Find answers, ask questions, and connect with our <br>community around the world.

Home Forums OpenFOAM Forum Rotating Machines SST kOmega error

  • Rotating Machines SST kOmega error

    Posted by Adityan on June 12, 2022 at 1:11 pm

    Hi Everyone,
    I have done doing the kEpsilon Version of the Simulation
    But when I changed the Turbulence model to kOmega, it is showing error.
    mpirun -np 4 pimpleFoam -parallel | tee log.pimpleFoam
    ————————————————————————–
    WARNING: Linux kernel CMA support was requested via the
    btl_vader_single_copy_mechanism MCA variable, but CMA support is
    not available due to restrictive ptrace settings.

    The vader shared memory BTL will fall back on another single-copy
    mechanism if one is available. This may result in lower performance.

    Local host: DESKTOP-QJKQ6RU
    ————————————————————————–
    /*—————————————————————————*\
    | ========= | |
    | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
    | \\ / O peration | Version: 2112 |
    | \\ / A nd | Website: http://www.openfoam.com |
    | \\/ M anipulation | |
    \*—————————————————————————*/
    Build : _d44c8318-20220111 OPENFOAM=2112 version=2112
    Arch : “LSB;label=32;scalar=64”
    Exec : pimpleFoam -parallel
    Date : Jun 12 2022
    Time : 18:37:31
    Host : DESKTOP-QJKQ6RU
    PID : 1189
    I/O : uncollated
    Case : /home/adityan/OpenFOAM/adityan-v2112/run/propeller
    nProcs : 4
    Hosts :
    (
    (DESKTOP-QJKQ6RU 4)
    )
    Pstream initialized with:
    floatTransfer : 0
    nProcsSimpleSum : 0
    commsType : nonBlocking
    polling iterations : 0
    trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).
    fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)
    allowSystemOperations : Allowing user-supplied system call operations

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

    Create mesh for time = 0

    Selecting dynamicFvMesh dynamicMotionSolverFvMesh
    Selecting motion solver: solidBody
    Applying solid body motion to cellZone innerCylinderSmall
    Selecting solid-body motion function rotatingMotion
    Applying solid body motion to cellZone innerCylinderSmall

    PIMPLE: no residual control data found. Calculations will employ 2 corrector loops

    Reading field p

    Reading field U

    Reading/calculating face flux field phi

    AMI: Creating addressing and weights between 18496 source faces and 18720 target faces
    AMI: Patch source sum(weights) min:0.983877 max:1.01508 average:1.00007
    AMI: Patch target sum(weights) min:0.969379 max:1.00428 average:0.999988
    Selecting incompressible transport model Newtonian
    Selecting turbulence model type RAS
    Selecting RAS turbulence model kOmegaSST
    [0]
    [0]
    [0] –> FOAM FATAL IO ERROR: (openfoam—————————————————————————
    MPI_ABORT was invoked on rank 0 in communicator MPI_COMM_WORLD
    with errorcode 1.

    NOTE: invoking MPI_ABORT causes Open MPI to kill all MPI processes.
    You may or may not see output from other processes, depending on
    exactly when Open MPI kills them.
    ————————————————————————–
    2112)
    [0] Entry ‘method’ not found in dictionary “/home/adityan/OpenFOAM/adityan-v2112/run/propeller/system/fvSchemes.wallDist”
    [0]
    [0]
    [0] file: system/fvSchemes.wallDist
    [0]
    [0] From bool Foam::dictionary::readEntry(const Foam::word&, T&, Foam::keyType::option, bool) const [with T = Foam::word]
    [0] in file /usr/src/packages/BUILD/src/OpenFOAM/lnInclude/dictionaryTemplates.C at line 322.
    [0]
    FOAM parallel run exiting
    [0]
    [DESKTOP-QJKQ6RU:01184] 3 more processes have sent help message help-btl-vader.txt / cma-permission-denied
    [DESKTOP-QJKQ6RU:01184] Set MCA parameter “orte_base_help_aggregate” to 0 to see all help / error messages

    Barış Bicer replied 1 year, 9 months ago 2 Members · 9 Replies
  • 9 Replies
  • Barış Bicer

    Moderator
    June 12, 2022 at 2:33 pm

    Hi Adityan,

    Standard kOmega models are mainly used for near-wall treatment. (kOmega)-SST stands for shear stress transport. The SST formulation switches to a k−ϵ behavior in the free-stream, which avoids the k−ω problem of being sensitive to the inlet free-stream turbulence properties. However, it is used wallDistance treatment in the boundary layer.

    Therefore, you should define wallDist model in system/fvSchemes to let openfoam how to calculate it.

    Please add below lines end of fvSchemes file and then run again

    wallDist
    {
    method meshWave;
    }

    It will work.

    Best.

    Barış

  • Adityan

    Member
    June 14, 2022 at 5:14 pm

    Hi Baris,
    I have added the lines in the fvSchemes file.
    And that error got solved.
    But another error is still persisting. The omega file is missing.
    The error message looks like this
    ————————————————————————–
    WARNING: Linux kernel CMA support was requested via the
    btl_vader_single_copy_mechanism MCA variable, but CMA support is
    not available due to restrictive ptrace settings.

    The vader shared memory BTL will fall back on another single-copy
    mechanism if one is available. This may result in lower performance.

    Local host: DESKTOP-QJKQ6RU
    ————————————————————————–
    /*—————————————————————————*\
    | ========= | |
    | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
    | \\ / O peration | Version: 2112 |
    | \\ / A nd | Website: http://www.openfoam.com |
    | \\/ M anipulation | |
    \*—————————————————————————*/
    Build : _d44c8318-20220111 OPENFOAM=2112 version=2112
    Arch : “LSB;label=32;scalar=64”
    Exec : pimpleFoam -parallel
    Date : Jun 14 2022
    Time : 22:38:31
    Host : DESKTOP-QJKQ6RU
    PID : 574
    I/O : uncollated
    Case : /home/adityan/OpenFOAM/adityan-v2112/run/propeller
    nProcs : 4
    Hosts :
    (
    (DESKTOP-QJKQ6RU 4)
    )
    Pstream initialized with:
    floatTransfer : 0
    nProcsSimpleSum : 0
    commsType : nonBlocking
    polling iterations : 0
    trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).
    fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)
    allowSystemOperations : Allowing user-supplied system call operations

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

    Create mesh for time = 0

    Selecting dynamicFvMesh dynamicMotionSolverFvMesh
    Selecting motion solver: solidBody
    Applying solid body motion to cellZone innerCylinderSmall
    Selecting solid-body motion function rotatingMotion
    Applying solid body motion to cellZone innerCylinderSmall

    PIMPLE: no residual control data found. Calculations will employ 2 corrector loops

    Reading field p

    Reading field U

    Reading/calculating face flux field phi

    AMI: Creating addressing and weights between 18496 source faces and 18720 target faces
    AMI: Patch source sum(weights) min:0.983877 max:1.01508 average:1.00007
    AMI: Patch target sum(weights) min:0.969379 max:1.00428 average:0.999988
    Selecting incompressible transport model Newtonian
    Selecting turbulence model type RAS
    Selecting RAS turbulence model kOmegaSST
    Selecting patchDistMethod meshWave
    [0]
    [0]
    [0] –> FOAM FATAL ERROR: (openfoam-2112)
    [0] cannot find file “/home/adityan/OpenFOAM/adityan-v2112/run/propeller/processor0/0/omega”
    [0]
    [0] From virtual Foam::autoPtr<Foam::ISstream> Foam::fileOperations::uncollatedFileOperation::readStream(Foam::regIOobject&, const Foam::fileName&, const Foam::word&, bool) const
    [0] in file global/fileOperations/uncollatedFileOperation/uncollatedFileOperation.C at line 542.
    [0]
    FOAM parallel run exiting
    [0]
    [1]
    [1]
    [1] –> FOAM FATAL ERROR: (openfoam-2112)
    [1] cannot find file “/home/adityan/OpenFOAM/adityan-v2112/run/propeller/processor1/0/omega”
    [1]
    [1] From virtual Foam::autoPtr<Foam::ISstream> Foam::fileOperations::uncollatedFileOperation::readStream(Foam::regIOobject&, const Foam::fileName&, const Foam::word&, bool) const
    [1] in file global/fileOperations/uncollatedFileOperation/uncollatedFileOperation.C at line 542.
    [1]
    FOAM parallel run exiting
    [1]
    [3]
    [3]
    [3] –> FOAM FATAL ERROR: (openfoam-2112)
    [3] cannot find file “/home/adityan/OpenFOAM/adityan-v2112/run/propeller/processor3/0/omega”
    [3]
    [3] From virtual Foam::autoPtr<Foam::ISstream> Foam::fileOperations::uncollatedFileOperation::readStream(Foam::regIOobject&, const Foam::fileName&, const Foam::word&, bool) const
    [3] in file global/fileOperations/uncollatedFileOperation/uncollatedFileOperation.C at line 542.
    [3]
    FOAM parallel run exiting
    [3]
    [2]
    [2]
    [2] –> FOAM FATAL ERROR: (openfoam-2112)
    [2] cannot find file “/home/adityan/OpenFOAM/adityan-v2112/run/propeller/processor2/0/omega”
    [2]
    [2] From virtual Foam::autoPtr<Foam::ISstream> Foam::fileOperations::uncollatedFileOperation::readStream(Foam::regIOobject&, const Foam::fileName&, const Foam::word&, bool) const
    [2] in file global/fileOperations/uncollatedFileOperation/uncollatedFileOperation.C at line 542.
    [2]
    FOAM parallel run exiting
    [2]
    ————————————————————————–
    MPI_ABORT was invoked on rank 0 in communicator MPI_COMM_WORLD
    with errorcode 1.

    NOTE: invoking MPI_ABORT causes Open MPI to kill all MPI processes.
    You may or may not see output from other processes, depending on
    exactly when Open MPI kills them.
    ————————————————————————–
    [DESKTOP-QJKQ6RU:00569] 3 more processes have sent help message help-btl-vader.txt / cma-permission-denied
    [DESKTOP-QJKQ6RU:00569] Set MCA parameter “orte_base_help_aggregate” to 0 to see all help / error messages
    [DESKTOP-QJKQ6RU:00569] 3 more processes have sent help message help-mpi-api.txt / mpi-abort

  • Barış Bicer

    Moderator
    June 15, 2022 at 3:07 pm

    Hi Adityan,

    As you said that omega file is missing in 0/ folder. Please copy an omega file from a tutorial case and modify it according to your boundary names.

    for example : https://develop.openfoam.com/Development/openfoam/-/blob/master/tutorials/incompressible/pimpleFoam/RAS/rotatingFanInRoom/0.orig/omega

    for your info.

    Barış

  • Adityan

    Member
    June 15, 2022 at 5:24 pm

    Hi Baris,
    I defined the omega file as this
    /*——————————–*- C++ -*———————————-*\
    | ========= | |
    | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
    | \\ / O peration | Version: v2112 |
    | \\ / A nd | Website: http://www.openfoam.com |
    | \\/ M anipulation | |
    \*—————————————————————————*/
    FoamFile
    {
    version 2.0;
    format ascii;
    class volScalarField;
    object omega;
    }
    // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

    internalField uniform 0.1;

    boundaryField
    {
    outerCylinder
    {
    type omegaWallFunction;
    value uniform 0.1;
    }
    propellerTip
    {
    type omegaWallFunction;
    value nonuniform List<scalar> 0;
    }
    propellerStem1
    {
    type omegaWallFunction;
    value nonuniform List<scalar> 0;
    }
    propellerStem2
    {
    type omegaWallFunction;
    value nonuniform List<scalar> 0;
    }
    propellerStem3
    {
    type omegaWallFunction;
    value nonuniform List<scalar> 0;
    }
    AMI1
    {
    type cyclicAMI;
    value uniform 0.1;
    }

    AMI2
    {
    type cyclicAMI;
    value uniform 0.1;
    }
    inlet
    {
    type fixedValue;
    value nonuniform List<scalar> 0;
    }
    outlet
    {
    type inletOutlet;
    inletValue uniform 0.1;
    value uniform 0.1;
    }
    procBoundary0to1
    {
    type processor;
    value uniform 0.1;
    }
    }

    // ************************************************************************* //
    But I got this message while running decomposePar
    /*—————————————————————————*\
    | ========= | |
    | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
    | \\ / O peration | Version: 2112 |
    | \\ / A nd | Website: http://www.openfoam.com |
    | \\/ M anipulation | |
    \*—————————————————————————*/
    Build : _d44c8318-20220111 OPENFOAM=2112 version=2112
    Arch : “LSB;label=32;scalar=64”
    Exec : decomposePar
    Date : Jun 15 2022
    Time : 22:50:57
    Host : DESKTOP-QJKQ6RU
    PID : 589
    I/O : uncollated
    Case : /home/adityan/OpenFOAM/adityan-v2112/run/propeller
    nProcs : 1
    trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).
    fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)
    allowSystemOperations : Allowing user-supplied system call operations

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

    Decomposing mesh

    Create mesh

    Calculating distribution of cells
    Decomposition method hierarchical [4] (region region0)

    Finished decomposition in 0.17 s

    Calculating original mesh data

    Distributing cells to processors

    Distributing faces to processors

    Distributing points to processors

    Constructing processor meshes

    Processor 0
    Number of cells = 131518
    Number of faces shared with processor 1 = 2748
    Number of processor patches = 1
    Number of processor faces = 2748
    Number of boundary faces = 464

    Processor 1
    Number of cells = 131518
    Number of faces shared with processor 0 = 2748
    Number of faces shared with processor 2 = 6388
    Number of processor patches = 2
    Number of processor faces = 9136
    Number of boundary faces = 14503

    Processor 2
    Number of cells = 131518
    Number of faces shared with processor 1 = 6388
    Number of faces shared with processor 3 = 8860
    Number of processor patches = 2
    Number of processor faces = 15248
    Number of boundary faces = 22152

    Processor 3
    Number of cells = 131518
    Number of faces shared with processor 2 = 8860
    Number of processor patches = 1
    Number of processor faces = 8860
    Number of boundary faces = 25616

    Number of processor faces = 17996
    Max number of cells = 131518 (0% above average 131518)
    Max number of processor patches = 2 (33.3333% above average 1.5)
    Max number of faces between processors = 15248 (69.4599% above average 8998)

    Time = 0
    AMI: Creating addressing and weights between 18496 source faces and 18720 target faces
    AMI: Patch source sum(weights) min:0.983877 max:1.00392 average:1.00005
    AMI: Patch target sum(weights) min:0.969379 max:1.00428 average:0.99995

    –> FOAM FATAL IO ERROR: (openfoam-2112)
    Expected a ‘(‘ or a ‘{‘ while reading List, found on line 31: punctuation ‘;’

    file: 0/omega at line 31.

    From char Foam::Istream::readBeginList(const char*)
    in file db/IOstreams/IOstreams/Istream.C at line 155.

    FOAM exiting

  • Barış Bicer

    Moderator
    June 15, 2022 at 6:20 pm

    Hi again,

    What is the line of 31?

    there is a punctuation mistake there!

  • Adityan

    Member
    June 16, 2022 at 2:09 am

    Hi Baris,
    I checked line 31, the punctuation mistake specified is to either use ( or {.
    When I changed it to (scalar), it again showed error.
    So I tried to redefine my omega file, like this,
    \*—————————————————————————*/
    FoamFile
    {
    version 2.0;
    format ascii;
    class volScalarField;
    object omega;
    }
    // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

    internalField uniform 0.1;

    boundaryField
    {
    #includeEtc “caseDicts/setConstraintTypes”

    inlet
    {
    type fixedValue;
    value $internalField;
    }

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

    wall
    {
    type omegaWallFunction;
    value $internalField;
    }
    }

    // ************************************************************************* //
    Then I ran the decomposePar line, and It worked Fine.
    But when I tried to run the simulation,
    It is showing error in the fvSchemes.
    ————————————————————————–
    WARNING: Linux kernel CMA support was requested via the
    btl_vader_single_copy_mechanism MCA variable, but CMA support is
    not available due to restrictive ptrace settings.

    The vader shared memory BTL will fall back on another single-copy
    mechanism if one is available. This may result in lower performance.

    Local host: DESKTOP-QJKQ6RU
    ————————————————————————–
    /*—————————————————————————*\
    | ========= | |
    | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
    | \\ / O peration | Version: 2112 |
    | \\ / A nd | Website: http://www.openfoam.com |
    | \\/ M anipulation | |
    \*—————————————————————————*/
    Build : _d44c8318-20220111 OPENFOAM=2112 version=2112
    Arch : “LSB;label=32;scalar=64”
    Exec : pimpleFoam -parallel
    Date : Jun 16 2022
    Time : 07:33:17
    Host : DESKTOP-QJKQ6RU
    PID : 630
    I/O : uncollated
    Case : /home/adityan/OpenFOAM/adityan-v2112/run/propeller
    nProcs : 4
    Hosts :
    (
    (DESKTOP-QJKQ6RU 4)
    )
    Pstream initialized with:
    floatTransfer : 0
    nProcsSimpleSum : 0
    commsType : nonBlocking
    polling iterations : 0
    trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).
    fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)
    allowSystemOperations : Allowing user-supplied system call operations

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

    Create mesh for time = 0

    Selecting dynamicFvMesh dynamicMotionSolverFvMesh
    Selecting motion solver: solidBody
    Applying solid body motion to cellZone innerCylinderSmall
    Selecting solid-body motion function rotatingMotion
    Applying solid body motion to cellZone innerCylinderSmall

    PIMPLE: no residual control data found. Calculations will employ 2 corrector loops

    Reading field p

    Reading field U

    Reading/calculating face flux field phi

    AMI: Creating addressing and weights between 18496 source faces and 18720 target faces
    AMI: Patch source sum(weights) min:0.983877 max:1.01508 average:1.00007
    AMI: Patch target sum(weights) min:0.969379 max:1.00428 average:0.999988
    Selecting incompressible transport model Newtonian
    Selecting turbulence model type RAS
    Selecting RAS turbulence model kOmegaSST
    Selecting patchDistMethod meshWave
    RAS
    {
    RASModel kOmegaSST;
    turbulence on;
    printCoeffs on;
    alphaK1 0.85;
    alphaK2 1;
    alphaOmega1 0.5;
    alphaOmega2 0.856;
    gamma1 0.555556;
    gamma2 0.44;
    beta1 0.075;
    beta2 0.0828;
    betaStar 0.09;
    a1 0.31;
    b1 1;
    c1 10;
    F3 false;
    decayControl false;
    kInf 0;
    omegaInf 0;
    }

    No MRF models present

    No finite volume options present
    Constructing face velocity Uf

    Courant Number mean: 2.49647e-05 max: 0.0531646
    Sampled surface:
    zNormal -> vtk
    sampledCuttingPlane: zNormal : plane:(0 0 1) (0 0 0) offsets:(0)
    isoQ -> vtk
    isoSurface: isoQ : isoMethod:default regularise:full snap:1 field:Q value:(1000)
    propeller -> ensight
    sampledPatch: propeller : patches:(“propeller.*”)

    forces forces:
    rho: rhoInf
    Freestream density (rhoInf) set to 1
    Not including porosity effects

    propellerInfo propellerInfo1:
    rho: rhoInf
    Freestream density (rhoInf) set to 1.2
    Not including porosity effects

    Courant Number mean: 2.49647e-05 max: 0.0531646

    Starting time loop

    Courant Number mean: 2.49647e-05 max: 0.0531646
    deltaT = 1.20482e-05
    Time = 1.20482e-05

    PIMPLE: iteration 1
    AMI: Creating addressing and weights between 18496 source faces and 18720 target faces
    AMI: Patch source sum(weights) min:0.983867 max:1.01597 average:1.00007
    AMI: Patch target sum(weights) min:0.962468 max:1.00661 average:0.999987
    smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 0.0946845, No Iterations 10
    smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 0.00774885, No Iterations 1
    smoothSolver: Solving for Uz, Initial residual = 1, Final residual = 0.0946481, No Iterations 10
    [DESKTOP-QJKQ6RU:00625] 3 more processes have sent help message help-btl-vader.txt / cma-permission-denied
    [DESKTOP-QJKQ6RU:00625] Set MCA parameter “orte_base_help_aggregate” to 0 to see all help / error messages
    GAMG: Solving for p, Initial residual = 1, Final residual = 9.21078e-07, No Iterations 20
    time step continuity errors : sum local = 6.76076e-11, global = -2.03802e-11, cumulative = -2.03802e-11
    PIMPLE: iteration 2
    smoothSolver: Solving for Ux, Initial residual = 0.160935, Final residual = 9.21934e-07, No Iterations 42
    smoothSolver: Solving for Uy, Initial residual = 0.204695, Final residual = 8.66628e-07, No Iterations 38
    smoothSolver: Solving for Uz, Initial residual = 0.162391, Final residual = 9.35482e-07, No Iterations 42
    GAMG: Solving for p, Initial residual = 0.0869521, Final residual = 6.45077e-07, No Iterations 14
    time step continuity errors : sum local = 3.2649e-09, global = 1.0838e-09, cumulative = 1.06342e-09
    [0]
    [0]
    [0] –> FOAM FATAL IO ERROR: (openfoam-2112)
    ————————————————————————–
    MPI_ABORT was invoked on rank 0 in communicator MPI_COMM_WORLD
    with errorcode 1.

    NOTE: invoking MPI_ABORT causes Open MPI to kill all MPI processes.
    You may or may not see output from other processes, depending on
    exactly when Open MPI kills them.
    ————————————————————————–
    [0] Entry ‘div(phi,omega)’ not found in dictionary “system/fvSchemes.divSchemes”
    [0]
    [0]
    [0] file: system/fvSchemes.divSchemes at line 31 to 39.
    [0]
    [0] From const Foam::entry& Foam::dictionary::lookupEntry(const Foam::word&, Foam::keyType::option) const
    [0] in file db/dictionary/dictionary.C at line 375.
    [0]
    FOAM parallel run exiting
    [0]
    [2]
    [2]
    [2] –> FOAM FATAL IO ERROR: (openfoam-2112)
    [2] Entry ‘div(phi,omega)’ not found in dictionary “stream.divSchemes”
    [2]
    [2]
    [2] file: stream.divSchemes at line 0.
    [2]
    [2] From const Foam::entry& Foam::dictionary::lookupEntry(const Foam::word&, Foam::keyType::option) const
    [2] in file db/dictionary/dictionary.C at line 375.
    [2]
    FOAM parallel run exiting
    [2]
    [3]
    [3]
    [3] –> FOAM FATAL IO ERROR: (openfoam-2112)
    [3] Entry ‘div(phi,omega)’ not found in dictionary “stream.divSchemes”
    [3]
    [3]
    [3] file: stream.divSchemes at line 0.
    [3]
    [3] From const Foam::entry& Foam::dictionary::lookupEntry(const Foam::word&, Foam::keyType::option) const
    [3] in file db/dictionary/dictionary.C at line 375.
    [3]
    FOAM parallel run exiting
    [3]
    [1]
    [1]
    [1] –> FOAM FATAL IO ERROR: (openfoam-2112)
    [1] Entry ‘div(phi,omega)’ not found in dictionary “stream.divSchemes”
    [1]
    [1]
    [1] file: stream.divSchemes at line 0.
    [1]
    [1] From const Foam::entry& Foam::dictionary::lookupEntry(const Foam::word&, Foam::keyType::option) const
    [1] in file db/dictionary/dictionary.C at line 375.
    [1]
    FOAM parallel run exiting
    [1]
    [DESKTOP-QJKQ6RU:00625] 3 more processes have sent help message help-mpi-api.txt / mpi-abort
    So I replaced the epsilon with omega in the fvSchemes.
    But after again running the simulation, It is showing an error again.
    ————————————————————————–
    WARNING: Linux kernel CMA support was requested via the
    btl_vader_single_copy_mechanism MCA variable, but CMA support is
    not available due to restrictive ptrace settings.

    The vader shared memory BTL will fall back on another single-copy
    mechanism if one is available. This may result in lower performance.

    Local host: DESKTOP-QJKQ6RU
    ————————————————————————–
    /*—————————————————————————*\
    | ========= | |
    | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
    | \\ / O peration | Version: 2112 |
    | \\ / A nd | Website: http://www.openfoam.com |
    | \\/ M anipulation | |
    \*—————————————————————————*/
    Build : _d44c8318-20220111 OPENFOAM=2112 version=2112
    Arch : “LSB;label=32;scalar=64”
    Exec : pimpleFoam -parallel
    Date : Jun 16 2022
    Time : 07:36:46
    Host : DESKTOP-QJKQ6RU
    PID : 656
    I/O : uncollated
    Case : /home/adityan/OpenFOAM/adityan-v2112/run/propeller
    nProcs : 4
    Hosts :
    (
    (DESKTOP-QJKQ6RU 4)
    )
    Pstream initialized with:
    floatTransfer : 0
    nProcsSimpleSum : 0
    commsType : nonBlocking
    polling iterations : 0
    trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).
    fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)
    allowSystemOperations : Allowing user-supplied system call operations

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

    Create mesh for time = 0

    Selecting dynamicFvMesh dynamicMotionSolverFvMesh
    Selecting motion solver: solidBody
    Applying solid body motion to cellZone innerCylinderSmall
    Selecting solid-body motion function rotatingMotion
    Applying solid body motion to cellZone innerCylinderSmall

    PIMPLE: no residual control data found. Calculations will employ 2 corrector loops

    Reading field p

    Reading field U

    Reading/calculating face flux field phi

    AMI: Creating addressing and weights between 18496 source faces and 18720 target faces
    AMI: Patch source sum(weights) min:0.983877 max:1.01508 average:1.00007
    AMI: Patch target sum(weights) min:0.969379 max:1.00428 average:0.999988
    Selecting incompressible transport model Newtonian
    Selecting turbulence model type RAS
    Selecting RAS turbulence model kOmegaSST
    Selecting patchDistMethod meshWave
    RAS
    {
    RASModel kOmegaSST;
    turbulence on;
    printCoeffs on;
    alphaK1 0.85;
    alphaK2 1;
    alphaOmega1 0.5;
    alphaOmega2 0.856;
    gamma1 0.555556;
    gamma2 0.44;
    beta1 0.075;
    beta2 0.0828;
    betaStar 0.09;
    a1 0.31;
    b1 1;
    c1 10;
    F3 false;
    decayControl false;
    kInf 0;
    omegaInf 0;
    }

    No MRF models present

    No finite volume options present
    Constructing face velocity Uf

    Courant Number mean: 2.49647e-05 max: 0.0531646
    Sampled surface:
    zNormal -> vtk
    sampledCuttingPlane: zNormal : plane:(0 0 1) (0 0 0) offsets:(0)
    isoQ -> vtk
    isoSurface: isoQ : isoMethod:default regularise:full snap:1 field:Q value:(1000)
    propeller -> ensight
    sampledPatch: propeller : patches:(“propeller.*”)

    forces forces:
    rho: rhoInf
    Freestream density (rhoInf) set to 1
    Not including porosity effects

    propellerInfo propellerInfo1:
    rho: rhoInf
    Freestream density (rhoInf) set to 1.2
    Not including porosity effects

    Courant Number mean: 2.49647e-05 max: 0.0531646

    Starting time loop

    Courant Number mean: 2.49647e-05 max: 0.0531646
    deltaT = 1.20482e-05
    Time = 1.20482e-05

    PIMPLE: iteration 1
    AMI: Creating addressing and weights between 18496 source faces and 18720 target faces
    AMI: Patch source sum(weights) min:0.983867 max:1.01597 average:1.00007
    AMI: Patch target sum(weights) min:0.962468 max:1.00661 average:0.999987
    smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 0.0946845, No Iterations 10
    smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 0.00774885, No Iterations 1
    [DESKTOP-QJKQ6RU:00651] 3 more processes have sent help message help-btl-vader.txt / cma-permission-denied
    [DESKTOP-QJKQ6RU:00651] Set MCA parameter “orte_base_help_aggregate” to 0 to see all help / error messages
    smoothSolver: Solving for Uz, Initial residual = 1, Final residual = 0.0946481, No Iterations 10
    GAMG: Solving for p, Initial residual = 1, Final residual = 9.21078e-07, No Iterations 20
    time step continuity errors : sum local = 6.76076e-11, global = -2.03802e-11, cumulative = -2.03802e-11
    PIMPLE: iteration 2
    smoothSolver: Solving for Ux, Initial residual = 0.160935, Final residual = 9.21934e-07, No Iterations 42
    smoothSolver: Solving for Uy, Initial residual = 0.204695, Final residual = 8.66628e-07, No Iterations 38
    smoothSolver: Solving for Uz, Initial residual = 0.162391, Final residual = 9.35482e-07, No Iterations 42
    GAMG: Solving for p, Initial residual = 0.0869521, Final residual = 6.45077e-07, No Iterations 14
    time step continuity errors : sum local = 3.2649e-09, global = 1.0838e-09, cumulative = 1.06342e-09
    [0]
    [0]
    [0] –> FOAM FATAL IO ERROR: (openfoam—————————————————————————
    MPI_ABORT was invoked on rank 0 in communicator MPI_COMM_WORLD
    with errorcode 1.

    NOTE: invoking MPI_ABORT causes Open MPI to kill all MPI processes.
    You may or may not see output from other processes, depending on
    exactly when Open MPI kills them.
    ————————————————————————–
    2112)
    [0] Entry ‘omegaFinal’ not found in dictionary “system/fvSolution.solvers”
    [0]
    [0]
    [0] file: system/fvSolution.solvers at line 21 to 56.
    [0]
    [0] From const Foam::dictionary& Foam::dictionary::subDict(const Foam::word&, Foam::keyType::option) const
    [0] in file db/dictionary/dictionary.C at line 469.
    [0]
    FOAM parallel run exiting
    [0]
    [1]
    [1]
    [1] –> FOAM FATAL IO ERROR: (openfoam-2112)
    [1] Entry ‘omegaFinal’ not found in dictionary “stream.solvers”
    [1]
    [1]
    [1] file: stream.solvers at line 0.
    [1]
    [1] From const Foam::dictionary& Foam::dictionary::subDict(const Foam::word&, Foam::keyType::option) const
    [1] in file db/dictionary/dictionary.C at line 469.
    [1]
    FOAM parallel run exiting
    [1]
    [DESKTOP-QJKQ6RU:00651] PMIX ERROR: UNREACHABLE in file ../../../src/server/pmix_server.c at line 2193
    [DESKTOP-QJKQ6RU:00651] PMIX ERROR: UNREACHABLE in file ../../../src/server/pmix_server.c at line 2193
    [2]
    [2]
    [2] –> FOAM FATAL IO ERROR: (openfoam-2112)
    [2] Entry ‘omegaFinal’ not found in dictionary “stream.solvers”
    [2]
    [2]
    [2] file: stream.solvers at line 0.
    [2]
    [2] From const Foam::dictionary& Foam::dictionary::subDict(const Foam::word&, Foam::keyType::option) const
    [2] in file db/dictionary/dictionary.C at line 469.
    [2]
    FOAM parallel run exiting
    [2]
    [3]
    [3]
    [3] –> FOAM FATAL IO ERROR: (openfoam-2112)
    [3] Entry ‘omegaFinal’ not found in dictionary “stream.solvers”
    [3]
    [3]
    [3] file: stream.solvers at line 0.
    [3]
    [3] From const Foam::dictionary& Foam::dictionary::subDict(const Foam::word&, Foam::keyType::option) const
    [3] in file db/dictionary/dictionary.C at line 469.
    [3]
    FOAM parallel run exiting
    [3]
    [DESKTOP-QJKQ6RU:00651] 3 more processes have sent help message help-mpi-api.txt / mpi-abort
    What all parameters should we need to change here?

  • Barış Bicer

    Moderator
    June 16, 2022 at 7:56 am

    Hi Adityan,

    Good improvement.

    we should think carefully in OpenFOAM. We said to OpenFOAM so far that we would like to use komegaSST model. then specified missing Omega file in /0 folder. But we didnt say to OpenFOAM that how omega equation will be discretised?

    therefore please add below line in the fvScehemes files of divSchemes section

    div(phi,omega) Gauss linearUpwind grad(U);

    and then you should also tell OpenFOAM how the omega matrix will be solved.

    therefore you should also add below lines inside fvSolution file under the solver section,

    “(U|k|omega)”
    {
    solver smoothSolver;
    smoother symGaussSeidel;
    tolerance 1e-06;
    relTol 0.1;
    }

    “(U|k|omega)Final”
    {
    $U;
    tolerance 1e-06;
    relTol 0;
    }
    I hope that it clarifies your questions

    Best.

    Barış

  • Adityan

    Member
    June 22, 2022 at 5:34 pm

    Hi Baris,
    It worked, I am able to finally get the results, in kOmega model,
    Thanks alot,
    Regards

  • Barış Bicer

    Moderator
    June 23, 2022 at 3:33 pm

    great news Adityan!

    Congratulations!

Log in to reply.

error: Content is protected !!