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/)
-   -   Compressor Simulation using rhoPimpleDyMFoam (https://www.cfd-online.com/Forums/openfoam-solving/143340-compressor-simulation-using-rhopimpledymfoam.html)

Jetfire October 22, 2014 06:25

Compressor Simulation using rhoPimpleDyMFoam
 
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 06:35

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 06:38

1 Attachment(s)
This is the complete domain of my simulation

vasava October 22, 2014 07:39

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 03:36

@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 05:50

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 09:01

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 01:04

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 01:20

Quote:

Originally Posted by Jetfire (Post 516082)
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 01:30

1 Attachment(s)
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 04:16

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 05:02

Quote:

Originally Posted by tomf (Post 516109)
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 05:09

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 05:31

@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.:confused:


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 03:02

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 09:24

Whats the matter with your current results? Any problems?

Jetfire November 6, 2014 23:00

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 02:26

So at least there is no problem ...

Jetfire November 7, 2014 02:33

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 02:54

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.


All times are GMT -4. The time now is 07:21.