interFoamとinterIsoFoamのインプットの違い

バージョン2306で確認した。

インプットファイルの比較

比較図は左がinterFoamで右がinterIsoFoamのチュートリアルケース。

0.orig/alpha.water

空白行の有り無しくらいの差でインプットに違いはない。

0.orig/p_rgh

0.orig/U

constant/dynamicMeshDict

interIsoFoamにはdynamicMeshDictがある。

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2306                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      dynamicMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dynamicFvMesh   staticFvMesh;


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

constant/g

細かい記述の違いはあるがキーワード数値に大きな違いはない。

constant/transportProperties

細かい記述の違いはあるがキーワード数値に大きな違いはない。

constant/turbulenceProperties

細かい記述の違いはあるがキーワード数値に大きな違いはない。

system/blockMeshDict

system/controlDict

system/decomposeParDict

違いなし。

system/fvSchemes

system/fvSolution

system/setFieldsDict

特に違いなし。

system/sampling

interFoamのチュートリアルにだけ存在。

それぞれのチュートリアルケースを入れ替えて実行

interFoamのチュートリアルケースをinterIsoFoamで実行

チュートリアル実行のためにAllrunを書き換え

#!/bin/sh
cd "${0%/*}" || exit                                # Run from this directory
. ${WM_PROJECT_DIR:?}/bin/tools/RunFunctions        # Tutorial run functions
#------------------------------------------------------------------------------

restore0Dir

runApplication blockMesh

runApplication setFields

runApplication interIsoFoam

#------------------------------------------------------------------------------

計算は実行できた。

Courant Number mean: 0.180077 max: 0.911563
Interface Courant Number mean: 0.0106017 max: 0.669282
deltaT = 0.0026925
Time = 1

PIMPLE: iteration 1
isoAdvection: After conservative bounding: min(alpha) = 0, max(alpha) = 1 + 8.49821e-08
Phase-1 volume fraction = 0.127565  Min(alpha.water) = 0  Max(alpha.water) = 1
DICPCG:  Solving for p_rgh, Initial residual = 0.0388851, Final residual = 0.00110888, No Iterations 2
time step continuity errors : sum local = 0.00122878, global = 4.39984e-07, cumulative = 0.00276999
DICPCG:  Solving for p_rgh, Initial residual = 0.00133789, Final residual = 5.10775e-05, No Iterations 19
time step continuity errors : sum local = 5.61667e-05, global = -1.21574e-05, cumulative = 0.00275783
DICPCG:  Solving for p_rgh, Initial residual = 0.000286543, Final residual = 7.53089e-08, No Iterations 59
time step continuity errors : sum local = 8.31681e-08, global = 3.88184e-09, cumulative = 0.00275783
ExecutionTime = 9.25 s  ClockTime = 26 s

End

log.interIsoFoamを確認。

fvSolution.solvers.alpha.water.*にreconstructionSchemeがないためデフォルトを使うとワーニング。

No finite volume options present
--> FOAM Warning : Entry 'reconstructionScheme' not found in dictionary "/mnt/c/Users/hamma/Documents/97thOpenCAE/damBreak_interFoam_OF2306_laminar/damBreak/system/fvSolution.solvers.alpha.water.*"
using default

そのほかもinterIsoFoamに関するワーニングが3つほど表示された。

PIMPLE: iteration 1
--> FOAM Warning :
From void Foam::cutFaceAdvect::cutPoints(Foam::label, Foam::scalar, Foam::DynamicList<Foam::Vector<double> >&)
in file cellCuts/cutFace/cutFaceAdvect.C at line 927
cutPoints = 4((0.457052 0.443619 0) (0.457052 0.456381 0) (0.457052 0.456381 0.0146) (0.457052 0.443619 0.0146)) for pts = 4((0.457052 0.443619 0) (0.457052 0.456381 0) (0.457052 0.456381 0.0146) (0.457052 0.443619 0.0146)), f - f0 = 4(3729 3748 4546 4527) and f0 = 9.59456e-08

実行結果（interFoamのチュートリアルをinterIsoFoamで実行）

interFoamのチュートリアルをinterFoamで実行

差は出ているのでinterIsoFoamの影響は出ていそう。

最後にinterIsoFoamの結果を示す。こちらはメッシュの分割数も違うのでより、界面がはっきりしている。

interIsoFoamのチュートリアル実行結果

interIsoFoamのチュートリアルケースをinterFoamで実行

Allrunを次のように修正

#!/bin/sh
cd "${0%/*}" || exit                                # Run from this directory
. ${WM_PROJECT_DIR:?}/bin/tools/RunFunctions        # Tutorial run functions
#------------------------------------------------------------------------------

restore0Dir

runApplication blockMesh

runApplication setFields

runApplication interFoam
foamSequenceVTKFiles -vtp
#------------------------------------------------------------------------------

interFoamの実行時にエラーが発生。

PIMPLE: iteration 1


--> FOAM FATAL IO ERROR: (openfoam-2306)
Entry 'nAlphaCorr' not found in dictionary "/mnt/c/Users/hamma/Documents/97thOpenCAE/damBreak_interIsoFoam_OF2306/system/fvSolution.solvers.alpha.water.*"


file: system/fvSolution.solvers.alpha.water.* at line 22 to 31.

    From bool Foam::dictionary::readEntry(const Foam::word&, T&, Foam::keyType::option, Foam::IOobjectOption::readOption) const [with T = int]
    in file ./src/OpenFOAM/lnInclude/dictionaryTemplates.C at line 327.

FOAM exiting

fvSolutionを見ると、nAlphaCorrは確かにない。

solvers
{
    "alpha.water.*"
    {
        isoFaceTol      1e-6;
        surfCellTol     1e-6;
        nAlphaBounds    3;
        snapTol         1e-12;
        clip            true;
        reconstructionScheme isoAlpha;
        writeFields     true;

        nAlphaSubCycles 1;
        cAlpha          1; // Note: cAlpha is not used by isoAdvector but must
                           // be specified because interfacePropertes object
                           // reads it during construction.
    }

interFoamのチュートリアルからnAlphaCorrをfvSolutionに移植。

"alpha.water.*"
    {
        isoFaceTol      1e-6;
        surfCellTol     1e-6;
        nAlphaBounds    3;
        snapTol         1e-12;
        clip            true;
        reconstructionScheme isoAlpha;
        writeFields     true;
        nAlphaCorr      2;

        nAlphaSubCycles 1;
        cAlpha          1; // Note: cAlpha is not used by isoAdvector but must
                           // be specified because interfacePropertes object
                           // reads it during construction.
    }

interFoam実行時にエラーが出る。

PIMPLE: iteration 1


--> FOAM FATAL IO ERROR: (openfoam-2306)
Entry 'div(phirb,alpha)' not found in dictionary "system/fvSchemes.divSchemes"


file: system/fvSchemes.divSchemes at line 30 to 31.

    From const Foam::entry& Foam::dictionary::lookupEntry(const Foam::word&, Foam::keyType::option) const
    in file db/dictionary/dictionary.C at line 375.

FOAM exiting

fvSchemesにinterFoamチュートリアルからdiv(phirb,alpha)を移植

divSchemes
{
    div(rhoPhi,U)    Gauss limitedLinearV 1;
    div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
    div(phirb,alpha) Gauss linear;
}

interFoamでエラー発生。

--> FOAM FATAL IO ERROR: (openfoam-2306)
Entry 'div(phi,alpha)' not found in dictionary "system/fvSchemes.divSchemes"


file: system/fvSchemes.divSchemes at line 30 to 32.

    From const Foam::entry& Foam::dictionary::lookupEntry(const Foam::word&, Foam::keyType::option) const
    in file db/dictionary/dictionary.C at line 375.

FOAM exiting

fvSchemesにdiv(phi,alpha)を追記。（interFoamのインプットから移植）

divSchemes
{
    div(rhoPhi,U)    Gauss limitedLinearV 1;
    div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
    div(phirb,alpha) Gauss linear;
    div(phi,alpha)  Gauss vanLeer;
}

interFoamは少し実行されるが途中でエラーになる。

Time = 0.02

PIMPLE: iteration 1
MULES: Solving for alpha.water
MULES: Solving for alpha.water
Phase-1 volume fraction = 0.124769  Min(alpha.water) = -4.34239e-18  Max(alpha.water) = 1
GAMG:  Solving for p_rgh, Initial residual = 0.0309471, Final residual = 0.000186698, No Iterations 1
time step continuity errors : sum local = 0.000781576, global = 6.37278e-07, cumulative = -1.57561e-06
GAMG:  Solving for p_rgh, Initial residual = 0.000196838, Final residual = 4.60438e-06, No Iterations 4
time step continuity errors : sum local = 1.88526e-05, global = 5.8965e-06, cumulative = 4.32089e-06
GAMG:  Solving for p_rgh, Initial residual = 9.95014e-06, Final residual = 5.28705e-10, No Iterations 12
time step continuity errors : sum local = 2.17348e-09, global = 2.07228e-09, cumulative = 4.32296e-06
ExecutionTime = 0.52 s  ClockTime = 1 s



--> FOAM FATAL ERROR: (openfoam-2306)

    failed lookup of reconstructionScheme (objectRegistry region0)
    available objects of type reconstructionSchemes:
0()


    From const Type& Foam::objectRegistry::lookupObject(const Foam::word&, bool) const [with Type = Foam::reconstructionSchemes]
    in file ./src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 571.

FOAM exiting

reconstructionScheme で何かが起きているので、fvSolutionでコメントアウト。

"alpha.water.*"
    {
        isoFaceTol      1e-6;
        surfCellTol     1e-6;
        nAlphaBounds    3;
        snapTol         1e-12;
        clip            true;
        //reconstructionScheme isoAlpha;
        writeFields     true;
        nAlphaCorr      2;

        nAlphaSubCycles 1;
        cAlpha          1; // Note: cAlpha is not used by isoAdvector but must
                           // be specified because interfacePropertes object
                           // reads it during construction.
    }

エラーメッセージは変わらなかった。

インプット比較で差があった部分を中心に再確認する。計算が走ってから途中で発散せずに落ちていることからcontrolDictのfunctionsを疑う。functionsの中をコメントアウトする。

functions
{
    // surfaces
    // {
    //     type            surfaces;
    //     libs            (geometricVoF sampling);
    //     writeControl    writeTime;

    //     surfaceFormat   vtp;
    //     fields          (p U);

    //     interpolationScheme cell;

    //     surfaces
    //     {
    //         freeSurf
    //         {
    //             type            interface;
    //             interpolate     false;
    //         }
    //     }
    // }
}

計算は進むようになったが、途中でエラー終了した。

Courant Number mean: 0.188855 max: 0.879953
Interface Courant Number mean: 0.0115789 max: 0.493851
deltaT = 0.000869565
Time = 0.265217

PIMPLE: iteration 1
MULES: Solving for alpha.water
MULES: Solving for alpha.water
Phase-1 volume fraction = 0.124769  Min(alpha.water) = -0.00189022  Max(alpha.water) = 1
GAMG:  Solving for p_rgh, Initial residual = 0.0772416, Final residual = 0.000910686, No Iterations 1
time step continuity errors : sum local = 0.000316055, global = -4.90856e-06, cumulative = 0.000170627
GAMG:  Solving for p_rgh, Initial residual = 0.00104247, Final residual = 2.25071e+134, No Iterations 1000
time step continuity errors : sum local = 7.82347e+133, global = -5.11591e+130, cumulative = -5.11591e+130
[stack trace]
=============
#1  Foam::sigFpe::sigHandler(int) in /usr/lib/openfoam/openfoam2306/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so
#2  ? in /lib/x86_64-linux-gnu/libc.so.6
#3  Foam::scalarProduct<double, double>::type Foam::sumProd<double>(Foam::UList<double> const&, Foam::UList<double> const&) in /usr/lib/openfoam/openfoam2306/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so
#4  Foam::PCG::scalarSolve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in /usr/lib/openfoam/openfoam2306/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so
#5  Foam::GAMGSolver::solveCoarsestLevel(Foam::Field<double>&, Foam::Field<double> const&) const in /usr/lib/openfoam/openfoam2306/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so
#6  Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in /usr/lib/openfoam/openfoam2306/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so
#7  Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in /usr/lib/openfoam/openfoam2306/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so
#8  Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) in /usr/lib/openfoam/openfoam2306/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so
#9  ? in /usr/lib/openfoam/openfoam2306/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so
#10  Foam::fvMesh::solve(Foam::fvMatrix<double>&, Foam::dictionary const&) const in /usr/lib/openfoam/openfoam2306/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so
#11  ? in /usr/lib/openfoam/openfoam2306/platforms/linux64GccDPInt32Opt/bin/interFoam
#12  ? in /lib/x86_64-linux-gnu/libc.so.6
#13  __libc_start_main in /lib/x86_64-linux-gnu/libc.so.6
#14  ? in /usr/lib/openfoam/openfoam2306/platforms/linux64GccDPInt32Opt/bin/interFoam
=============
Floating point exception

controlDictのfunctionsが原因だとわかったので、fvSolutionのreconstructionSchemeも元に戻す。

計算が落ちるタイミングは変わらなかった。

エラー前の出力結果

エラー前のステップのログを見ると、エラーが発生したのはp_rghの3回目の計算のところだとわかる。

Courant Number mean: 0.187632 max: 0.889183
Interface Courant Number mean: 0.011652 max: 0.496776
deltaT = 0.000869565
Time = 0.264348

PIMPLE: iteration 1
MULES: Solving for alpha.water
MULES: Solving for alpha.water
Phase-1 volume fraction = 0.124769  Min(alpha.water) = -0.00188413  Max(alpha.water) = 1
GAMG:  Solving for p_rgh, Initial residual = 0.0652241, Final residual = 0.000764112, No Iterations 1
time step continuity errors : sum local = 0.000244135, global = -6.56321e-06, cumulative = 0.000174323
GAMG:  Solving for p_rgh, Initial residual = 0.00085468, Final residual = 2.80426e-05, No Iterations 3
time step continuity errors : sum local = 9.07342e-06, global = 1.21197e-06, cumulative = 0.000175535
GAMG:  Solving for p_rgh, Initial residual = 0.000138136, Final residual = 8.80191e-10, No Iterations 15
time step continuity errors : sum local = 2.84353e-10, global = -7.01505e-11, cumulative = 0.000175535
ExecutionTime = 14.69 s  ClockTime = 22 s

Courant Number mean: 0.188855 max: 0.879953
Interface Courant Number mean: 0.0115789 max: 0.493851
deltaT = 0.000869565
Time = 0.265217

PIMPLE: iteration 1
MULES: Solving for alpha.water
MULES: Solving for alpha.water
Phase-1 volume fraction = 0.124769  Min(alpha.water) = -0.00189022  Max(alpha.water) = 1
GAMG:  Solving for p_rgh, Initial residual = 0.0772416, Final residual = 0.000910686, No Iterations 1
time step continuity errors : sum local = 0.000316055, global = -4.90856e-06, cumulative = 0.000170627
GAMG:  Solving for p_rgh, Initial residual = 0.00104247, Final residual = 2.25071e+134, No Iterations 1000
time step continuity errors : sum local = 7.82347e+133, global = -5.11591e+130, cumulative = -5.11591e+130
[stack trace]
=============
#1  Foam::sigFpe::sigHandler(int) in /usr/lib/openfoam/openfoam2306/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so

感覚的にfvSolutionが怪しい気がしたので、interFoamのチュートリアルにあるrelaxationFactorsを移植する。

PIMPLE
{
    momentumPredictor no;
    nCorrectors     3;
    nOuterCorrectors 1;
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;
}

relaxationFactors
{
    equations
    {
        ".*" 1;
    }
}

計算が実行できた。

interIsoFoamのチュートリアルをinterFoamで計算した結果

interIsoFoamのチュートリアル実行結果