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/)
-   -   simulating flow over naca0012 using LES (WALE subgrid model) (https://www.cfd-online.com/Forums/openfoam-solving/221224-simulating-flow-over-naca0012-using-les-wale-subgrid-model.html)

zeinelserfy October 9, 2019 07:00
simulating flow over naca0012 using LES (WALE subgrid model)
 
I am trying to run les simulation for flow over Naca0012 using WALE subgrid model.I first created the 3-D domain and run the case for steady state case using simpleFoam and then i used the converged solution as initial solution for the les by renaming the folder (6000 to 1e-5) then i decomposed the domain. I am using pimpleFoam for les simulation but the problem is that the simulation is not converging and the pressure equation solver reach the maximum no fo iteration (1000)without reaching a converged solution.

Is there any examples or have anyone worked on les for aerofoil ?

This the RANS results which is set as initial value for les
the velocity fields
https://www.simscale.com/forum/uploa...0ca7bb93a4.png
pressure fields
https://www.simscale.com/forum/uploa...c842bfbeb8.png
after running les simulation for few time step results seems to be not converged
the velocity field
https://www.simscale.com/forum/uploa...a082e3dd32.png
pressure field
https://www.simscale.com/forum/uploa...edba997015.png


boundary conditions
U
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  5.x                                  |
|  \\  /    A nd          | Web:      www.OpenFOAM.org                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version    2.0;
    format      ascii;
    class      volVectorField;
    location    "0";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField  uniform (71.3 0 0);

boundaryField
{
    aerofoil
    {
        type            fixedValue;
        value          uniform (0 0 0);
    }
    top
    {
        type            symmetryPlane;
    }
    bottom
    {
        type            symmetryPlane;
    }
    inlet
    {
        type            fixedValue;
        value          uniform (71.3 0 0);
    }
    outlet
    {
    {
        type            freestream;
        freestreamValue uniform (71.3 0 0);
        value          uniform (71.3 0 0);
    }
    }
    front
    {
        type            cyclic;
    }
    back
    {
        type            cyclic;
    }
}


// ************************************************************************* //
p
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  5.x                                  |
|  \\  /    A nd          | Web:      www.OpenFOAM.org                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version    2.0;
    format      ascii;
    class      volScalarField;
    location    "0";
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -2 0 0 0 0];

internalField  uniform 0;

boundaryField
{
    aerofoil
    {
        type            zeroGradient;
    }
    top
    {
        type            symmetryPlane;
    }
    bottom
    {
        type            symmetryPlane;
    }
    inlet
    {
        type            zeroGradient;
    }
    outlet
    {
        type            fixedValue;
        value          uniform 0;
    }
    front
    {
        type            cyclic;
    }
    back
    {
        type            cyclic;
    }
}


// ************************************************************************* //
nut
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  5.x                                  |
|  \\  /    A nd          | Web:      www.OpenFOAM.org                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version    2.0;
    format      ascii;
    class      volScalarField;
    location    "0";
    object      nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -1 0 0 0 0];

internalField  uniform 0.3;

boundaryField
{
    aerofoil
    {
        type            zeroGradient;
    }
    top
    {
        type            symmetryPlane;
    }
    bottom
    {
        type            symmetryPlane;
    }
    inlet
    {
        type            calculated;
        value          uniform 0.3;
    }
    outlet
    {
        type            calculated;
        value          uniform 0.3;
    }
    front
    {
        type            cyclic;
    }
    back
    {
        type            cyclic;
    }
}


// ************************************************************************* //
turbulence properties
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  2.2.0                                |
|  \\  /    A nd          | Web:      www.OpenFOAM.org                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version    2.0;
    format      ascii;
    class      dictionary;
    location    "constant";
    object      turbulenceProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

simulationType LES;

LES
{
LESModel        WALE;
turbulence      on;
printCoeffs    on;

delta          vanDriest;


vanDriestCoeffs
{
    delta          cubeRootVol;
    cubeRootVolCoeffs
    {
        deltaCoeff      1;
    }

    Aplus          26;
    Cdelta          0.158;
}
}
// ************************************************************************* //
the log files for the solver
Code:
PIMPLE: iteration 1
smoothSolver:  Solving for Ux, Initial residual = 9.57422e-05, Final residual = 1.81812e-09, No Iterations 1
smoothSolver:  Solving for Uy, Initial residual = 0.000310804, Final residual = 9.27005e-09, No Iterations 1
smoothSolver:  Solving for Uz, Initial residual = 0.00020072, Final residual = 8.29752e-07, No Iterations 1
Setting residual field for first solver iteration for solver field: p
GAMG:  Solving for p, Initial residual = 0.00708105, Final residual = 0.000695998, No Iterations 9
time step continuity errors : sum local = 6.92239e-12, global = -2.6458e-13, cumulative = -1.06871e-07
GAMG:  Solving for p, Initial residual = 0.000863465, Final residual = 0.000201283, No Iterations 1000
time step continuity errors : sum local = 1.99187e-12, global = -5.66889e-14, cumulative = -1.06871e-07
ExecutionTime = 5589.05 s  ClockTime = 11577 s

yPlus yPlus write:
    writing field yPlus
    patch aerofoil y+ : min = 0.00605518, max = 2.25921, average = 0.535984
wallShearStress wallShear write:
    writing field wallShearStress
    min/max(aerofoil) = (-1069.08 -49.9867 -4.19134), (647.826 514.472 4.15718)
    functionObjects::vorticity vorticity1 writing field: vorticity
forceCoeffs forceCoeffs1 execute:
    Coefficients
        Cd      : 0.0738408        (pressure: 0.0689114        viscous: 0.00492941)
        Cs      : 6.77456e-10        (pressure: -1.25113e-18        viscous: 6.77456e-10)
        Cl      : 3.00569        (pressure: 3.01024        viscous: -0.00454994)
        CmRoll      : -0.150284        (pressure: -0.150512        viscous: 0.000227497)
        CmPitch      : 0.933706        (pressure: 0.936566        viscous: -0.00286007)
        CmYaw      : 0.00369203        (pressure: 0.00344556        viscous: 0.000246471)
        Cd(f)    : -0.113364
        Cd(r)    : 0.187205
        Cs(f)    : 0.00369203
        Cs(r)    : -0.00369203
        Cl(f)    : 2.43655
        Cl(r)    : 0.569138
Courant Number mean: 0.000346019 max: 0.893467
deltaT = 7.73047e-08
Time = 8.04068e-06

PIMPLE: iteration 1
smoothSolver:  Solving for Ux, Initial residual = 9.46517e-05, Final residual = 1.82501e-09, No Iterations 1
smoothSolver:  Solving for Uy, Initial residual = 0.000308434, Final residual = 9.37502e-09, No Iterations 1
smoothSolver:  Solving for Uz, Initial residual = 0.000199936, Final residual = 8.34842e-07, No Iterations 1
Setting residual field for first solver iteration for solver field: p
GAMG:  Solving for p, Initial residual = 0.00703103, Final residual = 0.000696314, No Iterations 7
time step continuity errors : sum local = 6.93153e-12, global = -2.75319e-13, cumulative = -1.06872e-07
GAMG:  Solving for p, Initial residual = 0.000853688, Final residual = 0.000198625, No Iterations 1000
time step continuity errors : sum local = 1.96743e-12, global = -5.63175e-14, cumulative = -1.06872e-07
ExecutionTime = 5621.8 s  ClockTime = 11643 s

yPlus yPlus write:
    writing field yPlus
    patch aerofoil y+ : min = 0.00981989, max = 2.25001, average = 0.53326
wallShearStress wallShear write:
    writing field wallShearStress
    min/max(aerofoil) = (-1060.39 -50.7689 -4.17043), (639.549 509.112 4.1795)
    functionObjects::vorticity vorticity1 writing field: vorticity
forceCoeffs forceCoeffs1 execute:
    Coefficients
        Cd      : 0.0722708        (pressure: 0.0673676        viscous: 0.00490315)
        Cs      : 6.55462e-10        (pressure: -1.22961e-18        viscous: 6.55462e-10)
        Cl      : 2.94238        (pressure: 2.94688        viscous: -0.00450319)
        CmRoll      : -0.147119        (pressure: -0.147344        viscous: 0.00022516)
        CmPitch      : 0.913849        (pressure: 0.91668        viscous: -0.00283127)
        CmYaw      : 0.00361352        (pressure: 0.00336837        viscous: 0.000245157)
        Cd(f)    : -0.110984
        Cd(r)    : 0.183254
        Cs(f)    : 0.00361352
        Cs(r)    : -0.00361352
        Cl(f)    : 2.38504
        Cl(r)    : 0.557341
Courant Number mean: 0.000348545 max: 0.893368
deltaT = 7.78785e-08
Time = 8.11856e-06

PIMPLE: iteration 1
smoothSolver:  Solving for Ux, Initial residual = 9.35858e-05, Final residual = 1.83204e-09, No Iterations 1
smoothSolver:  Solving for Uy, Initial residual = 0.000306084, Final residual = 9.47784e-09, No Iterations 1
smoothSolver:  Solving for Uz, Initial residual = 0.000198762, Final residual = 8.40133e-07, No Iterations 1
Setting residual field for first solver iteration for solver field: p
GAMG:  Solving for p, Initial residual = 0.00700483, Final residual = 0.000694214, No Iterations 7
time step continuity errors : sum local = 6.92003e-12, global = -2.74424e-13, cumulative = -1.06872e-07

Lookid October 9, 2019 08:01
Hello,

some comments that I hope will help:

1) Use delta cubeRootVol for WALE, no need for vanDriest damping (https://caefn.com/openfoam/wale-sgs-model)
2) Try using PIMPLE as PIMPLE, not PISO, it will definitely help the pressure converge. i.e. put a lot of nOuterCorrectors + Residual goal. You will go to the next timestep once the specified residual is attained. Below is what I used for a LES simulation. You should have quite a lot of loops at first, but it should reduce a lot once it's stable. After 5 pimple loop it converges for my case. But I am not an expert at all, it is my first case.

Code:
PIMPLE
{
    nOuterCorrectors 50;
    nCorrectors    2;
    nNonOrthogonalCorrectors 2;
    pRefCell        0;
    pRefValue      0;

    outerCorrectorResidualControl //(or residualControl, depends on the version of OF)
    {
        p { tolerance 1e-4; relTol 0;} // I was said 1e-4 is enough
        U { tolerance 1e-5; relTol 0;}
    }

}
3) in fvSchemes, something that helped me a bit is using 'filteredLinear2 0.3 0' for scalars and 'filteredLinear2V 0.3 0' for U. You introduced a bit of upwind to stabilize some potential sh**, while keeping a central difference behaviour.

Please keep an update of how it is going :)

Santiago October 9, 2019 09:21
Quote:
Originally Posted by Lookid (Post 746578)
Hello,

some comments that I hope will help:

1) Use delta cubeRootVol for WALE, no need for vanDriest damping (https://caefn.com/openfoam/wale-sgs-model)
2) Try using PIMPLE as PIMPLE, not PISO, it will definitely help the pressure converge. i.e. put a lot of nOuterCorrectors + Residual goal. You will go to the next timestep once the specified residual is attained. Below is what I used for a LES simulation. You should have quite a lot of loops at first, but it should reduce a lot once it's stable. After 5 pimple loop it converges for my case. But I am not an expert at all, it is my first case.

Code:
PIMPLE
{
    nOuterCorrectors 50;
    nCorrectors    2;
    nNonOrthogonalCorrectors 2;
    pRefCell        0;
    pRefValue      0;

    outerCorrectorResidualControl //(or residualControl, depends on the version of OF)
    {
        p { tolerance 1e-4; relTol 0;} // I was said 1e-4 is enough
        U { tolerance 1e-5; relTol 0;}
    }

}
3) in fvSchemes, something that helped me a bit is using 'filteredLinear2 0.3 0' for scalars and 'filteredLinear2V 0.3 0' for U. You introduced a bit of upwind to stabilize some potential sh**, while keeping a central difference behaviour.

Please keep an update of how it is going :)
Unless your grid is pretty much garbage you don't need such "over-relaxation" of the solution. 50 outer iterations it's too much, specially if you're running big cases (50 times the solution of the pressure equation? Good luck with that). Besides, a naca profile is a very simple case, and one should be able to build a grid with optimum quality.

One thing: A proper LES (explicit) must avoid low-order upwinding, if you want your model to be accountable for most of the residual dissipation. Otherwise you are just doing "part explicit part implicit" LES which, when mixed, mean absolutely nothing.

Lookid October 9, 2019 09:34
Thank you for the clarifications :D

Quote:
Originally Posted by Santiago (Post 746593)
50 outer iterations it's too much
It is an arbitrary number never reached, I could have 10000 there. The point is to have the residual converged, and it never takes long as said. That being said, is it still a bad thing to do? Or LES should always be PISO?

Quote:
Originally Posted by Santiago (Post 746593)
A proper LES (explicit) must avoid low-order upwinding
I used the filteredLinear thingy because I had this wavy pattern (https://www.cfd-online.com/Forums/op...tml#post383679). As I understood it's appears if too coarse mesh and it shouldnt appear when Pe<2, not sure though. Otherwise yes, Gauss linear if this problem isn't here.

zeinelserfy October 9, 2019 09:40
Thanks for you reply Lilian Chabannes

I will try your recommendations

Can you check fvSchemes and fvSolutions?
fvSchemes
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  2.2.0                                |
|  \\  /    A nd          | Web:      www.OpenFOAM.org                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version    2.0;
    format      ascii;
    class      dictionary;
    location    "system";
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default        backward;
}

gradSchemes
{
    default        Gauss linear;
    grad(p)        Gauss linear;
    grad(U)        Gauss linear;
}

divSchemes
{
    default        none;
    div(phi,U)      Gauss linear;
    div(phi,k)      Gauss limitedLinear 1;
    div(phi,B)      Gauss limitedLinear 1;
    div(B)          Gauss linear;
    div(phi,nuTilda) Gauss limitedLinear 1;
    div((nuEff*dev2(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
    default        none;
    laplacian(nuEff,U) Gauss linear corrected;
    laplacian((1|A(U)),p) Gauss linear corrected;
    laplacian(DkEff,k) Gauss linear corrected;
    laplacian(DBEff,B) Gauss linear corrected;
    laplacian(DnuTildaEff,nuTilda) Gauss linear corrected;
}

interpolationSchemes
{
    default        linear;
    interpolate(U)  linear;
}

snGradSchemes
{
    default        corrected;
}

fluxRequired
{
    default        no;
    p              ;
}


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





fvSolutons
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  v1906                                |
|  \\  /    A nd          | Web:      www.OpenFOAM.com                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version    2.0;
    format      ascii;
    class      dictionary;
    location    "system";
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    p
    {
        solver          GAMG;
        tolerance      0;
        relTol          0.1;
        smoother        GaussSeidel;
    }

    pFinal
    {
        $p;
        smoother        DICGaussSeidel;
        tolerance      1e-06;
        relTol          0;
    }

    "(U|k|nuTilda)"
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance      1e-05;
        relTol          0.1;
        minIter        1;
    }

    "(U|k|nuTilda)Final"
    {
        $U;
        tolerance      1e-05;
        relTol          0;
    }
}

PIMPLE
{
    nOuterCorrectors 1;
    nCorrectors    2;
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue      0;
}


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

zeinelserfy October 9, 2019 19:40
Quote:
Originally Posted by Santiago (Post 746593)
Unless your grid is pretty much garbage you don't need such "over-relaxation" of the solution. 50 outer iterations it's too much, specially if you're running big cases (50 times the solution of the pressure equation? Good luck with that). Besides, a naca profile is a very simple case, and one should be able to build a grid with optimum quality.
you mean that if the number of outer iterations is high this means that there is a problem with the mesh or it needs to be refined ??
Quote:
Originally Posted by Santiago (Post 746593)
One thing: A proper LES (explicit) must avoid low-order upwinding, if you want your model to be accountable for most of the residual dissipation. Otherwise you are just doing "part explicit part implicit" LES which, when mixed, mean absolutely nothing.
which scheme should be used with les?

zeinelserfy October 9, 2019 21:12
Quote:
Originally Posted by Lookid (Post 746578)
Hello,

some comments that I hope will help:

1) Use delta cubeRootVol for WALE, no need for vanDriest damping (https://caefn.com/openfoam/wale-sgs-model)
2) Try using PIMPLE as PIMPLE, not PISO, it will definitely help the pressure converge. i.e. put a lot of nOuterCorrectors + Residual goal. You will go to the next timestep once the specified residual is attained. Below is what I used for a LES simulation. You should have quite a lot of loops at first, but it should reduce a lot once it's stable. After 5 pimple loop it converges for my case. But I am not an expert at all, it is my first case.

Code:
PIMPLE
{
    nOuterCorrectors 50;
    nCorrectors    2;
    nNonOrthogonalCorrectors 2;
    pRefCell        0;
    pRefValue      0;

    outerCorrectorResidualControl //(or residualControl, depends on the version of OF)
    {
        p { tolerance 1e-4; relTol 0;} // I was said 1e-4 is enough
        U { tolerance 1e-5; relTol 0;}
    }

}
3) in fvSchemes, something that helped me a bit is using 'filteredLinear2 0.3 0' for scalars and 'filteredLinear2V 0.3 0' for U. You introduced a bit of upwind to stabilize some potential sh**, while keeping a central difference behaviour.

Please keep an update of how it is going :)
I have set residual control for the outeriterations but after 1 time step
the solver crashed
Code:
zels496@en-cer00228:/data/cases/LES/naca0012-4initiaRANS/case1$ mpirun -np 16 pimpleFoam -parallel >log
[en-cer00228:06917] 15 more processes have sent help message help-mpi-btl-base.txt / btl:no-nics
[en-cer00228:06917] Set MCA parameter "orte_base_help_aggregate" to 0 to see all help / error messages
[3] #0  Foam::error::printStack(Foam::Ostream&) at ??:?
[3] #1  Foam::sigFpe::sigHandler(int) at ??:?
[3] #2  ? in /lib/x86_64-linux-gnu/libc.so.6
[3] #3  Foam::GaussSeidelSmoother::smooth(Foam::word const&, Foam::Field<double>&, Foam::lduMatrix const&, Foam::Field<double> const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, unsigned char, int) at ??:?
[3] #4  Foam::GaussSeidelSmoother::smooth(Foam::Field<double>&, Foam::Field<double> const&, unsigned char, int) const at ??:?
[3] #5  Foam::smoothSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
[3] #6  Foam::fvMatrix<Foam::Vector<double> >::solveSegregated(Foam::dictionary const&) at ??:?
[3] #7  Foam::fvMatrix<Foam::Vector<double> >::solveSegregatedOrCoupled(Foam::dictionary const&) at ??:?
[3] #8  Foam::fvMesh::solve(Foam::fvMatrix<Foam::Vector<double> >&, Foam::dictionary const&) const at ??:?
[3] #9  ? at ??:?
[3] #10  __libc_start_main in /lib/x86_64-linux-gnu/libc.so.6
[3] #11  ? at ??:?
[en-cer00228:06924] *** Process received signal ***
[en-cer00228:06924] Signal: Floating point exception (8)
[en-cer00228:06924] Signal code:  (-6)
[en-cer00228:06924] Failing at address: 0x335bd92400001b0c
[en-cer00228:06924] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x354b0)[0x7fa21dba24b0]
[en-cer00228:06924] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0x38)[0x7fa21dba2428]
[en-cer00228:06924] [ 2] /lib/x86_64-linux-gnu/libc.so.6(+0x354b0)[0x7fa21dba24b0]
[en-cer00228:06924] [ 3] /data/openFOAM/OpenFOAM-v1906/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZN4Foam19GaussSeidelSmoother6smoothERKNS_4wordERNS_5FieldIdEERKNS_9lduMatrixERKS5_RKNS_10FieldFieldIS4_dEERKNS_8UPtrListIKNS_17lduInterfaceFieldEEEhi+0x347)[0x7fa21ef0e4e7]
[en-cer00228:06924] [ 4] /data/openFOAM/OpenFOAM-v1906/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZNK4Foam19GaussSeidelSmoother6smoothERNS_5FieldIdEERKS2_hi+0x28)[0x7fa21ef0e688]
[en-cer00228:06924] [ 5] /data/openFOAM/OpenFOAM-v1906/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZNK4Foam12smoothSolver5solveERNS_5FieldIdEERKS2_h+0x6ed)[0x7fa21ef05a3d]
[en-cer00228:06924] [ 6] /data/openFOAM/OpenFOAM-v1906/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so(_ZN4Foam8fvMatrixINS_6VectorIdEEE15solveSegregatedERKNS_10dictionaryE+0x5d3)[0x7fa222f1f893]
[en-cer00228:06924] [ 7] /data/openFOAM/OpenFOAM-v1906/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so(_ZN4Foam8fvMatrixINS_6VectorIdEEE24solveSegregatedOrCoupledERKNS_10dictionaryE+0x408)[0x7fa222f2c4b8]
[en-cer00228:06924] [ 8] /data/openFOAM/OpenFOAM-v1906/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so(_ZNK4Foam6fvMesh5solveERNS_8fvMatrixINS_6VectorIdEEEERKNS_10dictionaryE+0x23)[0x7fa222ed5e33]
[en-cer00228:06924] [ 9] pimpleFoam[0x426521]
[en-cer00228:06924] [10] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xf0)[0x7fa21db8d830]
[en-cer00228:06924] [11] pimpleFoam[0x428589]
[en-cer00228:06924] *** End of error message ***
I do not know what is the cause of that problem, but seems something related to linear equation solver


All times are GMT -4. The time now is 08:39.