Compressor Simulation using rhoPimpleDyMFoam

Jetfire · October 22, 2014, 07:25

Hi

I am simulating compressor stage of a turbocharger with the rhoPimpleDyMFoam solver. running moveDynamicMesh -checkAMI was smooth without any errors which assures that my mesh rotates properly and i have defined my interfaces correctly , please point out if i am assuming this wrong.

However running the solver my simulation crashes showing this

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.3.0-f5222ca19ce6
Exec   : rhoPimpleDyMFoam
Date   : Oct 22 2014
Time   : 15:58:22
Host   : "EAT-Standalone"
PID    : 4587
Case   : /home/eatin/OpenFOAM/eatin-2.3.0/run/tutorials/TurboCharger/Trial_4
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Selecting dynamicFvMesh solidBodyMotionFvMesh
Selecting solid-body motion function rotatingMotion
Applying solid body motion to cellZone FLUID_ROTOR

PIMPLE: Operating solver in PISO mode

Reading thermophysical properties

Selecting thermodynamics package 
{
    type            hePsiThermo;
    mixture         pureMixture;
    transport       sutherland;
    thermo          hConst;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleEnthalpy;
}

AMI: Creating addressing and weights between 1900 source faces and 32076 target faces
AMI: Patch source sum(weights) min/max/average = 0.995594, 1, 0.999764
AMI: Patch target sum(weights) min/max/average = 0.432794, 1, 0.996788
AMI: Creating addressing and weights between 17748 source faces and 5456 target faces
AMI: Patch source sum(weights) min/max/average = 0.435302, 1.03344, 1.00009
AMI: Patch target sum(weights) min/max/average = 0.816766, 1.00271, 0.999924
AMI: Creating addressing and weights between 17839 source faces and 1957 target faces
AMI: Patch source sum(weights) min/max/average = 0.86998, 1, 0.999108
AMI: Patch target sum(weights) min/max/average = 0.991279, 1, 0.99992
Reading field U

Reading/calculating face flux field phi

Creating turbulence model

Selecting turbulence model type RASModel
Selecting RAS turbulence model kEpsilon
#0  Foam::error::printStack(Foam::Ostream&) in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::compressible::mutkWallFunctionFvPatchScalarField::calcMut() const in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#4  Foam::compressible::mutWallFunctionFvPatchScalarField::updateCoeffs() in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#5  Foam::fvPatchField<double>::evaluate(Foam::UPstream::commsTypes) in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/bin/rhoPimpleDyMFoam"
#6  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::evaluate() in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/bin/rhoPimpleDyMFoam"
#7  Foam::compressible::RASModels::kEpsilon::kEpsilon(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::fluidThermo const&, Foam::word const&, Foam::word const&) in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#8  Foam::compressible::RASModel::adddictionaryConstructorToTable<Foam::compressible::RASModels::kEpsilon>::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::fluidThermo const&, Foam::word const&) in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#9  Foam::compressible::RASModel::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::fluidThermo const&, Foam::word const&) in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#10  Foam::compressible::turbulenceModel::addturbulenceModelConstructorToTable<Foam::compressible::RASModel>::NewturbulenceModel(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::fluidThermo const&, Foam::word const&) in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#11  Foam::compressible::turbulenceModel::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::fluidThermo const&, Foam::word const&) in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleTurbulenceModel.so"
#12  
 in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/bin/rhoPimpleDyMFoam"
#13  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#14  
 in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/bin/rhoPimpleDyMFoam"
Floating point exception (core dumped)

I am not able to identify what exactly is the problem and i suppose this is not due to the AMI interfaces as moveDynamicMesh was running perfectly. I have understood after reading few threads that it might be related to my boundary conditions, fvSchemes or fvSolution but i have no idea how to correct this. Please help me solve this and let me know if you need anymore details regarding my simulation.

Thanks

Jetfire · October 22, 2014, 07:35

Coming to my simulation i have to simulate compressor stage of a turbocharger
Meshing was done using ANSYS ICEM CFD , i had 3 mesh files
1. Inlet&Outlet
2.Volute
3.Rotor
I imported them to openfoam using fluent3DMeshToFoam and then used mergeMeshes to make the complete domain, after that used
splitMeshRegions -makeCellZones -overwrite to distinguish between the rotating zone and stationary zone.

I am attaching few pictures of the domain so you could get a clear picture.Please have a look at them

Jetfire · October 22, 2014, 07:38

This is the complete domain of my simulation

vasava · October 22, 2014, 08:39

1. How are you merging your three meshes that you have imported from fluent?
2. How did you create AMI patches?
3. Do you have 'sets' folder (with several domains) inside the constant folder?

Jetfire · October 23, 2014, 04:36

@vasava

As i have 3 mesh files
1.I created 3 case folders 1.Rotor 2.Volute 3.Inlet_Outlet
2. Placed the 3 mesh files into corresponding case folders and used fluent3DMeshToFoam fluent.msh -scale 0.001 for each to convert to meters
3.merged Rotor and volute , and then merged the combined mesh with Inlet_Outlet
4.used splitMeshRegions -makeCellZones -overwrite to create cell zones of different regions , 3 in my case

To create the AMI patches i used the createPatchDict, I will attach it for your reference

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      createPatchDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

// Do a synchronisation of coupled points after creation of any patches.
// Note: this does not work with points that are on multiple coupled patches
//       with transformations (i.e. cyclics).
pointSync false;

// Patches to create.
patches
(
    {
        //- Master side patch
        name            AMI1;
        patchInfo
        {
            type            cyclicAMI;
            matchTolerance  0.0001;
            neighbourPatch  AMI2;
            transform       noOrdering;
       
        }
        constructFrom patches;
        patches (INT_STA_ROT_master);
    }

    {
        //- Slave side patch
        name            AMI2;
        patchInfo
        {
            type            cyclicAMI;
            matchTolerance  0.0001;
            neighbourPatch  AMI1;
            transform       noOrdering;
       
        }
        constructFrom patches;
        patches (INT_STA_ROT_slave);
    }

    {
        //- Master side patch
        name            AMI3;
        patchInfo
        {
            type            cyclicAMI;
            matchTolerance  0.0001;
            neighbourPatch  AMI4;
            transform       noOrdering;
            
        }
        constructFrom patches;
        patches (INT_ROT_STA_master);
    }

    {
        //- Slave side patch
        name            AMI4;
        patchInfo
        {
            type            cyclicAMI;
            matchTolerance  0.0001;
            neighbourPatch  AMI3;
            transform       noOrdering;
        
        }
        constructFrom patches;
        patches (INT_ROT_STA_slave);
    }


    {
        //- Master side patch
        name            AMI5;
        patchInfo
        {
            type            cyclicAMI;
            matchTolerance  0.0001;
            neighbourPatch  AMI6;
            transform       noOrdering;
            
        }
        constructFrom patches;
        patches (INT_OUTLET_HOUSING_master);
    }

    {
        //- Slave side patch
        name            AMI6;
        patchInfo
        {
            type            cyclicAMI;
            matchTolerance  0.0001;
            neighbourPatch  AMI5;
            transform       noOrdering;
            
        }
        constructFrom patches;
        patches (INT_OUTLET_HOUSING_slave);
    }

);

Yes, i have sets in my constant folder with different domains

tomf · October 23, 2014, 06:50

Hi,

Your problem seems to be in the turbulence model, I am guessing you have put epsilon equal to zero somewhere in either a boundary patch or the internalField. Change this to a sensible value for your case.

Regards,
Tom

vasava · October 23, 2014, 10:01

Your mesh setup seems alright. I agree with tomf, get some appropriate values for turbulence and use them in initial condition.

Also can you post your boundary file here?

Jetfire · October 27, 2014, 02:04

Hi ,

Sorry for the late reply and thanks for your response
I have checked my epsilon file and have not put zero anywhere and ya as you have suggested i am working on my initial and boundary conditions as this might be the source of error.

@vasava
Here is my boundary file

Code:

FoamFile
{
    version     2.0;
    format      binary;
    class       polyBoundaryMesh;
    location    "constant/polyMesh";
    object      boundary;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

16
(
    WALL_HUB
    {
        type            wall;
        inGroups        1(wall);
        nFaces          32413;
        startFace       16826280;
    }
    WALL_BACK_PLATE_ROT
    {
        type            wall;
        inGroups        1(wall);
        nFaces          14330;
        startFace       16858693;
    }
    WALL_SHOURD
    {
        type            wall;
        inGroups        1(wall);
        nFaces          36540;
        startFace       16873023;
    }
    WALL_BLADE
    {
        type            wall;
        inGroups        1(wall);
        nFaces          96768;
        startFace       16909563;
    }
    WALL_HOUSING
    {
        type            wall;
        inGroups        1(wall);
        nFaces          265149;
        startFace       17006331;
    }
    WALL_BACK_PLATE_STA
    {
        type            wall;
        inGroups        1(wall);
        nFaces          39172;
        startFace       17271480;
    }
    WALL_FREESLIP_INLET
    {
        type            wall;
        inGroups        1(wall);
        nFaces          6004;
        startFace       17310652;
    }
    WALL_FREESLIP_OUTLET
    {
        type            wall;
        inGroups        1(wall);
        nFaces          17404;
        startFace       17316656;
    }
    OUTLET
    {
        type            patch;
        nFaces          1957;
        startFace       17334060;
    }
    INLET
    {
        type            patch;
        nFaces          2945;
        startFace       17336017;
    }
    AMI1
    {
        type            cyclicAMI;
        inGroups        1(cyclicAMI);
        nFaces          1900;
        startFace       17338962;
        matchTolerance  0.0001;
        transform       noOrdering;
        neighbourPatch  AMI2;
     
    }
    AMI2
    {
        type            cyclicAMI;
        inGroups        1(cyclicAMI);
        nFaces          32076;
        startFace       17340862;
        matchTolerance  0.0001;
        transform       noOrdering;
        neighbourPatch  AMI1;
      
    }
    AMI3
    {
        type            cyclicAMI;
        inGroups        1(cyclicAMI);
        nFaces          17748;
        startFace       17372938;
        matchTolerance  0.0001;
        transform       noOrdering;
        neighbourPatch  AMI4;
       
    }
    AMI4
    {
        type            cyclicAMI;
        inGroups        1(cyclicAMI);
        nFaces          5456;
        startFace       17390686;
        matchTolerance  0.0001;
        transform       noOrdering;
        neighbourPatch  AMI3;
        
    }
    AMI5
    {
        type            cyclicAMI;
        inGroups        1(cyclicAMI);
        nFaces          17839;
        startFace       17396142;
        matchTolerance  0.0001;
        transform       noOrdering;
        neighbourPatch  AMI6;
        
    }
    AMI6
    {
        type            cyclicAMI;
        inGroups        1(cyclicAMI);
        nFaces          1957;
        startFace       17413981;
        matchTolerance  0.0001;
        transform       noOrdering;
        neighbourPatch  AMI5;
        
    }
)

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

One question , I have many boundaries i.e 16 in my boundary file. Is it necessary to define initial and boundary conditions for all these in my 0 folder?

vasava · October 27, 2014, 02:20

Quote:

Originally Posted by Jetfire

Hi ,
One question , I have many boundaries i.e 16 in my boundary file. Is it necessary to define initial and boundary conditions for all these in my 0 folder?

Yes you have to else openFoam will complain even before your calculation starts.

The boundary file looks ok but did you try any other turbulence setup??

Jetfire · October 27, 2014, 02:30

Hi vasava,

Do you mean any of these two? I started with K-Epsilon as it was the basic turbulence model to start with.
1.K-omega SST
2.Spalart-Allmaras

I am attaching my 0 folder , please take a look at my initial and boundary conditions and help me correct them. I have copied and modified the files from annularThermalMixer tutorial.

tomf · October 27, 2014, 05:16

You have provided a relative pressure of 0 Pa, you should put the absolute pressure. OpenFOAM does not use a "gauge pressure" or similar for compressible solvers. The solver now tried to solve for an absolute vacuum, which it could not do. I guess it only found out when density was required to calculated some part of the turbulence model.

For incompressible cases 0 m2/s2 is allowed since in that case the absolute pressure does not matter.

Regards,
Tom

Jetfire · October 27, 2014, 06:02

Quote:

Originally Posted by tomf

You have provided a relative pressure of 0 Pa, you should put the absolute pressure. OpenFOAM does not use a "gauge pressure" or similar for compressible solvers. The solver now tried to solve for an absolute vacuum, which it could not do. I guess it only found out when density was required to calculated some part of the turbulence model.

For incompressible cases 0 m2/s2 is allowed since in that case the absolute pressure does not matter.

Regards,
Tom

Hi tomf,
I changed the pressure file as suggested by you creating a pressure difference between inlet and outlet but i still end up getting the same error .

Alexeym has suggested this might be the cause of my error:

Hi,

as you've got FPE in mutkWallFunctionFvPatchScalarField::calcMut(), look at the source of the wall function:

Code:

tmp<scalarField> mutkWallFunctionFvPatchScalarField::calcMut() const
{
    const label patchi = patch().index();
    const turbulenceModel& turbModel =
        db().lookupObject<turbulenceModel>("turbulenceModel");
    const scalarField& y = turbModel.y()[patchi];
    const scalarField& rhow = turbModel.rho().boundaryField()[patchi];
    const tmp<volScalarField> tk = turbModel.k();
    const volScalarField& k = tk();
    const scalarField& muw = turbModel.mu().boundaryField()[patchi];

    const scalar Cmu25 = pow025(Cmu_);

    tmp<scalarField> tmutw(new scalarField(patch().size(), 0.0));
    scalarField& mutw = tmutw();

    forAll(mutw, faceI)
    {
        label faceCellI = patch().faceCells()[faceI];

        scalar yPlus =
            Cmu25*y[faceI]*sqrt(k[faceCellI])/(muw[faceI]/rhow[faceI]);

        if (yPlus > yPlusLam_)
        {
            mutw[faceI] = muw[faceI]*(yPlus*kappa_/log(E_*yPlus) - 1);
        }
    }

    return tmutw;
}

There's several possible reasons for FPE:
1. rhow[faceI] == 0
2. muw[faceI] == 0
3. k[faceCellI] < 0
4. E_*yPlus <= 0 (this is not the case, cause yPlus > yPlusLam_)

So you need to check if any of conditions 1-3 is true in your case.

I am able to figure out that these conditions come from the equations to have a proper solution but unable to understand which values i should correct.Please explain me if you can interpret what the problem exactly is.

Thanks

tomf · October 27, 2014, 06:09

Could you just show the p file, I was not talking about a pressure difference between inlet and outlet, I meant that you cannot have 0 Pa anywhere in the domain (internalField or any boundary condition), it should be around your absolute operating pressure (101325 Pa for standard atmosphere conditions).

I guess it should look something like this:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      binary;
    class       volScalarField;
    location    "0";
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform 101325;

boundaryField
{
    WALL_HUB
    {
        type            zeroGradient;
    }
    OUTLET
    {
        type            fixedValue;
        value           uniform 101325;
    }
    INLET
    {
        type            zeroGradient;
    }
    WALL_BACK_PLATE_ROT
    {
        type            zeroGradient;
    }
    WALL_SHOURD
    {
        type            zeroGradient;
    }
    WALL_BACK_PLATE_STA
    {
        type            zeroGradient;
    }
    WALL_BLADE
    {
        type            zeroGradient;
    }
    WALL_HOUSING
    {
        type            zeroGradient;
    }
    WALL_FREESLIP_INLET
    {
        type            zeroGradient;
    }
    WALL_FREESLIP_OUTLET
    {
        type            zeroGradient;
    }
    AMI1
    {
        type            cyclicAMI;
        value           uniform 101325;
    }
    AMI2
    {
        type            cyclicAMI;
        value           uniform 101325;
    }
    AMI3
    {
        type            cyclicAMI;
        value           uniform 101325;
    }
    AMI4
    {
        type            cyclicAMI;
        value           uniform 101325;
    }
    AMI5
    {
        type            cyclicAMI;
        value           uniform 101325;
    }
    AMI6
    {
        type            cyclicAMI;
        value           uniform 101325;
    }
}


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

Regards,
Tom

Jetfire · October 27, 2014, 06:31

@tomf,

Thank you very much.
Just changed my p-file as suggested by you, now my simulation started running!!

I was always worried about the mut-file , dint expect the error was in my p-file.

For now the simulation is running but too slow,have to run it in parallel and maybe some changes in my fvSchemes and fvSolution will do. il come back to you in case of any queries, thanks a lot!

Jetfire · November 6, 2014, 04:02

Hi ,

I am simulating compressor of a turbocharger using rhoPimpleDyMFoam with kOmegaSST turbulence model.
Boundary conditons are as follows:

mass flow outlet : 0.04 kg/s
total pressure inlet:101325
total temperature inlet:298k
compressor rpm: 300,000

Can you help me with my FvSchemes and FvSolutions as to what modifications i should be doing for better results. let me know if you need any more details about the simulation.

FvSchemes

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default         Euler;
}

gradSchemes
{
    default         Gauss linear;
}

divSchemes
{
    default         none;

    div(phi,U)      Gauss linearUpwind grad(U);
    div(phi,h)      Gauss linearUpwind grad(h);
    div(phi,K)      Gauss linear;
    div(meshPhi,p)  Gauss linear;
    div(phi,k)      Gauss upwind;
    div(phi,omega) Gauss upwind;
    div((muEff*dev2(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
    default         Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default         no;
    p               ;
    pcorr           ;
}


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

FvSolution

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    p
    {
        solver           GAMG;
        smoother         GaussSeidel;
        cacheAgglomeration on;
        agglomerator     faceAreaPair;
        nCellsInCoarsestLevel 10;
        mergeLevels      1;
        tolerance       1e-6;
        relTol          0.01;
    }

    pFinal
    {
        $p;
        relTol          0;
    }

    pcorr
    {
        $p;
        tolerance       1e-2;
        relTol          0;
    }

    "(rho|U|h|k|epsilon|omega)"
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-06;
        relTol          0.1;
    }

    "(rho|U|h|k|epsilon|omega)Final"
    {
        $U;
        relTol          0;
    }

}

PIMPLE
{
    momentumPredictor   yes;
    transonic           no;
    nOuterCorrectors    1;
    nCorrectors         3;
    nNonOrthogonalCorrectors 1;
    rhoMin          rhoMin [ 1 -3 0 0 0 ] 0.5;
    rhoMax          rhoMax [ 1 -3 0 0 0 ] 2.0;
}

relaxationFactors
{
    fields
    {
    }
    equations
    {
        "(U|h|k|epsilon|omega).*" 1;
    }
}


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

Thanks

RodriguezFatz · November 6, 2014, 10:24

Whats the matter with your current results? Any problems?

Jetfire · November 7, 2014, 00:00

Hi RodriguezFatz,

I have started running the simulation and each timestep is taking a lot of time. Is there anything to do with my FvSolution or FvSchemes files to speed up my simulation? I am already running it on 8 cores.

Tobi · November 7, 2014, 03:26

So at least there is no problem ...

Jetfire · November 7, 2014, 03:33

Hi tobi,

My simulation has been running from past 1 day and still going on
Here is the output

Code:

Courant Number mean: 0.000114809 max: 1
deltaT = 1.41799e-09
Time = 5.81839e-07

solidBodyMotionFunctions::rotatingMotion::transformation(): Time = 5.81839e-07 transformation: ((0 0 0) (0.999958 (0.00913938 0 0)))
AMI: Creating addressing and weights between 1900 source faces and 32076 target faces
AMI: Patch source sum(weights) min/max/average = 0.99546, 1, 0.999763
AMI: Patch target sum(weights) min/max/average = 0.467982, 1, 0.996805
AMI: Creating addressing and weights between 17748 source faces and 5456 target faces
AMI: Patch source sum(weights) min/max/average = 0.538509, 1.06046, 1.00015
AMI: Patch target sum(weights) min/max/average = 0.685009, 1.00305, 0.999864
AMI: Creating addressing and weights between 17839 source faces and 1957 target faces
AMI: Patch source sum(weights) min/max/average = 0.86998, 1, 0.999108
AMI: Patch target sum(weights) min/max/average = 0.991279, 1, 0.99992
GAMG:  Solving for pcorr, Initial residual = 1, Final residual = 0.00998453, No Iterations 47
GAMG:  Solving for pcorr, Initial residual = 0.0244185, Final residual = 0.00465247, No Iterations 1
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
rhoEqn max/min : 2.15688 0.182153
smoothSolver:  Solving for Ux, Initial residual = 3.26172e-05, Final residual = 2.14196e-09, No Iterations 1
smoothSolver:  Solving for Uy, Initial residual = 0.00157835, Final residual = 1.29594e-07, No Iterations 1
smoothSolver:  Solving for Uz, Initial residual = 0.00176688, Final residual = 1.35932e-07, No Iterations 1
smoothSolver:  Solving for h, Initial residual = 0.000933756, Final residual = 7.49315e-08, No Iterations 1
GAMG:  Solving for p, Initial residual = 7.71888e-05, Final residual = 3.25475e-13, No Iterations 1
GAMG:  Solving for p, Initial residual = 1.49854e-09, Final residual = 1.49854e-09, No Iterations 0
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0.00014808, global = -0.000129601, cumulative = -0.0697627
rho max/min : 2 0.5
GAMG:  Solving for p, Initial residual = 1.52653e-07, Final residual = 1.52653e-07, No Iterations 0
GAMG:  Solving for p, Initial residual = 1.52653e-07, Final residual = 1.52653e-07, No Iterations 0
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0.000148089, global = -0.000129601, cumulative = -0.0698923
rho max/min : 2 0.5
GAMG:  Solving for p, Initial residual = 1.52573e-07, Final residual = 1.52573e-07, No Iterations 0
GAMG:  Solving for p, Initial residual = 1.52573e-07, Final residual = 1.52573e-07, No Iterations 0
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0.000148089, global = -0.000129601, cumulative = -0.0700219
rho max/min : 2 0.5
smoothSolver:  Solving for omega, Initial residual = 2.31798e-06, Final residual = 1.30867e-10, No Iterations 1
bounding omega, min: -6301.47 max: 5.70133e+09 average: 2.17771e+06
smoothSolver:  Solving for k, Initial residual = 2.69839e-05, Final residual = 1.04992e-09, No Iterations 1
ExecutionTime = 62085.4 s  ClockTime = 83417 s

Courant Number mean: 0.000114789 max: 1
deltaT = 1.41799e-09
Time = 5.83257e-07

solidBodyMotionFunctions::rotatingMotion::transformation(): Time = 5.83257e-07 transformation: ((0 0 0) (0.999958 (0.00916165 0 0)))
AMI: Creating addressing and weights between 1900 source faces and 32076 target faces
AMI: Patch source sum(weights) min/max/average = 0.995459, 1, 0.999763
AMI: Patch target sum(weights) min/max/average = 0.468157, 1, 0.996805
AMI: Creating addressing and weights between 17748 source faces and 5456 target faces
AMI: Patch source sum(weights) min/max/average = 0.537877, 1.06201, 1.00015
AMI: Patch target sum(weights) min/max/average = 0.681757, 1.00303, 0.999863
AMI: Creating addressing and weights between 17839 source faces and 1957 target faces
AMI: Patch source sum(weights) min/max/average = 0.86998, 1, 0.999108
AMI: Patch target sum(weights) min/max/average = 0.991279, 1, 0.99992
GAMG:  Solving for pcorr, Initial residual = 1, Final residual = 0.00918253, No Iterations 49
GAMG:  Solving for pcorr, Initial residual = 0.0244148, Final residual = 0.00465114, No Iterations 1
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
rhoEqn max/min : 2.15666 0.1872
smoothSolver:  Solving for Ux, Initial residual = 3.25967e-05, Final residual = 2.1407e-09, No Iterations 1
smoothSolver:  Solving for Uy, Initial residual = 0.00157519, Final residual = 1.29333e-07, No Iterations 1
smoothSolver:  Solving for Uz, Initial residual = 0.00176436, Final residual = 1.35799e-07, No Iterations 1
smoothSolver:  Solving for h, Initial residual = 0.000915801, Final residual = 7.35108e-08, No Iterations 1
GAMG:  Solving for p, Initial residual = 7.69707e-05, Final residual = 3.22893e-13, No Iterations 1
GAMG:  Solving for p, Initial residual = 1.49221e-09, Final residual = 1.49221e-09, No Iterations 0
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0.000148538, global = -0.000130024, cumulative = -0.0701519
rho max/min : 2 0.5
GAMG:  Solving for p, Initial residual = 1.51827e-07, Final residual = 1.51827e-07, No Iterations 0
GAMG:  Solving for p, Initial residual = 1.51827e-07, Final residual = 1.51827e-07, No Iterations 0
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0.000148547, global = -0.000130024, cumulative = -0.0702819
rho max/min : 2 0.5
GAMG:  Solving for p, Initial residual = 1.51748e-07, Final residual = 1.51748e-07, No Iterations 0
GAMG:  Solving for p, Initial residual = 1.51748e-07, Final residual = 1.51748e-07, No Iterations 0
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0.000148547, global = -0.000130024, cumulative = -0.0704119
rho max/min : 2 0.5
smoothSolver:  Solving for omega, Initial residual = 2.31335e-06, Final residual = 1.3162e-10, No Iterations 1
bounding omega, min: -3196.96 max: 5.70337e+09 average: 2.17777e+06
smoothSolver:  Solving for k, Initial residual = 2.69244e-05, Final residual = 1.05185e-09, No Iterations 1
ExecutionTime = 62226.4 s  ClockTime = 83606 s

Courant Number mean: 0.000114768 max: 1
deltaT = 1.41798e-09
Time = 5.84675e-07

solidBodyMotionFunctions::rotatingMotion::transformation(): Time = 5.84675e-07 transformation: ((0 0 0) (0.999958 (0.00918393 0 0)))
AMI: Creating addressing and weights between 1900 source faces and 32076 target faces
AMI: Patch source sum(weights) min/max/average = 0.995457, 1, 0.999763
AMI: Patch target sum(weights) min/max/average = 0.468334, 1, 0.996805
AMI: Creating addressing and weights between 17748 source faces and 5456 target faces
AMI: Patch source sum(weights) min/max/average = 0.537262, 1.06316, 1.00015
AMI: Patch target sum(weights) min/max/average = 0.678559, 1.00301, 0.999883
AMI: Creating addressing and weights between 17839 source faces and 1957 target faces
AMI: Patch source sum(weights) min/max/average = 0.86998, 1, 0.999108
AMI: Patch target sum(weights) min/max/average = 0.991279, 1, 0.99992

Do i need to change solver for pressure and modify the tolerances. Please suggest

Tobi · November 7, 2014, 03:54

Hi,

my simulations are running on 40 cores 2 weeks ...
But you time step is very small and your density is wrong (I think)

Code:

rho max/min : 2 0.5

you make something wrong.
I dont know what because you do not share many details. You should check out you time steps... maybe your pressure, velocity, k, epsilon are expoding. As I can see, you should use the correct form of the PIMPLE algorithm. Maybe it will be stabilized. Checkout my blog or also available at the wiki.

November 6, 2014, 10:24		#16
RodriguezFatz Senior Member Philipp Join Date: Jun 2011 Location: Germany Posts: 1,297 Rep Power: 27	Whats the matter with your current results? Any problems? __________________ The skeleton ran out of shampoo in the shower.

November 7, 2014, 03:26		#18
Tobi Super Moderator Tobias Holzmann Join Date: Oct 2010 Location: Bad Wörishofen Posts: 2,711 Blog Entries: 6 Rep Power: 52	So at least there is no problem ... __________________ Keep foaming, Tobias Holzmann

November 7, 2014, 03:54		#20
Tobi Super Moderator Tobias Holzmann Join Date: Oct 2010 Location: Bad Wörishofen Posts: 2,711 Blog Entries: 6 Rep Power: 52	Hi, my simulations are running on 40 cores 2 weeks ... But you time step is very small and your density is wrong (I think) Code: rho max/min : 2 0.5 you make something wrong. I dont know what because you do not share many details. You should check out you time steps... maybe your pressure, velocity, k, epsilon are expoding. As I can see, you should use the correct form of the PIMPLE algorithm. Maybe it will be stabilized. Checkout my blog or also available at the wiki. __________________ Keep foaming, Tobias Holzmann

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Study of the EEqn.H in rhoPimpleDyMFoam.	Horacio Aguerre	OpenFOAM Programming & Development	11	August 19, 2022 03:47
Developing a rhoPimpleDyMFoam solver	bvieira	OpenFOAM Programming & Development	20	October 9, 2014 13:12
rhoPimpleDymFoam	jvd.mechanic	OpenFOAM Running, Solving & CFD	0	June 15, 2014 06:20
Divergence in rhoPimpleDyMFoam	bvieira	OpenFOAM Running, Solving & CFD	1	July 19, 2012 03:22

October 22, 2014, 07:35		#2
Jetfire Member Abhijit Join Date: Jul 2014 Posts: 75 Rep Power: 12	Coming to my simulation i have to simulate compressor stage of a turbocharger Meshing was done using ANSYS ICEM CFD , i had 3 mesh files 1. Inlet&Outlet 2.Volute 3.Rotor I imported them to openfoam using fluent3DMeshToFoam and then used mergeMeshes to make the complete domain, after that used splitMeshRegions -makeCellZones -overwrite to distinguish between the rotating zone and stationary zone. I am attaching few pictures of the domain so you could get a clear picture.Please have a look at them

October 22, 2014, 08:39		#4
vasava Senior Member Paritosh Vasava Join Date: Oct 2012 Location: Lappeenranta, Finland Posts: 732 Rep Power: 23	1. How are you merging your three meshes that you have imported from fluent? 2. How did you create AMI patches? 3. Do you have 'sets' folder (with several domains) inside the constant folder?

October 23, 2014, 06:50		#6
tomf Senior Member Tom Fahner Join Date: Mar 2009 Location: Breda, Netherlands Posts: 647 Rep Power: 32	Hi, Your problem seems to be in the turbulence model, I am guessing you have put epsilon equal to zero somewhere in either a boundary patch or the internalField. Change this to a sensible value for your case. Regards, Tom

October 23, 2014, 10:01		#7
vasava Senior Member Paritosh Vasava Join Date: Oct 2012 Location: Lappeenranta, Finland Posts: 732 Rep Power: 23	Your mesh setup seems alright. I agree with tomf, get some appropriate values for turbulence and use them in initial condition. Also can you post your boundary file here?

October 27, 2014, 05:16		#11
tomf Senior Member Tom Fahner Join Date: Mar 2009 Location: Breda, Netherlands Posts: 647 Rep Power: 32	You have provided a relative pressure of 0 Pa, you should put the absolute pressure. OpenFOAM does not use a "gauge pressure" or similar for compressible solvers. The solver now tried to solve for an absolute vacuum, which it could not do. I guess it only found out when density was required to calculated some part of the turbulence model. For incompressible cases 0 m2/s2 is allowed since in that case the absolute pressure does not matter. Regards, Tom Jetfire likes this.

October 27, 2014, 06:31		#14
Jetfire Member Abhijit Join Date: Jul 2014 Posts: 75 Rep Power: 12	@tomf, Thank you very much. Just changed my p-file as suggested by you, now my simulation started running!! I was always worried about the mut-file , dint expect the error was in my p-file. For now the simulation is running but too slow,have to run it in parallel and maybe some changes in my fvSchemes and fvSolution will do. il come back to you in case of any queries, thanks a lot!

November 7, 2014, 00:00		#17
Jetfire Member Abhijit Join Date: Jul 2014 Posts: 75 Rep Power: 12	Hi RodriguezFatz, I have started running the simulation and each timestep is taking a lot of time. Is there anything to do with my FvSolution or FvSchemes files to speed up my simulation? I am already running it on 8 cores.