CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Pressure rising indefinitely with rhoSimpleFoam (https://www.cfd-online.com/Forums/openfoam-solving/151735-pressure-rising-indefinitely-rhosimplefoam.html)

Werne April 16, 2015 06:21
Pressure rising indefinitely with rhoSimpleFoam
 
2 Attachment(s)
Hello,

I'm trying to simulate the flow in a conical annular gap with a rotating inner wall for my masters thesis. I'm using rhoSimpleFoam.

My Problem is, that I can't get a converged solution. Even after 100.000 Iterations the pressure continues to rise slowly.

Here are my boundary conditions, fvSolution and fvSchemes:

Code:
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  2.2.2                                |
|  \\  /    A nd          | Web:      www.OpenFOAM.org                      |
|    \\/    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;
        massFlowRate    constant 0.0038;    //0.004167
        value          uniform (0 0 0); 
    }

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

  SYM_1_OBEN
    {
        type            cyclicAMI;
    }

    SYM_1_UNTEN
    {
        type            cyclicAMI;
    }

    SYM_2_OBEN
    {
        type            cyclicAMI;
    }

    SYM_2_UNTEN
    {
        type            cyclicAMI;
    }

    MOVINGWALL_OBEN
    {
        type            rotatingWallVelocity;
    origin        (0 0 0);
    axis        (1 0 0);
    omega        838;
    }

    MOVINGWALL_UNTEN
    {
        type            rotatingWallVelocity;
    origin        (0 0 0);
    axis        (1 0 0);
    omega        838;
    }

    BOHRUNG
    {
        type            fixedValue;
        value          uniform (0 0 0);
    }

    WALL_OBEN
    {
        type            fixedValue;
        value          uniform (0 0 0);
    }

    WALL_UNTEN
    {
        type            fixedValue;
        value          uniform (0 0 0);
    }

    PLENUMWALL
    {
        type            fixedValue;
        value          uniform (0 0 0);
    }

    KEIL
    {
        type            slip;
    }

    GAP_S
    {
        type            fixedValue;
        value          uniform (0 0 0);
    }

    GAB_W
    {
        type            fixedValue;
        value          uniform (0 0 0);
    }

}
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  2.2.2                                |
|  \\  /    A nd          | Web:      www.OpenFOAM.org                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version    2.0;
    format      ascii;
    class      volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [1 -1 -2 0 0 0 0];

internalField  uniform 320000;

boundaryField
{
    INLET
    {
    type        zeroGradient;
    }

    OUTLET
    {
        type            fixedValue;
    value        uniform 220000;
    }

    SYM_1_OBEN
    {
        type            cyclicAMI;
    }

    SYM_1_UNTEN
    {
        type            cyclicAMI;
    }

    SYM_2_OBEN
    {
        type            cyclicAMI;
    }

    SYM_2_UNTEN
    {
        type            cyclicAMI;
    }

    MOVINGWALL_OBEN
    {
        type            zeroGradient;
    }

    MOVINGWALL_UNTEN
    {
        type            zeroGradient;
    }

    BOHRUNG
    {
        type            zeroGradient;
    }

    WALL_OBEN
    {
        type            zeroGradient;
    }

    WALL_UNTEN
    {
        type            zeroGradient;
    }

    PLENUMWALL
    {
        type            zeroGradient;
    }

    KEIL
    {
        type            zeroGradient;
    }

    GAP_S
    {
        type            zeroGradient;
    }

    GAB_W
    {
        type            zeroGradient;
    }
}
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  2.2.2                                |
|  \\  /    A nd          | Web:      www.OpenFOAM.org                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version    2.0;
    format      ascii;
    class      volScalarField;
    object      T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 0 1 0 0 0];

internalField  uniform 360;

boundaryField
{
    INLET
    {
        type            fixedValue;
        value          $internalField;
    }

    OUTLET
    {
        type            inletOutlet;
    inletValue    $internalField;
    value        $internalField;
    }

    SYM_1_OBEN
    {
        type            cyclicAMI;
    }

    SYM_1_UNTEN
    {
        type            cyclicAMI;
    }

    SYM_2_OBEN
    {
        type            cyclicAMI;
    }

    SYM_2_UNTEN
    {
        type            cyclicAMI;
    }

    MOVINGWALL_OBEN
    {
        type            zeroGradient;
    }

    MOVINGWALL_UNTEN
    {
        type            zeroGradient;
    }

    BOHRUNG
    {
        type            zeroGradient;
    }

    WALL_UNTEN
    {
        type            fixedValue;
        value          $internalField;
    }

    WALL_OBEN
    {
        type            fixedValue;
        value          $internalField;
    }

    PLENUMWALL
    {
        type            zeroGradient;
    }

    KEIL
    {
        type            zeroGradient;
    }

    GAP_S
    {
        type            zeroGradient;
    }

    GAB_W
    {
        type            zeroGradient;
    }
}
fvSolution:

Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  2.2.2                                |
|  \\  /    A nd          | Web:      www.OpenFOAM.org                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version    2.0;
    format      ascii;
    class      dictionary;
    location    "system";
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
 

  p
    {
    solver GAMG;
    tolerance 1e-7;  //1e-8
    relTol 0.05;
    smoother GaussSeidel;
    nPreSweeps 0;
    nPostSweeps 2;
    cacheAgglomeration on;
    agglomerator faceAreaPair;
    nCellsInCoarsestLevel 100;
    mergeLevels 1;
    }

  U
  {
        solver          smoothSolver;
        smoother        GaussSeidel;
        nSweeps        2;
        tolerance      1e-07;  ////1e-08
        relTol          0.01;
    } 

    h
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance      1e-7;  //1e-09
        relTol          0.1;
    }

    "(k|omega)"
    {
        $U;
        tolerance      1e-07;
        relTol          0.1;
    }   
 
}

SIMPLE
{
    nNonOrthogonalCorrectors 2;
    rhoMin          rhoMin [ 1 -3 0 0 0 ] 1.5;
    rhoMax          rhoMax [ 1 -3 0 0 0 ] 7;
  //  transonic    true;

    residualControl
    {
        p              1e-6;       
        U              1e-6;       
        h              1e-6;       

        // possibly check turbulence fields
          "(k|epsilon|omega)" 1e-6;   
    }
}

relaxationFactors
{
    fields
    {
        p              0.3; //0.1
        rho            0.005; //0.05
    }
    equations
    {
        U              0.7; //0.7
        k        0.7; //0.7
        omega        0.7; //0.7
        h              0.7; //0.7
    }
}
fvSchemes:

Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  2.2.2                                |
|  \\  /    A nd          | Web:      www.OpenFOAM.org                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version    2.0;
    format      ascii;
    class      dictionary;
    location    "system";
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default        steadyState;
}

gradSchemes
{
    default        Gauss linear;//cellLimited Gauss linear 1.0;    // Gauss linear;
}

divSchemes
{
    default    bounded Gauss upwind;
    div(phi,U)      bounded Gauss upwind;//bounded Gauss upwind;
    div((muEff*dev2(T(grad(U))))) Gauss linear;
    div(phi,e)      bounded Gauss upwind;
    div(phi,k)      bounded Gauss upwind;
    div(phi,omega)      bounded Gauss upwind;
    div(phi,Ekp)    bounded Gauss upwind;
}

laplacianSchemes
{
    default      Gauss linear corrected;//Gauss linear limited 0.5; //Gauss linear corrected;
}

interpolationSchemes
{
    default        linear;
}

snGradSchemes
{
    default          corrected;  //limited 0.5;
}

fluxRequired
{
    default        no;
    p              ;
}


// ************************************************************************* //
I have attached a picture of the development of the pressure in my simulation. As you can see, it rises swiftly up to a certain point and aufterwards it slows down. However, it continues to rise, no matter how long I let the simulation run.

http://www.cfd-online.com/Forums/dat...AASUVORK5CYII=I really hope, that someone can give me any hints, what I can do to stabilize my solution.

Thank you in advance!

If you need any additional information, feel free to ask :)

edit: One problem that I've found is, that the enthalpy is converging very slowly. I've attached a gnuplot graph with my residuals. Could this be the cause of my problems? If so, what can I do about it?

kamakura117 April 16, 2015 16:12
Hello:

Your enthalpy converges slowly because the pressure is constantly rising. H = U + pV

So, this comes to the pressure formulation. rhoSimpleFoam is for compressible fluids and the SIMPLE method does iterate pretty slowly between the pressure and velocity fields, so with your configuration, this is something you'll have to live with.

However, I would recommend a few changes:

1) Use rhoPimpleFoam with time-dependent solver. This will usually converged far more quickly, especially for your case.

2) Use a "totalPressure" inlet pressure condition. This will alleviate some constraints on forcing a uniform pressure field.

3) A "fixedFluxPressure" with gradient = 0, on the outlet. This again, helps a bit by giving the pressure solver a bit of flexibility on the boundary.

Werne April 16, 2015 16:43
Thank you for your answer. Regarding your suggestions:
1) I already use rhoPimpleFoam with some succes. However, the goal of my thesis is to compare the results of a transient and a stationary simulation. Therefore, I can't abandon rhoSimpleFoam.

2) I have no experience with the totalPressure boundary condition in OpenFoam. What would be the corresponding boundary condition in the velocity field? Still "flowRateInletVelocity" or would I have to change it to "zeroGradient"?

3) Basically the same questions as in 2). I have never used this boundary condition before. How do I use it? If I look in the code it says, that it sets the pressure gradient so, that it corrsponds to the flux specified in the velocity boundary condition. Does this mean, that I have to set the velocity boundary to simething like "flowRateInletVelocity"?

kamakura117 April 16, 2015 23:42
I see. You may consider initializing with your other simulation using mapFieldsDict. This can get your pressure field closer to the steady-state condition, then let the steady-state solver do it's pseudo-magic. Still, you're going to have to let the steady-state solver takes its time - the system is very stiff and the only other option is to play with your relation and preconditioners to attempt to accelerated the convergence.

Both of your questions are valid. You would need to set your velocity boundary conditions to ensure continuity and help address the stiffness of the system of equations. Depending on your physical boundaries, you might not need to be so strict; however, I would correspondingly set your intlet and outlet to flowRateInletVelocity and pressureInletOutletVelocity, respectively, where the outlet vector would simply be (0 0 0).


All times are GMT -4. The time now is 21:36.