CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

simulating flow over naca0012 using LES (WALE subgrid model)

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 9, 2019, 07:00
Default simulating flow over naca0012 using LES (WALE subgrid model)
  #1
New Member
 
zein elserfy
Join Date: May 2018
Posts: 12
Rep Power: 3
zeinelserfy is on a distinguished road
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

pressure fields

after running les simulation for few time step results seems to be not converged
the velocity field

pressure field



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

Last edited by zeinelserfy; October 9, 2019 at 07:29. Reason: adding more information
zeinelserfy is offline   Reply With Quote

Old   October 9, 2019, 08:01
Default
  #2
Member
 
Lilian Chabannes
Join Date: Apr 2017
Posts: 54
Rep Power: 4
Lookid is on a distinguished road
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
__________________
Feel free to join the OpenFOAM Discord https://discord.gg/P9p9eHn, a live chat about OpenFOAM
Lookid is offline   Reply With Quote

Old   October 9, 2019, 09:21
Default
  #3
Senior Member
 
Santiago Lopez Castano
Join Date: Nov 2012
Posts: 233
Rep Power: 9
Santiago is on a distinguished road
Quote:
Originally Posted by Lookid View Post
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.
Santiago is offline   Reply With Quote

Old   October 9, 2019, 09:34
Default
  #4
Member
 
Lilian Chabannes
Join Date: Apr 2017
Posts: 54
Rep Power: 4
Lookid is on a distinguished road
Thank you for the clarifications

Quote:
Originally Posted by Santiago View Post
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 View Post
A proper LES (explicit) must avoid low-order upwinding
I used the filteredLinear thingy because I had this wavy pattern (Dicretization schemes in LES (pitzDaily)). 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.
__________________
Feel free to join the OpenFOAM Discord https://discord.gg/P9p9eHn, a live chat about OpenFOAM
Lookid is offline   Reply With Quote

Old   October 9, 2019, 09:40
Default
  #5
New Member
 
zein elserfy
Join Date: May 2018
Posts: 12
Rep Power: 3
zeinelserfy is on a distinguished road
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 is offline   Reply With Quote

Old   October 9, 2019, 19:40
Default
  #6
New Member
 
zein elserfy
Join Date: May 2018
Posts: 12
Rep Power: 3
zeinelserfy is on a distinguished road
Quote:
Originally Posted by Santiago View Post
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 View Post
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 is offline   Reply With Quote

Old   October 9, 2019, 21:12
Default
  #7
New Member
 
zein elserfy
Join Date: May 2018
Posts: 12
Rep Power: 3
zeinelserfy is on a distinguished road
Quote:
Originally Posted by Lookid View Post
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
zeinelserfy is offline   Reply With Quote

Reply

Tags
les model, naca0012, wale

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Use of k-epsilon and k-omega Models Jade M Main CFD Forum 38 September 17, 2019 03:05
[rhoCentralFoam] simulating compressible inviscid flow Yuval OpenFOAM Running, Solving & CFD 2 January 27, 2016 21:33
Discrete Phase Model, outlet mass flow rate does not fit edu_aero FLUENT 28 September 18, 2015 06:53
Wrong flow in ratating domain problem Sanyo CFX 17 August 15, 2015 06:20
Multiphase flow. Dispersed and free surface model Luis CFX 8 May 29, 2007 18:13


All times are GMT -4. The time now is 08:45.