[sErik]

Hi Foamers,

I have a problem with simpleFoam. Every time I try to run the solver, I recieve this error

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;
}


Starting time loop

Time = 1

DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.00241826, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.00193225, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.00242562, No Iterations 1
DICPCG: Solving for p, Initial residual = 1, Final residual = 0.00979073, No Iterations 399
DICPCG: Solving for p, Initial residual = 0.308751, Final residual = 0.0029273, No Iterations 12
time step continuity errors : sum local = 7.89254, global = -1.95354, cumulative = -1.95354
#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/opt/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib/libc.so.6"
#3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/opt/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#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&) in "/opt/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#5 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam:perator/<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<doub le, Foam::fvPatchField, Foam::volMesh> > const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/opt/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#6 Foam::incompressible::RASModels::kEpsilon::correct () in "/opt/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#7 main in "/opt/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64GccDPOpt/simpleFoam"
#8 __libc_start_main in "/lib/libc.so.6"
#9 _start at /usr/src/packages/BUILD/glibc-2.9/csu/../sysdeps/x86_64/elf/start.S:116

The weird thing is, that I've already managed to get it running. But after a system crash, all the result were deleted. Now I want to rerun the solver, but without success.
This is fvSchemes

ddtSchemes
{
default steadyState;
}

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

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(grad(U).T()))) 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(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 corrected;
}

This here fvSolutions

p
{
solver PCG;
preconditioner DIC;
tolerance 1e-06;
relTol 0.01;
}

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;
}

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

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

SIMPLE
{
nNonOrthogonalCorrectors 1;
}

relaxationFactors
{
p 0.3;
U 0.7;
k 0.7;
epsilon 0.7;
R 0.7;
nuTilda 0.7;
}

[ngj]

Hi Erik

The error is due to the fact that you have specified 0 as boundary conditions/internal field for k and/or epsilon (errro #3 and #6 tells the story). Your need to specify finite values, however to remember when setting them that they need to be chosen such that the eddy viscosity is not initialized with some large value.

Bests,

Niels

[sErik]

Hi Niels,

thanks a lot! Now it's running. I've set k=0,375 and epsilon=14.855.

Best regards,
Erik

[sErik]

Hi Foamers,

I still have trouble with my simulation. bounding epsilon is exploding and huge right from the start!
It's about a pipe flow with a starting pressure of 7638Pa and a inlet velocity of 1.7448 m/s. I'm interessted in the drop of pressure an the end of the curved pipe.

...
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 kEpsilon
kEpsilonCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
sigmaEps 1.3;
}
Starting time loop

Time = 0.001

DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.0959227, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.0562844, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.095863, No Iterations 1
GAMG: Solving for p, Initial residual = 1, Final residual = 0.00703477, No Iterations 4
GAMG: Solving for p, Initial residual = 0.23568, Final residual = 0.00179757, No Iterations 3
time step continuity errors : sum local = 0.00216907, global = -0.000147145, cumulative = -0.000147145
DILUPBiCG: Solving for epsilon, Initial residual = 0.994795, Final residual = 0.0275726, No Iterations 2
bounding epsilon, min: -82.1271 max: 5.59944e+06 average: 495.63
DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 0.000932489, No Iterations 1
ExecutionTime = 13 s ClockTime = 26 s

Time = 0.002

DILUPBiCG: Solving for Ux, Initial residual = 0.553916, Final residual = 0.0316065, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.760731, Final residual = 0.0524181, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.649458, Final residual = 0.0508126, No Iterations 1
GAMG: Solving for p, Initial residual = 0.965877, Final residual = 0.00695088, No Iterations 7
GAMG: Solving for p, Initial residual = 0.284313, Final residual = 0.00135296, No Iterations 3
time step continuity errors : sum local = 0.00278298, global = -0.000389391, cumulative = -0.000536535
DILUPBiCG: Solving for epsilon, Initial residual = 0.944274, Final residual = 0.0104053, No Iterations 2
DILUPBiCG: Solving for k, Initial residual = 0.984862, Final residual = 0.0866853, No Iterations 1
ExecutionTime = 22.05 s ClockTime = 44 s

Time = 0.003

DILUPBiCG: Solving for Ux, Initial residual = 0.2867, Final residual = 0.0118204, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.613741, Final residual = 0.0435605, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.610194, Final residual = 0.0566501, No Iterations 1
GAMG: Solving for p, Initial residual = 0.849475, Final residual = 0.00591298, No Iterations 7
GAMG: Solving for p, Initial residual = 0.408281, Final residual = 0.0022316, No Iterations 3
time step continuity errors : sum local = 0.00442252, global = -0.000694598, cumulative = -0.00123113
DILUPBiCG: Solving for epsilon, Initial residual = 0.0269077, Final residual = 0.00258516, No Iterations 1
bounding epsilon, min: -636276 max: 1.63604e+10 average: 633200
DILUPBiCG: Solving for k, Initial residual = 0.480218, Final residual = 0.0114333, No Iterations 2
ExecutionTime = 31.11 s ClockTime = 62 s
...

I don't know what to do anymore - I've tried a lot of different settings.
These are my settings:
k

internalField uniform 0.375;

boundaryField
{
Inlet
{
type fixedValue;
value uniform 0.375;
}
Outlet
{
type zeroGradient;
}
Leitung_11
{
type kqRWallFunction;
value $internalField;
}
...

epsilon

internalField uniform 14.855;

boundaryField
Inlet
{
type fixedValue;
value uniform 14.855;
}
Outlet
{
type zeroGradient;
}
Leitung_11
{
type epsilonWallFunction;
value $internalField;
}...

U

internalField uniform (0 0 0);

boundaryField
{
Inlet
{
type fixedValue;
value uniform (1.7466 0 0);
}

Outlet
{
type zeroGradient;
}
Leitung_11
{
type zeroGradient;
value $internalField;
}

p

internalField uniform 0;

boundaryField
{
Inlet
{
type fixedValue;
value uniform 7638;
}

Outlet
{
type zeroGradient;
}
Leitung_11
{
type zeroGradient;
} ...

nut

internalField uniform 0;

boundaryField
{
Inlet
{
type calculated;
value uniform 0;
}
Outlet
{
type calculated;
value uniform 0;
}

Leitung_11
{
type nutWallFunction;
value uniform 0;
}...

nuTilda

internalField uniform 0;

boundaryField
{
Inlet
{
type fixedValue;
value uniform 0;
}
Outlet
{
type fixedValue;
value uniform 0;
}

Leitung_11
{
type zeroGradient;
value $internalField;
}...

R

internalField uniform (0 0 0 0 0 0);

boundaryField
{
Inlet
{
type fixedValue;
value uniform (0 0 0 0 0 0);
}

Outlet
{
type zeroGradient;
}

Leitung_11
{
type kqRWallFunction;
}
...

boundary

26
(
Inlet
{
type patch;
nFaces 328;
startFace 3575458;
}
Outlet
{
type patch;
nFaces 502;
startFace 3575786;
}
Leitung_11
{
type wall;
nFaces 16315;
startFace 3576288;
}...

Sorry for the long post!

[maddalena]

Hi,
I think your problem is connected with the boundary conditions: you are imposing a fixed value for p and U at the inlet and none at the outlet. You should use:

• inlet: U fixed Value, p zero Gradient;
• outlet: U zero Gradient, p fixed value.

hope this help. Cheers,
maddalena

[sErik]

I'll try it right now, but I don't understand it realy.
I have a pressure of 7638Pa and a velocity of 1,7448 m/s at the inlet, both values are fixed. How should I enter fixed value for p (or U) at the outlet, although this is what I'm interesseted in?