[au1]

Hi everybody,
I'm studying Mechanical Engineering at Politecnico di Bari (Italy). I'm writing a thesis analyzing incompressible flow over an airfoil. (turbulence model: k-omega; flow velocity: 20 m/s; nu=10^-4 m^2/s; rho= 1 kg/m^3)

I made the mesh with Pointwise. I run it first with Fluent and it worked.

I tried to run the analysis in OpenFOAM so I adapted the "motorbike" tutorial to my case. But it doesn't work.

Create time

Create mesh for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting RAS turbulence model kOmegaSST
kOmegaSSTCoeffs
{
alphaK1 0.85034;
alphaK2 1;
alphaOmega1 0.5;
alphaOmega2 0.85616;
gamma1 0.5532;
gamma2 0.4403;
beta1 0.075;
beta2 0.0828;
betaStar 0.09;
a1 0.31;
c1 10;
}

No field sources present


SIMPLE: no convergence criteria found. Calculations will run for 500 steps.


Starting time loop

Time = 1

#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 at smoothSolver.C:0
#4 Foam::smoothSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam"
#6
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam"
#7
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam"
#8 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam"
Floating point exception (core dumped)

Which is the problem? The smoothSolver? Boundary conditions? Mesh?

If you need any of the case files, please ask me.

[alexeym]

Hi,

As the solver crashes during the first iteration, it can be mesh, schemes, ICs and BCs. So please post:

1. checkMesh output
2. fvSchemes file
3. 0 folder

[au1]

CheckMesh

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.0.1 |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.0.1-51f1de99a4bc
Exec : checkMesh
Date : Jan 09 2015
Time : 11:58:32
Host : ime048
PID : 16607
Case : /home/tesisti/Togati/9-1-15/riferimento
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

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

Create polyMesh for time = 0

Time = 0

Mesh stats
points: 207080
internal points: 0
faces: 411979
internal faces: 204899
cells: 102813
boundary patches: 4
point zones: 0
face zones: 0
cell zones: 0

Overall number of cells of each type:
hexahedra: 102813
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 0

Checking topology...
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
Patch Faces Points Surface topology
frontAndBack 205626 207080 ok (non-closed singly connected)
inlet 797 1596 ok (non-closed singly connected)
outlet 258 518 ok (non-closed singly connected)
wall 399 798 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (-8.99996 -10 0) (20.037 10 1)
Mesh (non-empty, non-wedge) directions (1 1 0)
Mesh (non-empty) directions (1 1 0)
All edges aligned with or perpendicular to non-empty directions.
Boundary openness (1.52339e-17 4.52257e-18 7.30337e-15) OK.
***High aspect ratio cells found, Max aspect ratio: 91679.8, number of cells 4620
<<Writing 4620 cells with high aspect ratio to set highAspectRatioCells
Minumum face area = 9.31926e-10. Maximum face area = 1.18331. Face area magnitudes OK.
Min volume = 9.31926e-10. Max volume = 0.755274. Total volume = 537.264. Cell volumes OK.
Mesh non-orthogonality Max: 86.8972 average: 3.26641
*Number of severely non-orthogonal faces: 49.
Non-orthogonality check OK.
<<Writing 49 non-orthogonal faces to set nonOrthoFaces
Face pyramids OK.
Max skewness = 0.693042 OK.

Failed 1 mesh checks.

End

fvSchemes

FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
default steadyState;
}

gradSchemes
{
default Gauss linear;
}

divSchemes
{
default none;
div(phi,U) Gauss linearUpwindV grad(U);
div(phi,k) Gauss upwind;
div(phi,omega) Gauss upwind;
div((nuEff*dev(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
default Gauss linear corrected;
}

interpolationSchemes
{
default linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
}

I attached the 0 folder.

[alexeym]

Hi,

I was not able to find errors in the settings, my suggestions will be quite generic:

1. Change smoothSolver to PBiCG. Dictionary for the solver you can find in $FOAM_TUTORIALS/heatTransfer/buoyantBoussinesqPimpleFoam/hotRoom/system/fvSolution.

2. As your mesh has highly non-orthogonal faces, consider using cellMDLimited modifications of schemes for gradients. Examples can be found in $FOAM_TUTORIALS/incompressible/pisoFoam/les/motorBike/motorBike/system/fvSchemes (though not quite sure it will be there in 2.1.1, I don't have this version installed).

3. Add bounded to divergence schemes. Example can be found in $FOAM_TUTORIALS/incompressible/simpleFoam/pitzDailyExptInlet/system/fvSchemes.

[ssss]

Your does seem to be the problem. Are you sure you changed frontAndBack to empty in the boundary file?

[au1]

@alexeym

1) I changed the solver for U, k, omega from smoothSolver to PBiCG.

2) I used cellMDLimited

gradSchemes
{
default cellMDLimited Gauss linear 1;
}

3) In fvSchemes file of pitzDailyExptInlet tutorial I found this:

divSchemes
{
default none;
div(phi,U) Gauss upwind;
div(phi,k) Gauss upwind;
div(phi,epsilon) Gauss upwind;
div(phi,R) Gauss upwind;
div(R) Gauss linear;
div(phi,nuTilda) Gauss upwind;
div((nuEff*dev(T(grad(U))))) Gauss linear;
}

and when i tried to add "bounded" like this

divSchemes
{
default none;
div(phi,U) bounded Gauss linearUpwindV grad(U);
div(phi,k) bounded Gauss upwind;
div(phi,omega) bounded Gauss upwind;
div((nuEff*dev(T(grad(U))))) bounded Gauss linear;
}

or like this

divSchemes
{
default bounded;
}

it gaves me an error:

--> FOAM FATAL IO ERROR:
unknown div scheme bounded

Valid div schemes are :

1
(
Gauss
)

So I tried to run with only modifications 1 and 2.
Results:

Starting time loop

Time = 1

DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 6.09293e-05, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.000172088, No Iterations 1
#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::GAMGSolver::scalingFactor(Foam::Field<double >&, Foam::Field<double> const&, Foam::Field<double> const&, Foam::Field<double> const&) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4 Foam::GAMGSolver::scalingFactor(Foam::Field<double >&, Foam::lduMatrix const&, Foam::Field<double>&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMa trix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#8
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam"
#9 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#10
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam"
Floating point exception (core dumped)

@ssss
Yes, boundary conditions are ok.

Any more tips? Should be the problem the GAMGSolver (which is the selected solver for p)?

[ssss]

In order to use bounded in the fvSchemes you need Openfoam2.2.0 or greater, you are using of2.1.1

Are you sure your boundary conditions are correct? Maybe there is a variable whith initial value of 0 (omega...)?

[alexeym]

Hi,

Well, guess bounded was not implemented in 2.1.1.

According to the output, this time FPE happens in pEqn.H, so you've got two options:

1. Change solver for pressure to PCG.

2. Increase number of cell in coarsest level for GAMG solver (nCellsInCoarsestLevel). In general I set this value to nCellsInMesh^(1/3) (for 2D case it could be nCellsInMesh^(1/2), so for ~100,000 cells in your mesh the value should be around 320)

Also I've noticed this line in the output:

SIMPLE: no convergence criteria found. Calculations will run for 500 steps.

I think you should add residualControl to the SIMPLE dictionary in fvSolution file. You can find example in $FOAM_TUTORIALS/incompressible/simpleFoam/pitzDaily/system/fvSolution. Though in general final residuals should be around 1e-6 (in the example 1e-2/1e-3 were used).

[au1]

I'll download the 2.2 version as last option

@ssss
omega value is 1.78 everywhere. I uploaded the 0 folder in a precedent post so you can check it.

I added residualControl.

I increased the number of cell in coarsest level

p
{
solver GAMG;
tolerance 1e-7;
relTol 0.1;
smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
cacheAgglomeration on;
agglomerator faceAreaPair;
nCellsInCoarsestLevel 320;
mergeLevels 1;
}

but i had the same error.

So I changed the GAMG solver

p
{
solver PCG;
preconditioner DIC;
tolerance 1e-6;
relTol 0;
}

It run. I set endTime=500 in order to monitorate the situation. When I tried to open the results in paraView i had a problem:

created temporary '17-cfd.OpenFOAM'
Segmentation fault (core dumped)

So I couldn't visualize the results.

Looking to last outputs I think that something went wrong

Time = 499

DILUPBiCG: Solving for Ux, Initial residual = 0.0176025, Final residual = 8.92661e-06, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.022828, Final residual = 8.31351e-06, No Iterations 1
DICPCG: Solving for p, Initial residual = 3.92221e-07, Final residual = 3.92221e-07, No Iterations 0
time step continuity errors : sum local = 2.19464e+34, global = 9.28582e+31, cumulative = 9.09985e+32
DILUPBiCG: Solving for omega, Initial residual = 0.119754, Final residual = 2.62773e-05, No Iterations 1
DILUPBiCG: Solving for k, Initial residual = 0.160839, Final residual = 5.17799e-05, No Iterations 1
ExecutionTime = 851.27 s ClockTime = 854 s

forceCoeffs output:
Cd = -3.43866e+69
Cl = -3.51752e+53
Cm = -1.71933e+69
Cl(f) = 1.71933e+69
Cl(r) = -1.71933e+69

Time = 500

DILUPBiCG: Solving for Ux, Initial residual = 0.0153715, Final residual = 7.43431e-06, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.0209576, Final residual = 1.01333e-05, No Iterations 1
DICPCG: Solving for p, Initial residual = 4.0874e-07, Final residual = 4.0874e-07, No Iterations 0
time step continuity errors : sum local = 2.21535e+34, global = 1.02473e+32, cumulative = 1.01246e+33
DILUPBiCG: Solving for omega, Initial residual = 0.112249, Final residual = 9.26829e-06, No Iterations 1
DILUPBiCG: Solving for k, Initial residual = 0.152886, Final residual = 4.04e-05, No Iterations 1
ExecutionTime = 859.41 s ClockTime = 862 s

forceCoeffs output:
Cd = -3.43851e+69
Cl = -3.51762e+53
Cm = -1.71925e+69
Cl(f) = 1.71925e+69
Cl(r) = -1.71925e+69

End

Force coefficients have impossible values. And what about the time step continuity errors?

Any more tips before updating OF in order to use the bounded divSchemes?

[alexeym]

Hi,

"relTol 0" in pressure solver is too strict. Let it be 1e-2 or 0.1. Don't know what values of tolerance and relTol you have for velocity.

As you can see from residuals, solution is far from convergence. Increase endTime to say 25000. If solution converge earlier, it will just stop at the point of convergence.

Don't know the reason for the core dump, though as solution diverges, maybe certain values in result files lead to this behavior. Try using paraview's build-in OpenFOAM reader (paraFoam -builtin).

[au1]

I fixed the fvSolution file

solvers
{
p
{
solver PCG;
preconditioner DIC;
tolerance 1e-6;
relTol 0.1;
}

U
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-6;
relTol 0.1;
}

k
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-6;
relTol 0.1;
}

omega
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-6;
relTol 0.1;
}
}

SIMPLE
{
nNonOrthogonalCorrectors 0;
}

residualControl
{
p 1e-6;
U 1e-6;
k 1e-6;
omega 1e-6
}

potentialFlow
{
nNonOrthogonalCorrectors 10;
}

relaxationFactors
{
fields
{
p 0.3;
}
equations
{
U 0.7;
k 0.7;
omega 0.7;
}
}

cache
{
grad(U);
}

I set endTime to 25000.

Results:

Time = 826

DILUPBiCG: Solving for Ux, Initial residual = 0.459715, Final residual = 0.0100426, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.506025, Final residual = 0.0107321, No Iterations 1
DICPCG: Solving for p, Initial residual = 1.09289e-05, Final residual = 1.25529e-08, No Iterations 1
time step continuity errors : sum local = 4.44341e+58, global = 1.99964e+53, cumulative = 5.47876e+55
DILUPBiCG: Solving for omega, Initial residual = 0.533658, Final residual = 1.7975e-09, No Iterations 1
DILUPBiCG: Solving for k, Initial residual = 0.373316, Final residual = 1.61836e-07, No Iterations 1
ExecutionTime = 1028.32 s ClockTime = 1032 s

forceCoeffs output:
Cd = -1.33784e+122
Cl = -1.28579e+108
Cm = -6.68919e+121
Cl(f) = 6.68919e+121
Cl(r) = -6.68919e+121

Time = 827

DILUPBiCG: Solving for Ux, Initial residual = 0.507959, Final residual = 0.00769252, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.511595, Final residual = 0.00614268, No Iterations 1
DICPCG: Solving for p, Initial residual = 8.71646e-05, Final residual = 9.2361e-08, No Iterations 1
time step continuity errors : sum local = 4.93263e+58, global = 4.62504e+51, cumulative = 5.47922e+55
DILUPBiCG: Solving for omega, Initial residual = 0.517434, Final residual = 1.72607e-06, No Iterations 1
#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#5 Foam::fvMatrix<double>::solve() in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so"
#6 Foam::incompressible::RASModels::kOmegaSST::correc t() in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so"
#7
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam"
#8 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/simpleFoam"
Floating point exception (core dumped)

[alexeym]

Hi,

1. Increase number of non-orthogonal correctors. nNonOrthogonalCorrectors in SIMPLE dictionary. Set it to 3-4.

2. If solution still diverges. Relax more. Set relaxation factor for velocity to 0.3.

[au1]

I set the number of non-orthogonal correctors to 4.

Time = 24999

DILUPBiCG: Solving for Ux, Initial residual = 1.57507e-05, Final residual = 2.77971e-07, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 8.88111e-05, Final residual = 3.18473e-06, No Iterations 2
DICPCG: Solving for p, Initial residual = 0.000894356, Final residual = 8.78172e-05, No Iterations 9
DICPCG: Solving for p, Initial residual = 9.23095e-05, Final residual = 9.02085e-06, No Iterations 94
DICPCG: Solving for p, Initial residual = 9.77823e-06, Final residual = 9.6372e-07, No Iterations 55
DICPCG: Solving for p, Initial residual = 1.04882e-06, Final residual = 6.18521e-07, No Iterations 1
DICPCG: Solving for p, Initial residual = 6.19302e-07, Final residual = 6.19302e-07, No Iterations 0
time step continuity errors : sum local = 4.35178e-08, global = 8.0513e-09, cumulative = 1.09825e-05
DILUPBiCG: Solving for omega, Initial residual = 8.58339e-07, Final residual = 8.58339e-07, No Iterations 0
DILUPBiCG: Solving for k, Initial residual = 1.79678e-05, Final residual = 4.7525e-07, No Iterations 1
ExecutionTime = 9546.81 s ClockTime = 9575 s

forceCoeffs output:
Cd = 0.0370108
Cl = 5.52511e-19
Cm = 0.0185054
Cl(f) = -0.0185054
Cl(r) = 0.0185054

Time = 25000

DILUPBiCG: Solving for Ux, Initial residual = 1.57509e-05, Final residual = 2.77264e-07, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 8.88113e-05, Final residual = 3.18471e-06, No Iterations 2
DICPCG: Solving for p, Initial residual = 0.000875004, Final residual = 7.37109e-05, No Iterations 10
DICPCG: Solving for p, Initial residual = 9.25738e-05, Final residual = 8.82807e-06, No Iterations 90
DICPCG: Solving for p, Initial residual = 2.34116e-05, Final residual = 2.25928e-06, No Iterations 32
DICPCG: Solving for p, Initial residual = 1.41847e-05, Final residual = 1.23549e-06, No Iterations 2
DICPCG: Solving for p, Initial residual = 1.30288e-05, Final residual = 1.02704e-06, No Iterations 1
time step continuity errors : sum local = 7.21817e-08, global = -8.91159e-09, cumulative = 1.09736e-05
DILUPBiCG: Solving for omega, Initial residual = 8.58635e-07, Final residual = 8.58635e-07, No Iterations 0
DILUPBiCG: Solving for k, Initial residual = 1.79674e-05, Final residual = 4.85255e-07, No Iterations 1
ExecutionTime = 9552.63 s ClockTime = 9581 s

forceCoeffs output:
Cd = 0.0370012
Cl = 5.52454e-19
Cm = 0.0185006
Cl(f) = -0.0185006
Cl(r) = 0.0185006

End

Why lift coefficient is so small? (Fluent result for Cl was 0.8)

[alexeym]

Hi,

If you take a look at forceCoeffs.C:

        // lift, drag and moment
        coeffs[0] = (totForce & liftDir_)/(Aref_*pDyn);
        coeffs[1] = (totForce & dragDir_)/(Aref_*pDyn);
        coeffs[2] = (totMoment & pitchAxis_)/(Aref_*lRef_*pDyn);

        scalar Cl = sum(coeffs[0]);
        scalar Cd = sum(coeffs[1]);
        scalar Cm = sum(coeffs[2]);

If your Cd is OK, then, I guess, you've made a mistake in liftDir_ vector.

[RodriguezFatz]

Angelo please try:

p
    {
    solver           GAMG;
        tolerance        1e-12;
        relTol           0.1;
        smoother         DICGaussSeidel;
        nPreSweeps       0;
        nPostSweeps      1;
    nFinestSweeps    2;
    scaleCorrection  true;
    directSolveCoarsestLevel false;
        cacheAgglomeration on;
        agglomerator     faceAreaPair;
        nCellsInCoarsestLevel 500;
        mergeLevels      1;
        maxIter         100;
    }

and for all others:

"(U|k|omega)"
{
        solver           smoothSolver;
    preconditioner   DILU;
        smoother         DILUGaussSeidel;
        tolerance        1e-12;
        relTol           0.1;
        nSweeps          1;
        maxIter         100;
    }

and post the log output.

[RodriguezFatz]

Also one very clever person in this forum wrote you should never limit the pressure gradient.

[alexeym]

In fact it was here: http://www.openfoam.org/mantisbt/view.php?id=1410#c3246

[RodriguezFatz]

Right there, henry... very clever.