[saralen]

Hi all,


I've just compiled a solver with OF7 without problems, but, when I run the case I have the following error:


--> FOAM FATAL ERROR:
Attempt to cast type calculated to type nutWallFunction

From function To& Foam::refCast(From&) [with To = const Foam::nutWallFunctionFvPatchScalarField; From = const Foam::fvPatchField<double>]
in file /home/ubuntu/OpenFOAM/OpenFOAM-7/src/OpenFOAM/lnInclude/typeInfo.H at line 114.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 Foam::nutWallFunctionFvPatchScalarField::nutw(Foam ::turbulenceModel const&, int) at ??:?
#3 Foam::incompressible::alphatJayatillekeWallFunctio nFvPatchScalarField::updateCoeffs() at ??:?
#4 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::Boundary::evaluate() in "/home/sara/OpenFOAM/sara-7/platforms/linux64GccDPInt32Opt/bin/convectiveFoamInf"
#5 ? in "/home/sara/OpenFOAM/sara-7/platforms/linux64GccDPInt32Opt/bin/convectiveFoamInf"
#6 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7 ? in "/home/sara/OpenFOAM/sara-7/platforms/linux64GccDPInt32Opt/bin/convectiveFoamInf"
Aborted (core dumped)



I've already check online and suggestions about blockMesh problems seem not appropriate in this case. I think my nut file is ok.


this is my nut:


\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 2 -1 0 0 0 0];

internalField uniform 0;

boundaryField
{
floor
{
type nutkWallFunction;
value uniform 0;
}
ceiling
{
type nutkWallFunction;
value uniform 0;
}
fixedWalls
{
type nutkWallFunction;
value uniform 0;
}
emptyWalls
{
type empty;
value uniform 0;
}
}


// ************************************************** *********************** //





and this is my blockMeshdict




\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1;

vertices
(
(0 0 0)
(1 0 0)
(1 0.001 0)
(0 0.001 0)
(0 0 1)
(1 0 1)
(1 0.001 1)
(0 0.001 1)
);

blocks
(
hex (0 1 2 3 4 5 6 7) (128 1 128) simpleGrading (1 1 1)
);

edges
(
);


boundary
(
floor
{
type wall;
faces
(
(0 3 2 1)
);
}
ceiling
{
type wall;
faces
(
(4 5 6 7)
);
}
fixedWalls
{
type wall;
faces
(
(0 4 7 3)
(2 6 5 1)
);
}
emptyWalls
{
type empty;
faces
(
(4 0 1 5)
(7 6 2 3)
);
}


);

mergePatchPairs
(
);



Ps: the same case worked well on OF5. Passing from OF5 to OF7 I just modified a litte the solver and I don't have any problem in compling it.

Is maybe the problem due to a wrong path to access libraries?



Any suggestions?

I hope to have been clear!
Thanks,

Sara

[Constructor]

Hello, Sara.

I personally entered this error when running with low-Re k-omega SST in OF7. Did not find a reason.
Follow this.

[foamyva]

Same problem here, curious if anybody found a solution!

[mAlletto]

The Problem seems to come Frome the alphat wall function rather than the nut wall function. It comes when the function evaluatecoeff is called. See https://github.com/OpenFOAM/OpenFOAM...hScalarField.C

[jherb]

I had the same problem, when I (mistakenly) used wall boundary conditions for k and omega on a in- and/or outlet patch.

[Stuntmanbob]

Hey Sara,

i've encountered the same Error using the SST-Turbulence model in OpenFoam 7.

My case is the flow in a rectangle box, where the bottom is a wall and the top symmetry. The side walls got an cyclic bc. The mesh at the bottom should be fine enough for yPlus < 1, so i don't want to use any wallfunctions (apart of omegaWallFunction of course). The solver is rhoSimpleFoam.

According to this thread:
SST SimpleFoam Convergence Problems
i set
k@wall to fixedValue, uniform 0
k@outlet to zeroGradient
omega@wall to omegaWallFunction, uniform 1.0E-8 (small value)
nut@wall to calculated, uniform 0
nut@inlet to calculated, uniform 0
nut@outlet to zeroGradient
and get the same error like sara.


According to mAlletto in this thread i tried different bc for alphat at the wall, but the error still occurs.

Did anyone of you found a solution so far?

I will upload my 0 and system folder, if someone want so search for similarities or differences.

Greetings,
Stuntmanbob

[Bazinga]

FWIW I encounter the same error with OpenFOAM 7 and kOmegaSST. Simulation runs without problems in OpenFOAM 6

[courant_numero_uno]

I had the same problem with v1912. The case was a multi body sixdof simulation, where I guess the solver didn't like the sixdof calculating the motion for the wall function patch. Simulation seems to run fine with v1812.

[keitaro7_14]

Same error. In my case it appears ussing the chtMultiRegionFoam. Also with k-omega SST.

[GeertL]

Originally Posted by keitaro7_14

Same error. In my case it appears ussing the chtMultiRegionFoam. Also with k-omega SST.

I had a similar issue with the 2D airfoil case. However, the following change in the /0/nut file solved it:


old:

walls
{
type fixedValue;
value uniform 0;
}
new:
walls
{
type nutkWallFunction;
value uniform 0;
}



However, I do not know if this has any implications on the results or that in both cases it will be just set to 0 as requested by the uniform 0.

[frantov]

I had the same issue on v1912. It was fixed with boundary conditions and fvSolution solver for omega.

[louisgag]

Originally Posted by jherb

I had the same problem, when I (mistakenly) used wall boundary conditions for k and omega on a in- and/or outlet patch.

thanks, I had a similar issue... omega was somehow mistakenly set to omegaWallFunction on a slip patch and caused the error message.

[bany]

Originally Posted by louisgag

thanks, I had a similar issue... omega was somehow mistakenly set to omegaWallFunction on a slip patch and caused the error message.

When the chemistry is on, the same error occurs.
I cancel the omegaWallFunction BC for 0/nut, and the error disappears.