problem with wallFunctions (kEpsilon model)
 

Hi everybody,

I was trying to simulate the flow around a wing by means of RANS model in OpenFOAM. The wallfunctions I'm trying to use for the kEpsilon gives me the following error:

-----------------------------
gradientInternalCoeffs cannot be called for a genericFvPatchField (actual type kqRwallFunction)
on patch rear_wing of field k in file "/home/openfoam/Desktop/dinoOF/OFcase/3wing_SIMPLE/0/k"
You are probably trying to solve for a field with a generic boundary condition.

From function genericFvPatchField<Type>::gradientInternalCoeffs( ) const
in file fields/fvPatchFields/basic/generic/genericFvPatchField.C at line 782.
----------------------------

I compared my testcase with some tutorials and they seems to be similar, so I cannot understand where is the problem?!??

thanks in advance

dino

Do you use a selfmade BC on the specific patch? I once got the same error message, which was easily fixed by specifying a "value uniform 0" entry, e.g.
even though the boundary condition itself wouldn't need it.

//Tammo

actually I'm using an already implemented BC, i.e. kqRwallFunction.
In the "k" file I'm using these settings for all the walls:

rear_wing
{
type kqRwallFunction;
value uniform 0.00735;
}

main_wing
{
type kqRwallFunction;
value uniform 0.00735;
}

front_wing
{
type kqRwallFunction;
value uniform 0.00735;
}

The strange thing is that if I change only for the first one (rear_wing) the value uniform from 0.00735 to 0 I get the following error:

---------------
smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 0.0187915, No Iterations 2
smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 0.0186828, No Iterations 2
GAMG: Solving for p, Initial residual = 1, Final residual = 0.00799459, No Iterations 14
time step continuity errors : sum local = 8.85047e-07, global = 2.32762e-08, cumulative = 2.32762e-08
#0 Foam::error::printStack(Foam::Ostream&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6.x/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 "/home/openfoam/OpenFOAM/OpenFOAM-1.6.x/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 "/home/openfoam/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#5 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::operator/<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<doub le, Foam::fvPatchField, Foam::volMesh> > const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/home/openfoam/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#6 Foam::incompressible::RASModels::kEpsilon::correct () in "/home/openfoam/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#7 main in "/home/openfoam/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/simpleFoam"
#8 __libc_start_main in "/lib/libc.so.6"
#9 _start at /build/buildd/eglibc-2.10.1/csu/../sysdeps/x86_64/elf/start.S:116
Floating point exception
---------------------
and it remains also in the case i change the value for the other walls!!!
what could be the reason??

thanks for the fast reply

dino

Hi,

the error message tells you that you divide by zero somewhere, more specifically it is due to your setting at the rear_wing where you've set uniform 0

If you want a zero value there, just put a small non-zero value like 1e-10 to avoid division by zero there.

Best,
Florian

Hi,

do you use a solver for compressible flow?

I think I already had the same error. For compressible calculations using rhoSimpleFoam "kqRWallFunction" should be replaced by "compressible::kqRWallFunction". Same for omega, so I think also for epsilon in your case.

Just a guess.

Regards

for Florian:
if I set a very small value 1e-10, I get again the previous error (that I wrote in my first message).

for cboss:
it's an incompressible solver, SimpleFoam.

I read in similar threads that the problem could be that the needed library is not loaded but comparing with another testcase that works I cannot see significative difference. If somebody wants to have a look I can upload the testcase on fileshare website.

thanks to all for your availability

dino

Perhaps just a spelling error. According to your post you use "kqRwallFunction". Should be "kqRWallFunction". This produces the same error on my system.

Regards

thanks cboss, you're right!
that's exactly the kind of error I never realize!!
now it works great

thanks to all

I have the same problem when using twophaseEulerFoam,

gradientInternalCoeffs cannot be called for a genericFvPatchField (actual type epsilonWallFunction) on patch wall of field epsilon in file "/home/dft/OpenFOAM/dft-1.6/run/sg/0/epsilon" You are probably trying to solve for a field with a generic boundary condition.

please help me !

Can you post your epsilon field?

my epsilon field is as follows:
dimensions [ 0 2 -3 0 0 0 0 ];

internalField uniform 0.05;

referenceLevel 0;

boundaryField
{
inlet
{
type fixedValue;
value uniform 0.05;
}

wall
{
type epsilonWallFunction;
value uniform 0.001;
}

outlet
{
type zeroGradient;
}

}
Is there any problem?

thanks

In my fields for epsilon I have the following for the wall :

wall
{

type epsilonWallFunction;
Cmu 0.09;
kappa 0.41;
E 9.8;
value uniform 0.0067;

}

you have to specify the 3 constants,

hope this helps,

Marine

I reset the epsilon file, but it does not work. When i use the simpleFoam to caculate single phase flow, the wallfunction goes well. But in the simulation of two phase fow applying the twophaseeulerfoam , it displays the error.