CFD Online URL
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

simpleFoam error

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 21, 2010, 09:46
Default simpleFoam error
  #1
Member
 
Join Date: Nov 2009
Location: Munich
Posts: 43
Rep Power: 7
sErik is on a distinguished road
Hi Foamers,

I have a problem with simpleFoam. Every time I try to run the solver, I recieve this error
Quote:
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
Quote:
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
Quote:
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;
}
sErik is offline   Reply With Quote

Old   January 21, 2010, 11:06
Default
  #2
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,553
Rep Power: 23
ngj will become famous soon enoughngj will become famous soon enough
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
ngj is offline   Reply With Quote

Old   January 21, 2010, 11:21
Default
  #3
Member
 
Join Date: Nov 2009
Location: Munich
Posts: 43
Rep Power: 7
sErik is on a distinguished road
Hi Niels,

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

Best regards,
Erik
sErik is offline   Reply With Quote

Old   January 25, 2010, 08:41
Default
  #4
Member
 
Join Date: Nov 2009
Location: Munich
Posts: 43
Rep Power: 7
sErik is on a distinguished road
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.
Quote:
...
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
Quote:
internalField uniform 0.375;

boundaryField
{
Inlet
{
type fixedValue;
value uniform 0.375;
}
Outlet
{
type zeroGradient;
}
Leitung_11
{
type kqRWallFunction;
value $internalField;
}
...
epsilon
Quote:
internalField uniform 14.855;

boundaryField
Inlet
{
type fixedValue;
value uniform 14.855;
}
Outlet
{
type zeroGradient;
}
Leitung_11
{
type epsilonWallFunction;
value $internalField;
}...
U
Quote:
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
Quote:
internalField uniform 0;

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

Outlet
{
type zeroGradient;
}
Leitung_11
{
type zeroGradient;
} ...
nut
Quote:
internalField uniform 0;

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

Leitung_11
{
type nutWallFunction;
value uniform 0;
}...
nuTilda
Quote:
internalField uniform 0;

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

Leitung_11
{
type zeroGradient;
value $internalField;
}...
R
Quote:
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
Quote:
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!
sErik is offline   Reply With Quote

Old   January 25, 2010, 08:49
Smile
  #5
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 11
maddalena is on a distinguished road
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
maddalena is offline   Reply With Quote

Old   January 25, 2010, 09:18
Default
  #6
Member
 
Join Date: Nov 2009
Location: Munich
Posts: 43
Rep Power: 7
sErik is on a distinguished road
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?
sErik is offline   Reply With Quote

Reply

Thread Tools
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
Compile problem ivanyao OpenFOAM Running, Solving & CFD 1 October 12, 2012 10:31
Problem with compile the setParabolicInlet ivanyao OpenFOAM Running, Solving & CFD 6 September 5, 2008 21:50
Compiling problems with hello worldC fw407 OpenFOAM Installation 21 January 6, 2008 18:38
DecomposePar links against liblamso0 with OpenMPI jens_klostermann OpenFOAM Bugs 11 June 28, 2007 18:51
user subroutine error CFDUSER CFX 2 December 9, 2006 07:31


All times are GMT -4. The time now is 15:28.