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

simpleFoam: floating point exception

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

Like Tree1Likes
  • 1 Post By wyldckat

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 17, 2015, 09:42
Default simpleFoam: floating point exception
  #1
Senior Member
 
M. C.
Join Date: May 2013
Location: Italy
Posts: 286
Blog Entries: 6
Rep Power: 15
student666 is on a distinguished road
Hi all,

i'm facing a floating point exception as for bounding of k on a MRF simulation with simpleFoam.
As you may see, k bounding min value goes zero and then solution blows up.

Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.3.1-bcfaaa7b8660
Exec   : simpleFoam
Date   : Jan 17 2015
Time   : 14:00:39
Host   : "imatUbuntu"
PID    : 10043
Case   : /home/imatubuntu/OpenFOAM/imatubuntu-2.3.1/run/work/daria_small/canaleOutEBM/run
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

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

Create mesh for time = 450

Reading field p

Reading field U

Reading/calculating face flux field phi

AMI: Creating addressing and weights between 23802 source faces and 24851 target faces
AMI: Patch source sum(weights) min/max/average = 0.99887638, 1.0072276, 1.0003408
AMI: Patch target sum(weights) min/max/average = 0.99894094, 1.0013817, 1.0000049
AMI: Creating addressing and weights between 19122 source faces and 4952 target faces
AMI: Patch source sum(weights) min/max/average = 0.81524507, 1.0000002, 0.99936938
AMI: Patch target sum(weights) min/max/average = 0.88260207, 1, 0.99875295
AMI: Creating addressing and weights between 12730 source faces and 2812 target faces
AMI: Patch source sum(weights) min/max/average = 0.99845796, 1.0051665, 1.0002107
AMI: Patch target sum(weights) min/max/average = 0.99968809, 1.0016961, 1.0000635
Selecting incompressible transport model Newtonian
Selecting RAS turbulence model kEpsilon
bounding k, min: 3.4598366e-31 max: 790.70186 average: 1.6601081
kEpsilonCoeffs
{
Cmu             0.09;
C1              1.44;
C2              1.92;
sigmaEps        1.3;
}

Creating finite volume options from "system/fvOptions"

Selecting finite volume options model type MRFSource
Source: MRF1
- applying source for all time
- selecting cells using cellZone MRF
- selected 2071456 cell(s) with volume 0.00052479319

Selecting finite volume options model type explicitPorositySource
Source: porosity1
- applying source for all time
- selecting cells using cellZone batteria
- selected 316332 cell(s) with volume 0.0017791776

Porosity region porosity1:
selecting model: DarcyForchheimer
creating porous zone: batteria

SIMPLE: convergence criteria
field p     tolerance 0.0001
field U     tolerance 0.001
field "(k|epsilon|omega)"     tolerance 0.001


Starting time loop

phi: phi
Compressible: 0
Turbulent: 1
LES: 0
Time = 465

--> FOAM Warning :
From function gaussConvectionScheme
in file finiteVolume/convectionSchemes/gaussConvectionScheme/gaussConvectionScheme.H at line 123
Reading "/home/imatubuntu/OpenFOAM/imatubuntu-2.3.1/run/work/daria_small/canaleOutEBM/run/system/fvSchemes.divSchemes.div(phi,U)" at line 34
Unbounded 'Gauss' div scheme used in steady-state solver, use 'bounded Gauss' to ensure boundedness.
To remove this warning switch off 'warnUnboundedGauss' in "/opt/openfoam231/etc/controlDict"
DILUPBiCG:  Solving for Ux, Initial residual = 0.00073404819, Final residual = 1.4551955e-05, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 0.00060673146, Final residual = 1.1398202e-05, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 0.00067247603, Final residual = 1.2637159e-05, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.00093841547, Final residual = 8.1897134e-07, No Iterations 7
GAMG:  Solving for p, Initial residual = 6.7902153e-05, Final residual = 6.4216769e-08, No Iterations 8
time step continuity errors : sum local = 1.9119291e-06, global = 5.0391913e-07, cumulative = 2.4629033e-06
DILUPBiCG:  Solving for epsilon, Initial residual = 0.00011465046, Final residual = 3.22368e-06, No Iterations 1
DILUPBiCG:  Solving for k, Initial residual = 0.00019167693, Final residual = 3.4461782e-06, No Iterations 1
bounding k, min: 0 max: 789.99843 average: 1.6552599
ExecutionTime = 602.8 s  ClockTime = 604 s

MassFlows:   outlet = 37.136307  inlet = -37.127109
Time = 466

--> FOAM Warning :
From function gaussConvectionScheme
in file finiteVolume/convectionSchemes/gaussConvectionScheme/gaussConvectionScheme.H at line 123
Reading "/home/imatubuntu/OpenFOAM/imatubuntu-2.3.1/run/work/daria_small/canaleOutEBM/run/system/fvSchemes.divSchemes.div(phi,U)" at line 34
Unbounded 'Gauss' div scheme used in steady-state solver, use 'bounded Gauss' to ensure boundedness.
To remove this warning switch off 'warnUnboundedGauss' in "/opt/openfoam231/etc/controlDict"
DILUPBiCG:  Solving for Ux, Initial residual = 0.00073368581, Final residual = 1.4702976e-05, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 0.00060705033, Final residual = 1.1472962e-05, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 0.00067250209, Final residual = 1.2664494e-05, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.00093413777, Final residual = 5.7548539e-07, No Iterations 7
GAMG:  Solving for p, Initial residual = 6.7233025e-05, Final residual = 4.1306896e-08, No Iterations 9
time step continuity errors : sum local = 1.2317376e-06, global = -8.7246108e-08, cumulative = 2.3756572e-06
#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::sigFpe::sigHandler(int) at ??:?
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) at ??:?
#4  void Foam::divide<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
#5  Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::operator/<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
#6  Foam::incompressible::RASModels::kEpsilon::correct() at ??:?
#7
at ??:?
#8  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9
at ??:?
Floating point exception (core dumped)
I'm using following 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                     steadyState;
}

gradSchemes
{
    default                   cellLimited Gauss linear 1; //Gauss linear//
 /*   grad(p)               cellLimited Gauss linear 1;// Gauss;
    grad(U)                 Gauss;*/
}

divSchemes
{
    default                     none;
   // div(phi,U)                   bounded Gauss linearUpwind default; //Joel suggestion
    div(phi,U)                 Gauss linearUpwindV cellLimited Gauss linear 1; //Alberto  http://www.cfd-online.com/Forums/openfoam/74618-simplefoam-convergence-large-domain-2.html
    //div(phi,U)            bounded Gauss limitedLinear 1; // bounded Gauss upwind
    div(phi,k)                  bounded Gauss upwind;
    div(phi,epsilon)            bounded Gauss upwind;
    div((nuEff*dev(T(grad(U)))))     Gauss linear;
}

laplacianSchemes
{
    default                    Gauss linear limited 0.5; //Joel suggestion
   // default                    Gauss linear limited 0.333;;//Gauss linear corrected;
   /* laplacian(nuEff,U)         Gauss linear corrected;
    laplacian((1|A(U)),p)         Gauss linear corrected;
    laplacian(DkEff,k)             Gauss linear corrected;
    laplacian(DepsilonEff,epsilon)     Gauss linear corrected;
    laplacian(DREff,R)             Gauss linear corrected;
    laplacian(DnuTildaEff,nuTilda)     Gauss linear corrected;
*/}

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

snGradSchemes
{
   //default                      limited 0.5; //joel suggestion
   // default                      limited 0; 
    default    corrected;
}

fluxRequired
{
    default         no;
    p               ;
}


// ************************************************************************* //
and fvSolution:

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      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
     p
  
    {
        solver          GAMG;
        tolerance       1e-08;
        relTol          0.001;//era 0.05
        smoother        GaussSeidel;
        cacheAgglomeration true;
        nCellsInCoarsestLevel 20;
        agglomerator    faceAreaPair;
        mergeLevels     1;
    }       

    U
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-05;
        relTol          0.1;
    }

    k
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-05;
        relTol          0.1;
    }

    epsilon
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-05;
        relTol          0.1;
    }

}

potentialFlow
{
    nNonOrthogonalCorrectors 1; //era10
}

SIMPLE
{
    nNonOrthogonalCorrectors 1;

    residualControl
    {
        p               1e-4;
        U               1e-3;
        "(k|epsilon|omega)" 1e-3;
    }
}



relaxationFactors
{
    fields
    {
        p               0.2;//0.2;
    }
    equations
    {
        U               0.3;//0.3;;
        k               0.3;//0.3;;
        epsilon         0.3;//0.3;;
       
    }
}


// ************************************************************************* //
what should I do or what other interpolation schemes should I use for k & epsilon?

thanks a lot
student666 is offline   Reply With Quote

Old   January 17, 2015, 10:41
Default
  #2
Senior Member
 
anonymous
Join Date: Aug 2014
Posts: 205
Rep Power: 11
ssss is on a distinguished road
bounding k, min: 0 max: 789.99843 average: 1.6552599

The max value doesn't seem to be right, which are your boundary conditions for the turbulence variables?

What does checkMesh say about your mesh?
ssss is offline   Reply With Quote

Old   January 17, 2015, 11:57
Default
  #3
Senior Member
 
M. C.
Join Date: May 2013
Location: Italy
Posts: 286
Blog Entries: 6
Rep Power: 15
student666 is on a distinguished road
Hi,

thanks for answering.

Just for understanding why do you say?
Quote:
The max value doesn't seem to be right
Here's the checkMesh log:

Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.3.1-bcfaaa7b8660
Exec   : checkMesh -parallel
Date   : Jan 17 2015
Time   : 17:43:48
Host   : "imatUbuntu"
PID    : 8809
Case   : /home/imatubuntu/OpenFOAM/imatubuntu-2.3.1/run/work/daria_small/canaleOutEBM/run
nProcs : 8
Slaves : 
7
(
"imatUbuntu.8810"
"imatUbuntu.8811"
"imatUbuntu.8812"
"imatUbuntu.8813"
"imatUbuntu.8814"
"imatUbuntu.8815"
"imatUbuntu.8816"
)

Pstream initialized with:
    floatTransfer      : 0
    nProcsSimpleSum    : 0
    commsType          : nonBlocking
    polling iterations : 0
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

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

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:           4172243
    faces:            11183065
    internal faces:   10306710
    cells:            3505516
    faces per cell:   6.1302744
    boundary patches: 21
    point zones:      0
    face zones:       0
    cell zones:       3

Overall number of cells of each type:
    hexahedra:     3271330
    prisms:        22206
    wedges:        0
    pyramids:      24665
    tet wedges:    0
    tetrahedra:    13498
    polyhedra:     173817
    Breakdown of polyhedra by number of faces:
        faces   number of cells
            6   27315
            7   11608
            8   1449
            9   102527
           12   24206
           13   2
           15   6082
           16   1
           17   1
           18   372
           20   4
           21   190
           24   60

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
   *Number of regions: 3
    The mesh has multiple regions which are not connected by any face.
  <<Writing region information to "0/cellToRegion"
  <<Writing region 0 with 2064714 cells to cellSet region0
  <<Writing region 1 with 726918 cells to cellSet region1
  <<Writing region 2 with 713884 cells to cellSet region2

Checking basic patch addressing...
                   Patch    Faces   Points
                AMI_ROT1    23802    25146
                AMI_ROT3    19122    19718
                AMI_ROT2    12730    13839
                  blades   299506   302735
               boccaglio   125559   127400
                wallStat    31222    32677
                 amiAsp1     2812     3124
                 amiAsp2     4952     5017
                   inlet    16413    16848
                    tubi    38109    38461
                 wallAsp    41432    41375
                wallBatt    32061    33455
                wallDead     3590     3824
          amiFanRotating    24851    25628
                  outlet    74704    74937
          wallEspulsione    56594    57131
                 wallExt    13638    14000

Checking geometry...
    Overall domain bounding box (-0.173186 -0.2175 -0.35) (0.54 0.8 0.32225)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (-1.1273693e-15 -6.0712876e-15 -5.5882177e-16) OK.
    Max cell openness = 3.9932212e-16 OK.
    Max aspect ratio = 22.763918 OK.
    Minimum face area = 1.1992557e-13. Maximum face area = 0.00023338634.  Face area magnitudes OK.
    Min volume = 2.829272e-14. Max volume = 3.7684994e-06.  Total volume = 0.12891844.  Cell volumes OK.
    Mesh non-orthogonality Max: 79.296812 average: 6.0672307
   *Number of severely non-orthogonal (> 70 degrees) faces: 103.
    Non-orthogonality check OK.
  <<Writing 103 non-orthogonal faces to set nonOrthoFaces
    Face pyramids OK.
 ***Max skewness = 5.0571991, 82 highly skew faces detected which may impair the quality of the results
  <<Writing 99 skew faces to set skewFaces
    Coupled point location match (average 0) OK.

Failed 1 mesh checks.

End

Finalising parallel run
here's the k bounday conditions:

Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -2 0 0 0 0];

internalField   uniform 0.03375;

boundaryField
{
    outlet
    {
        type         zeroGradient;
    }
    inlet
    {
        type         zeroGradient;
    }


    wallAsp
    {
        type            kLowReWallFunction; //kqRWallFunction;
        value           uniform 0.0000001;
    }
    wallDead
    {
        type            kLowReWallFunction; //kqRWallFunction;
        value           uniform 0.0000001;
    }

    wallExt
    {
        type            kLowReWallFunction; //kqRWallFunction;
        value           uniform 0.0000001;
    }
    boccaglio
    {
        type            kLowReWallFunction; //kqRWallFunction;
        value           uniform 0.0000001;
    }
    blades
    {
        type            kLowReWallFunction; //kqRWallFunction;
        value           uniform 0.0000001;
    }
    wallStat
    {
        type            kLowReWallFunction; //kqRWallFunction;
        value           uniform 0.0000001;
    }
  /*  wallFan
    {
        type            kLowReWallFunction; //kqRWallFunction;
        value           uniform 0.0000001;
    }*/
    wallEspulsione
    {
        type            kLowReWallFunction; //kqRWallFunction;
        value           uniform 0.0000001;
    }
    tubi
    {
        type            kLowReWallFunction; //kqRWallFunction;
        value           uniform 0.0000001;
    }
    wallBatt
    {
        type            kLowReWallFunction; //kqRWallFunction;
        value           uniform 0.0000001;
    }


    AMI_ROT1
    {
        type            cyclicAMI;
        value           $internalField;
    }
    AMI_ROT2
    {
        type            cyclicAMI;
        value           $internalField;
    }
    AMI_ROT3
    {
        type            cyclicAMI;
        value           $internalField;
    }
    amiAsp1
    {
        type            cyclicAMI;
        value           $internalField;
    }
    amiAsp2
    {
        type            cyclicAMI;
        value           $internalField;
    }
    amiFanRotating
    {
        type            cyclicAMI;
        value           $internalField;
    }

}


// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      epsilon;            // EPSILON = Turbulent Dissipation Rate recalculate
                    // for each new case.   e=Cu*((k^(3/2))/l)   
                    // Cu=Turbulent Constant=0.09
                    // k=Turbulent Kinetic Energy     l=Turbulent Length Scale
                    // l can be estimated.  l=0.038*dh   dh=pipe diameter
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -3 0 0 0 0];

internalField   uniform 0.006975;           // was 0.000765

boundaryField 
{


    outlet
    {
        type         zeroGradient;
    }
    inlet
    {
        type         zeroGradient;
    }


    wallAsp
    {
        type            epsilonLowReWallFunction; //epsilonWallFunction;        
        value           uniform 0.006975;
    }
    wallDead
    {
        type            epsilonLowReWallFunction; //epsilonWallFunction;        
        value           uniform 0.006975;
    }

    wallExt
    {
        type            epsilonLowReWallFunction; //epsilonWallFunction;        
        value           uniform 0.006975;
    }
    boccaglio
    {
        type            epsilonLowReWallFunction; //epsilonWallFunction;        
        value           uniform 0.006975;
    }
    blades
    {
        type            epsilonLowReWallFunction; //epsilonWallFunction;        
        value           uniform 0.006975;
    }
    wallStat
    {

        value           uniform 0.006975;
    }

    wallEspulsione
    {
        type            epsilonLowReWallFunction; //epsilonWallFunction;       
        value           uniform 0.006975;
    }
    tubi
    {
        type            epsilonLowReWallFunction; //epsilonWallFunction;       
        value           uniform 0.006975;
    }
    wallBatt
    {
        type            epsilonLowReWallFunction; //epsilonWallFunction;        
        value           uniform 0.006975;
    }


    AMI_ROT1
    {
        type            cyclicAMI;
        value           $internalField;
    }
    AMI_ROT2
    {
        type            cyclicAMI;
        value           $internalField;
    }
    AMI_ROT3
    {
        type            cyclicAMI;
        value           $internalField;
    }
    amiAsp1
    {
        type            cyclicAMI;
        value           $internalField;
    }
    amiAsp2
    {
        type            cyclicAMI;
        value           $internalField;
    }
    amiFanRotating
    {
        type            cyclicAMI;
        value           $internalField;
    }

}


// ************************************************************************* //
I'm using epsilonLowReWallFunction & kLowReWallFunction as I can't keep a constnt value for y+.

Code:
Time = 100
Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting RAS turbulence model kEpsilon
kEpsilonCoeffs
{
    Cmu             0.09;
    C1              1.44;
    C2              1.92;
    sigmaEps        1.3;
}

Patch 3 named blades y+ : min: 0.67807798 max: 47.861605 average: 10.385627

Patch 4 named boccaglio y+ : min: 0.15849079 max: 42.118054 average: 3.7682556

Patch 5 named wallStat y+ : min: 0.36632298 max: 10.071332 average: 4.5537257

Patch 9 named tubi y+ : min: 0.10642169 max: 23.319607 average: 3.006639

Patch 10 named wallAsp y+ : min: 0.00080009906 max: 8.0571449 average: 1.8477912

Patch 11 named wallBatt y+ : min: 0.026648156 max: 30.8113 average: 2.1785036

Patch 12 named wallDead y+ : min: 0.00056670836 max: 2.7034135 average: 0.53314965

Patch 15 named wallEspulsione y+ : min: 0.15375772 max: 13.502387 average: 3.3477829

Patch 16 named wallExt y+ : min: 0.039157284 max: 3.4930396 average: 0.58972471

Writing yPlus to field yPlus

End
student666 is offline   Reply With Quote

Old   January 17, 2015, 14:51
Default
  #4
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,965
Blog Entries: 45
Rep Power: 126
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Greetings to all!

Quote:
Originally Posted by student666 View Post
Just for understanding why do you say?
Quote:
The max value doesn't seem to be right
@student666: I believe that ssss was possibly referring to personal experience with simulations made with simpleFoam. That value simply seems too high. Or just compare to the average value it's telling you and it's somewhat easy to guess that something is unlikely going very well in your simulation

From what I can see from the boundary conditions you've described, it seems to me that you've incorrectly defined them. I say this because you posted that you have the following boundary condition in the file "epsilon":
Code:
    wallStat
    {

        value           uniform 0.006975;
    }
The solver would very likely have complained about the fact that this boundary condition does not have a type defined.
Therefore, my guess is that you've modified the field files in the "0" folder, after having already simulated for 465 iterations or less. Which is why you should double-check the boundary conditions you have defined for these field files in the folder "465".

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   January 17, 2015, 16:58
Default
  #5
Senior Member
 
M. C.
Join Date: May 2013
Location: Italy
Posts: 286
Blog Entries: 6
Rep Power: 15
student666 is on a distinguished road
Hi and thanks.

I think the best solution is re-mesh the whole domain once again. Maybe skewness is quite surely 20% of the problem that can help me to improve by 80%.

By the way I try to ask:
what's the reason of using bounding schemes? or where can I read something about them?

About turbulence BC:
as for complex geometry it's quite hard to keep a proper value for y+; are epsilonLowReWallFunction & kLowReWallFunction a good alternative choice for wall functions?

Bye
student666 is offline   Reply With Quote

Old   January 18, 2015, 04:16
Default
  #6
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,965
Blog Entries: 45
Rep Power: 126
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Quick answers:
Quote:
Originally Posted by student666 View Post
By the way I try to ask:
what's the reason of using bounding schemes? or where can I read something about them?
Feature introduced in version 2.2.0. Very detailed explanation is given here: http://www.openfoam.org/version2.2.0/numerics.php

Quote:
Originally Posted by student666 View Post
About turbulence BC:
as for complex geometry it's quite hard to keep a proper value for y+; are epsilonLowReWallFunction & kLowReWallFunction a good alternative choice for wall functions?
Personally I've only recently found about the existence of these wall functions. I have not yet managed to fully understand in what situations it's correct to use them, therefore my advice is that you first test with simpler cases and prove with those cases if those boundary conditions are good enough for your case or not.
student666 likes this.
wyldckat is offline   Reply With Quote

Old   February 12, 2016, 04:56
Default MRFSimpleFoam - Convergence Problem!!
  #7
New Member
 
ravi
Join Date: Nov 2013
Posts: 10
Rep Power: 10
ark704 is on a distinguished road
Hi all,

I am trying to simulate a centrifugal fan with 3 individual meshes merged-(suction, impeller and spiral). My BC's are : Total Pressure Inlet and Volumetric Flow Outlet. My solver is blowing up showing the time step errors, bounding k and bounding epsilon in the range of e+30. How should I rectify this problem?

CheckMesh result is:
-------------------------------------------------------------------------------
Time = 0

Mesh stats
points: 814585
faces: 8243673
internal faces: 7706091
cells: 3987441
faces per cell: 4
boundary patches: 18
point zones: 0
face zones: 3
cell zones: 3

Overall number of cells of each type:
hexahedra: 0
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 3987441
polyhedra: 0

Checking topology...
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
Topological cell zip-up check OK.
Face-face connectivity OK.
<<Writing 7128 cells with two non-boundary faces to set twoInternalFacesCells
*Number of regions: 3
The mesh has multiple regions which are not connected by any face.
<<Writing region information to "0/cellToRegion"
<<Writing region 0 with 1619250 cells to cellSet region0
<<Writing region 1 with 1005986 cells to cellSet region1
<<Writing region 2 with 1362205 cells to cellSet region2

Checking patch topology for multiply connected surfaces...
Patch Faces Points Surface topology Bounding box
BOTTOM_SUCTION 5851 3445 ok (non-closed singly connected) (-3.22441 -0.712981 0.619) (0.712984 3.22441 0.619)
......
CP_1_SPIRAL 2407 2391 ok (non-closed singly connected) (-0.807087 -0.806972 0.415827) (0.807087 0.806995 0.494288)

Checking geometry...
Overall domain bounding box (-3.22441 -3.022 -0.132) (1.8 3.22441 1.564)
Mesh (non-empty, non-wedge) directions (1 1 1)
Mesh (non-empty) directions (1 1 1)
Boundary openness (2.36031e-16 2.32438e-17 -1.14065e-15) OK.
Max cell openness = 3.07852e-16 OK.
Max aspect ratio = 6.08759 OK.
Minimum face area = 3.71673e-07. Maximum face area = 0.00797706. Face area magnitudes OK.
Min volume = 1.86704e-10. Max volume = 0.00016558. Total volume = 19.3189. Cell volumes OK.
Mesh non-orthogonality Max: 68.1213 average: 15.5462
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 0.749613 OK.
Coupled point location match (average 0) OK.
Face tets OK.
Min/max edge length = 0.000457433 0.15509 OK.
<<Writing 16 near (closer than 8.19382e-06 apart) points to set nearPoints
All angles in faces OK.
All face flatness OK.
Cell determinant (wellposedness) : minimum: 0 average: 1.47314
***Cells with small determinant (< 0.001) found, number of cells: 7128
<<Writing 7128 under-determined cells to set underdeterminedCells
Concave cell check OK.
Face interpolation weight : minimum: 0.0775184 average: 0.437831
Face interpolation weight check OK.
Face volume ratio : minimum: 0.0840324 average: 0.794736
Face volume ratio check OK.

Failed 1 mesh checks.

End
----------------------------------------------------------------------------

Please check the file attached and guide me. I have removed the polyMesh file as it is confidential.

https://drive.google.com/file/d/0B7c...ew?usp=sharing
ark704 is offline   Reply With Quote

Old   February 21, 2016, 14:20
Default
  #8
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,965
Blog Entries: 45
Rep Power: 126
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Quote:
Originally Posted by ark704 View Post
Please check the file attached and guide me. I have removed the polyMesh file as it is confidential.
Quick answer: Without the mesh, it's not possible to fully diagnose the problem, given that the problem might actually be only due to how the mesh itself is configured.

If you can provide a complete test case that reproduces the same error, but while using a non-confidential geometry/mesh, then anyone will be able to assist you. It's very simple, you only have to use a very simple format/shape for the blades and any other pieces, while at the same time you use the same case set-up strategy.
__________________
wyldckat is offline   Reply With Quote

Old   February 23, 2016, 07:36
Default Ercoftac Centrifugal Pump - 3D - Convergence Issue
  #9
New Member
 
ravi
Join Date: Nov 2013
Posts: 10
Rep Power: 10
ark704 is on a distinguished road
I am facing convergence problem while running Ercoftac Centrifugal Pump (3D case) using MRF approach in OF 2.4, OS: Ubuntu 14.04. I am getting some bounding epsilon and k problems. Pls let me know the corrections/suggestions. You can find the case here:

https://drive.google.com/file/d/0B7c...ew?usp=sharing
ark704 is offline   Reply With Quote

Old   March 13, 2016, 18:23
Default
  #10
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,965
Blog Entries: 45
Rep Power: 126
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Quick answer: I've taken a look into your case and there are 2 apparent critical issues:
  1. Mesh is not in the same refinement level on both sides of the AMI interface. The consequence is shown in the attached image "Very high k values.png", where the large cells near one of the outside blades are gathering very high k values, when compared to the neighbour values.
  2. The mesh near the tips of the rotor is not uniform, which can lead to incorrect estimates of how of the mass flow is exchanged with the nearby cells. If possible, you should have a mesh a bit more similar to the airfoil/wing simulations.
  3. Running:
    Code:
    yPlusRAS -time 121
    told me this:
    Code:
    Patch 0 named ROTOR_BLADE y+ : min: 11.105692 max: 127.60367 average: 46.005078
    
    Patch 2 named WALL_INT_ROTOR y+ : min: 11.231932 max: 72.648097 average: 43.512939
    
    Patch 3 named WALL_EXT_ROTOR y+ : min: 22.22387 max: 97.865986 average: 63.419179
    
    Patch 5 named WALL_INT_STATOR y+ : min: 19.46216 max: 111.93062 average: 69.351668
    
    Patch 8 named STATOR_BLADE y+ : min: 8.6841145 max: 383.89523 average: 141.29642
    
    Patch 9 named WALL_EXT_STATOR y+ : min: 19.463452 max: 111.28735 average: 69.255703
    The problems that I can see here are:
    1. "STATOR_BLADE" has a maximum y+ value that is above 300, which can be a reason for concern.
    2. The minimum y+ values are all below the lower turbulent value of 30. This means that you're using incorrectly the k-epsilon wall treatment functions.
      • You should probably switch to using the turbulence model k-omega SST, which can use wall treatment functions that work in the laminar-to-turbulent region.
Attached Images
File Type: jpg Very high k values.jpg (153.0 KB, 60 views)
__________________
wyldckat is offline   Reply With Quote

Reply

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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Floating point exception error Alan OpenFOAM Running, Solving & CFD 11 July 1, 2021 21:51
Floating point exception (core dumped), running a new solver Mahyar Javidi OpenFOAM Running, Solving & CFD 6 April 7, 2018 12:43
simpleFoam Floating point exception error -help sudhasran OpenFOAM Running, Solving & CFD 3 March 12, 2012 16:23
Pipe flow in settlingFoam floating point exception jochemvandenbosch OpenFOAM Running, Solving & CFD 4 February 16, 2012 03:24
block-structured mesh for t-junction Robert@cfd ANSYS Meshing & Geometry 20 November 11, 2011 04:59


All times are GMT -4. The time now is 14:49.