
        omega           -0.0853;
        value           uniform ( 0 0 0 );
    }
    roll_up
    {
        type            rotatingWallVelocity;
        origin          ( 0 0.4225 0 );
        axis            ( 0 0 1 );
        omega           0.0853;
        value           uniform ( 0 0 0 );
    }
    air_cooling
    {
        type            fixedValue;
        value           uniform ( 0.0358 0 0 );
    }
    gap
    {
        type            fixedValue;
        value           uniform ( 0 0 0 );
    }
    die
    {
        type            fixedValue;
        value           uniform ( 0 0 0 );
    }
    outlet
    {
        type            fixedValue;
        value           uniform ( 0.0358 0 0 );
    }
    inlet
    {
        type            zeroGradient;
    }
    frontAndBackPlanes
    {
        type            empty;
    }
}
// ************************************************************************* //

fvSchemes

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default         Euler;
}

gradSchemes
{
    default         Gauss linear;
}

divSchemes
{
    div(rho*phi,U)  Gauss limitedLinearV 1;
    div(phi,alpha)  Gauss vanLeer;
    div(phirb,alpha) Gauss interfaceCompression;
}

laplacianSchemes
{
    default         Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default         no;
    p_rgh;
    pcorr;
    alpha1;
}
// ************************************************************************* //

fvSolution

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    pcorr
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-10;
        relTol          0;
    }

    p_rgh
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-07;
        relTol          0.05;
    }

    p_rghFinal
    {
        $p_rgh;
        tolerance       1e-07;
        relTol          0;
    }

    U
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-06;
        relTol          0;
    }
}

PIMPLE
{
    momentumPredictor no;
    nCorrectors     3;
    nNonOrthogonalCorrectors 0;
    nAlphaCorr      1;
    nAlphaSubCycles 2;
    cAlpha          1;
}
// ************************************************************************* //

controlDict

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application     interFoam;

startFrom       latestTime;

startTime       0;

stopAt          endTime;

endTime         10;

deltaT          0.00125;

writeControl    adjustableRunTime;

writeInterval   0.2;

purgeWrite      0;

writeFormat     ascii;

writePrecision  6;

writeCompression uncompressed;

timeFormat      fixed;

timePrecision   6;

graphFormat     gnuplot;

runTimeModifiable yes;

adjustTimeStep  yes;

maxCo           0.9;
maxAlphaCo      0.9;

maxDeltaT       0.1;
// ************************************************************************* //

The turbulence model is laminar.
Does someone have an idea where this difference might come from?
Thanks in advance, Anja

[vonboett]

Hello,

I am facing funny problems with alpha1 that didn't occur when OF 1.7.1 was used, so my intention is that using PIMPLE instead of PISO changes the situation. The problem occuring in other threads, too, is that if one has a simple outflow for example in a freeface channel, the alpha1 phase gets reflected at the outflow instead of leaving the domain. Any new hints?

[AnjaMiehe]

Hello Albrecht,
I tried my case in 1.7.1 after your hint, but without success. The velocity field looks the same as above for InterFoam, but it was worth a try. Maybe I try to find something different from the outflow.
Regards, Anja

[vonboett]

Hello Anja,

meanwhile I tried the outflow with:

U:
{
type inletOutlet;
inletValue uniform (0 0 0);
}
p_rgh:
{
type outletInlet;
outletValue uniform 0;
}
alpha1:
{
type zeroGradient;
}
which works fine in interFoam of OF 2.0. In about 8 hours I can tell more if it works with interFoam OF 2.1 set back to PISO. If I am the only one with these differences between the versions I have to check my Ubuntu installation, maybe the last update caused some weired change.

[AnjaMiehe]

Hello Albrecht,

I have tried the InletOutlet with my case in 2.1.0 and 1.7.1 . It is a bit better but not the desired result. When I have some free cores, I will try different methods in fvSchemes and / or the fvSolution. I post the velocity results in a picture below. How does your case go?

Regards,
Anja

[vonboett]

Ok turning old searching the cause of alpha1 being reflected at the outflow, I finally got it. Maybe this is a bug dependent on ubuntu version, but it is quite relevant. The difference between the two pictures below showing an outflow of a channel is only that I moved the grid from positive x quadrant to negative x quadrant. When the whol gid lies at a position that the x-coordinates are smaller than 0 the outflow works! Maybe this should be reported. I attatched the cases at my post in http://www.cfd-online.com/Forums/ope...tml#post362833 today (24.5.12)

[AnjaMiehe]

Hello Albrecht,
Thanks for the hint with negative x. Now I get the results from InletOutlet with outflow as well. The rest might really be fvSolution and fvSchemes.
Regards, Anja

[vonboett]

Meanwhile I reproduced the bug as well on a Mac OSX 10.6.5 intel with OF 1.7.x.
The case showing the reflection at the outlet is attatched, again the error vanishes when moving the mesh by -7 m in x direction to the negative quadrant. The attachment skipped the polyMesh folder due to file size, yust create the folder and move the blockMeshDict located at constant in it.

[vonboett]

...with p_rgh zeroGradient at the outlet it works fine, tested in OF 1.7.x and in OF 2.1.x. Anyway I'd be happy for any explanation why a fixedValue 0 boundary condition for p_rgh causes phase reflection only if one translates the mesh location from negative x-coordinates to positive x-coordinates.