[Jost K]

Hi all,

I am using waves2Foam with OpenFOAM-v2412.
I just wanted to share some tweaks I found here.
Maybe they can find their way into future releases of this wonderful toolbox.

I encountered a compilation error in the sampling utility:

surfaceElevation/sampledSurfaceElevation.C: In member function 'voidFoam::sampledSurfaceElevation::gatherAllSets()':
surfaceElevation/sampledSurfaceElevation.C:169:35: error: no matching function for call to 'Foam::globalIndex::reset(Foam::label, Foam::globalIndex::gatherOnly)'
  169 |         globalIndices_[seti].reset(coords.size(), globalIndex::gatherOnly{});

Apparently line 169 in the file src/waves2FoamSampling2206/surfaceElevation/sampledSurfaceElevation.C needs to be:

globalIndices_[seti].reset(globalIndex::gatherOnly{}, coords.size());

...instead of:

globalIndices_[seti].reset(coords.size(), globalIndex::gatherOnly{});

...for newer FOAM versions.
I have not checked since what version exactly.
This fixes the error for me.

Hope this helps others with the same problem.

Cheers,
Jost

[Jost K]

I have implemented the autoMap and rmap functions in the GABCs.
Those are needed when the GABCs are used with adaptive mesh refinement.
(I guess also with overset?)


My suggestion would be to put the following code in src/waves2FoamGABC/fvPatchFields/basic/robinV/robinVFvPatchField.C

template<class Type>
void Foam::robinVFvPatchField<Type>::autoMap
(
    const fvPatchFieldMapper& m
)
{
    fvPatchField<Type>::autoMap(m);
    
    sourceValue_.autoMap(m);
    fixedCoeffs_.autoMap(m);
    gradCoeffs_.autoMap(m);
}

template<class Type>
void Foam::robinVFvPatchField<Type>::rmap
(
    const fvPatchField<Type>& ptf,
    const labelList& addr
)
{
    fvPatchField<Type>::rmap(ptf, addr);
    
    const robinVFvPatchField<Type>& mptf =
        refCast<const robinVFvPatchField<Type>>(ptf);

    sourceValue_.rmap(mptf.sourceValue_, addr);
    fixedCoeffs_.rmap(mptf.fixedCoeffs_, addr);
    gradCoeffs_.rmap(mptf.gradCoeffs_, addr);
}

...and in src/waves2FoamGABC/fvPatchFields/basic/robinV/robinVFvPatchField.H:

        // Mapping functions

            //- Map (and resize as needed) from self given a mapping object
            virtual void autoMap
            (
                const fvPatchFieldMapper&
            );

            //- Reverse map the given fvPatchField onto this fvPatchField
            virtual void rmap
            (
                const fvPatchField<Type>&,
                const labelList&
            );

... and change the definitions in src/waves2FoamGABC/fvPatchFields/derived/gabcPressureRobinV/gabcPressureRobinVFvPatchScalarField.C to:

void gabcPressureRobinVFvPatchScalarField::autoMap
(
    const fvPatchFieldMapper& m
)
{
   robinVFvPatchField<scalar>::autoMap(m);
}


void gabcPressureRobinVFvPatchScalarField::rmap
(
    const fvPatchField<scalar>& ptf,
    const labelList& addr
)
{
   robinVFvPatchField<scalar>::rmap(ptf, addr);
}

I have only tested this with OpenFOAM-v2412.
Hope it will be useful.

Cheers,
Jost

[wlzr]

Hi Jost K,

I'm implementing overset functionality into waveFoam by referencing overInterDyMFoam's approach. After incorporating the differences between interFoam and waveFoam, the solver compiled successfully and worked with some test cases. However, I recently encountered a runtime error when running a specific case:
```
--> FOAM FATAL ERROR: (openfoam-2206)
unallocated autoPtr of type N4Foam22celerityShapeFunctionsE

From T* Foam::autoPtr<T>:perator->() [with T = Foam::celerityShapeFunctions]
in file /home/foam/OpenFOAM/OpenFOAM-v2206/src/OpenFOAM/lnInclude/autoPtrI.H at line 178.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::error::simpleExit(int, bool) at ??:?
#2 Foam::error::exiting(int, bool) at ??:?
#3 Foam::gabcPressureRobinVFvPatchScalarField::update Coeffs() at ??:?
#4 Foam::fvMatrix<double>::fvMatrix(Foam::GeometricFi eld<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::dimensionSet const&) in ~/OpenFOAM/foam-v2206/platforms/linux64GccDPInt32Opt/bin/overWaveDyM2Foam
#5 Foam::fv::gaussLaplacianScheme<double, double>::fvmLaplacianUncorrected(Foam::GeometricFi eld<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
#6 Foam::fv::gaussLaplacianScheme<double, double>::fvmLaplacian(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
#7 Foam::tmp<Foam::fvMatrix<double> > Foam::fvm::laplacian<double, double>(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in ~/OpenFOAM/foam-v2206/platforms/linux64GccDPInt32Opt/bin/overWaveDyM2Foam
#8 main in ~/OpenFOAM/foam-v2206/platforms/linux64GccDPInt32Opt/bin/overWaveDyM2Foam
#9 __libc_start_main in /lib/x86_64-linux-gnu/libc.so.6
#10 ? in ~/OpenFOAM/foam-v2206/platforms/linux64GccDPInt32Opt/bin/overWaveDyM2Foam
*** Process received signal ***
Signal: Aborted (6)
Signal code: (-6)
[ 0] /lib/x86_64-linux-gnu/libpthread.so.0(+0x14420)[0x7ff3c4a78420]
[ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0xcb)[0x7ff3c48b300b]
[ 2] /lib/x86_64-linux-gnu/libc.so.6(abort+0x12b)[0x7ff3c4892859]
[ 3] /home/foam/OpenFOAM/OpenFOAM-v2206/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZN4Foam5error10simpleExitEib+0x17a )[0x7ff3c51e2baa]
[ 4] /home/foam/OpenFOAM/OpenFOAM-v2206/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZN4Foam5error7exitingEib+0x4a)[0x7ff3c51e617a]
[ 5] /home/foam/OpenFOAM/foam-v2206/platforms/linux64GccDPInt32Opt/lib/libwaves2FoamGABC.so(_ZN4Foam36gabcPressureRobinVF vPatchScalarField12updateCoeffsEv+0x1367)[0x7ff3c5e442c7]
[ 6] overWaveDyM2Foam(_ZN4Foam8fvMatrixIdEC1ERKNS_14Geo metricFieldIdNS_12fvPatchFieldENS_7volMeshEEERKNS_ 12dimensionSetE+0x3d1)[0x55f0de50bfe1]
[ 7] /home/foam/OpenFOAM/OpenFOAM-v2206/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so(_ZN4Foam2fv20gaussLaplacianSche meIddE23fvmLaplacianUncorrectedERKNS_14GeometricFi eldIdNS_13fvsPatchFieldENS_11surfaceMeshEEES8_RKNS 3_IdNS_12fvPatchFieldENS_7volMeshEEE+0x98)[0x7ff3c91b5ba8]
[ 8] /home/foam/OpenFOAM/OpenFOAM-v2206/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so(_ZN4Foam2fv20gaussLaplacianSche meIddE12fvmLaplacianERKNS_14GeometricFieldIdNS_13f vsPatchFieldENS_11surfaceMeshEEERKNS3_IdNS_12fvPat chFieldENS_7volMeshEEE+0xa7)[0x7ff3c91abbc7]
[ 9] overWaveDyM2Foam(_ZN4Foam3fvm9laplacianIddEENS_3tm pINS_8fvMatrixIT_EEEERKNS_14GeometricFieldIT0_NS_1 3fvsPatchFieldENS_11surfaceMeshEEERKNS7_IS4_NS_12f vPatchFieldENS_7volMeshEEE+0x24e)[0x55f0de522ffe]
[10] overWaveDyM2Foam(main+0x9c5c)[0x55f0de4c155c]
[11] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xf3)[0x7ff3c4894083]
[12] overWaveDyM2Foam(+0x6642e)[0x55f0de4cb42e]
*** End of error message ***
```
The error seems GABC-related - when replacing GABC boundaries with relaxation zones, the case runs normally.The error persists even after recompiling with proper overset code integration.Do you have any thoughts on this phenomenon?Thank you for any insights!

[Jost K]

Hi wlzr,

I do not see a direct link between your error message and the autoMap and rmap functions but I guess it could still very well be related.
You can check your log file for the lines "AUTOMAP NOT CODED!" or "RMAP NOT CODED!". If you find one of them, you should probably try implementing the functions.
Please let us know if you see any progress.

Cheers,
Jost

[Shuo_Yuan]

Hello, may I ask which version of waves2foam you are using? My OpenFOAM version is also 2412, and my waves2foam is r2157. I modified the code according to your instructions, but the compilation still fails.

[Jost K]

Originally Posted by Shuo_Yuan

Hello, may I ask which version of waves2foam you are using? My OpenFOAM version is also 2412, and my waves2foam is r2157. I modified the code according to your instructions, but the compilation still fails.

Hi,

I am also on r2157.
Do you want to share your error message?
Please let us know once you have fixed it.

Cheers,
Jost

[Shuo_Yuan]

Originally Posted by Jost K

Hi,

I am also on r2157.
Do you want to share your error message?
Please let us know once you have fixed it.

Cheers,
Jost

I encountered over twenty compilation errors, and they are basically of the same type. My approach was to modify the source code where the errors were reported. For example, I changed `scalarField coorT = (cf & proj)` to `scalarField coorT = scalarField(cf & proj)`.
However, I feel this doesn't seem to work because more errors of the same type appear after the modification. I'm a bit stuck on how to proceed.

fvPatchFields/basic/robinV/robinVFvPatchField.C:368:27: error: conversion from 'tmp<scalarField>' (aka 'tmp<Field<double>>') to 'const scalarField' (aka 'const Field<double>') is ambiguous
368 | const scalarField r = sourceValue_.component(cmpt);
| ^ ~~~~~~~~~~~~~~~~~~~~~~~~~~~~
/Volumes/OpenFOAM-v2412/src/OpenFOAM/lnInclude/tmp.H:320:9: note: candidate function
320 | operator const T&() const { return cref(); }
| ^
/Volumes/OpenFOAM-v2412/src/OpenFOAM/lnInclude/FieldI.H:133:27: note: candidate constructor
133 | inline Foam::Field<Type>::Field(const tmp<Field<Type>>& tfld)
| ^

[Jost K]

Since I did not have any of that, I am wondering whether you are possibly using an incompatible compiler version. I am on GCC 13.3.0. I do not think there is Information available on the compiler compatibility of waves2Foam, but new versions might be stricter in enforcing things like the error you posted. So if you are on a newer compiler version, you might see an error where I just got a warning (of which there were plenty).