Pressure rising indefinitely with rhoSimpleFoam

Werne · April 16, 2015, 06:21

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.

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).

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Pressure Inlet VS velocity Inlet difference	Mohsin	FLUENT	9	January 4, 2021 10:34
Pressure Outlet Guage pressure	Mohsin	FLUENT	36	April 29, 2016 17:16
Calculation of the Governing Equations	Mihail	CFX	7	September 7, 2014 06:27
Fluent natural ventilation pressure boundary condition	pierresandre	FLUENT	24	November 8, 2011 14:32
pressure is not rising in compression stroke..	chetan	CFX	0	June 17, 2008 03:13

April 16, 2015, 16:12		#2
kamakura117 New Member N/A Join Date: Jul 2010 Posts: 29 Rep Power: 15	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.

April 16, 2015, 16:43		#3
Werne New Member Join Date: Feb 2013 Posts: 17 Rep Power: 13	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"?

April 16, 2015, 23:42		#4
kamakura117 New Member N/A Join Date: Jul 2010 Posts: 29 Rep Power: 15	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).