[Tobi]

Dear all,

I am facing a problem that I could not resolve till now. To my problem: I build a new boundary condition (Robin BC based on the mixedFvPatchField class; the library can be downloaded and used from my bitbucket account: https://bitbucket.org/shor-ty/laserconvectionbc/). However, the library is working fine in my Ph.D. solver as well as for the basic laplacianFoam solver. Trying to use the boundary within the heat-transfer solver lead to the following symbol lookup error:

buoyantPimpleFoam: symbol lookup error:  /home/shor-ty/OpenFOAM/shor-ty-dev/platforms/linux64GccDPInt32Opt/lib/liblaserConvectionBC.so:  undefined symbol:  _ZN4Foam27laserConvectionFvPatchFieldIdEC1ERKNS_7fvPatchERKNS_16DimensionedFieldIdNS_7volMeshEEERKNS_10dictionaryE

Normally, I guess that this error indicates a missing library. However, even if I use the debug compiled FOAM version, I cannot get more information out of the problem and I could not find any library that is missing to resolve this issue.

Any hint is highly appreciated.
Thanks in advance,


Edit: I figured out that it is not working with laplacianFoam either, so finally I got the error always (only if I compile it direct with my solver); ... (confused)

[deepsterblue]

c++filt on your symbol gives me this:

c++filt _ZN4Foam27laserConvectionFvPatchFieldIdEC1ERKNS_7fvPatchERKNS_16DimensionedFieldIdNS_7volMeshEEERKNS_10dictionaryE

Foam::laserConvectionFvPatchField<double>::laserConvectionFvPatchField(Foam::fvPatch const&, Foam::DimensionedField<double, Foam::volMesh> const&, Foam::dictionary const&)

Do you have this constructor implemented in your source file?

[Tobi]

Hi,

yes I have this constructor implemented:

template<class Type>
Foam::laserConvectionFvPatchField<Type>::laserConvectionFvPatchField
(
    const fvPatch& p,
    const DimensionedField<Type, volMesh>& iF,
    const dictionary& dict
)
:

[deepsterblue]

Alright... And has it been instantiated for 'double'? You need to have this line defined somewhere:

makePatchFields(laserConvection)

[Tobi]

Thanks for your reply. For sure I have this line. You can check the stuff here: https://bitbucket.org/shor-ty/laserconvectionbc/src and try it yourself. The class is a template class.

[Tobi]

I just want to mention that the boundary condition works fine if we compile it within the solver. However, the standalone library would be much better. Any hint is appreciated. Thanks in advance.

[deepsterblue]

Why are these lines commented out:

#ifdef NoRepository
#   include "laserConvectionFvPatchField.C"
#endif

That's the line which includes all your template code. When I uncomment it, it compiles fine, and the output of

nm liblaserConvectionBC.so | c++filt

yields weak symbols instead of undefined. I haven't tried including your library in a solver. Perhaps you could try it and let me know.

PS. You probably want to replace std::to_string (C++11 only) with Foam::name if you want portability.

[Tobi]

Hi,

thanks for the remark. I comment this lines because I got a previous declared here error. However, I realized that at the beginning I was compiling the wrong *.C file. Thats why this commented lines still were in the code. Now it is fine after uncommenting the lines again and checking everything again.

By the way I was also trying to uncomment the lines. It was not working. I forgot to wclean it.

Thank you very much.

[gu1]

I apologize for opening the thread again, but I had a similar error. My library compiles normally, but when I start the simulation... the solver has the same error as described above. Could you help me?

turbulentFoam: symbol lookup error: turbulentFoam: undefined symbol: _ZN4Foam17turbulentModelC1ERKNS_14GeometricFieldIN S_6VectorIdEENS_12fvPatchFieldENS_7volMeshEEERKNS1 _IdNS_13fvsPatchFieldENS_11surfaceMeshEEE

.C:
Foam::turbulentModel::turbulentModel
(
const volVectorField& U,
const surfaceScalarField& phi,
const dictionary& dict
)
:
IOdictionary
(
IOobject
(
"turbulentProperties",
U.time().constant(),
U.db(),
IOobject::MUST_READ,
IOobject::NO_WRITE
)
),
rho_(dict.lookup("rho")),
tau_(dict.lookup("tau")),
lawPtr_(turbulentLaw::New(word::null, U, phi, subDict("Stress")))

.H:

class turbulentModel
:
public IOdictionary
{
dimensionedScalar rho_;

dimensionedScalar tau_;

public:

TypeName("turbulentModel");

// Constructors:
turbulentModel
(
const volVectorField& U,
const surfaceScalarField& phi,
const dictionary& dict
);