overPimpleDyMFoam with kOmegaSST segmentation faults in v2406

Summary

kOmegaSST models (and maybe any turbulence model that requires wall-distance) when run with oversetPimpleDyMFoam falls over with a segmentation fault in v2406, despite running OK in v2312. There appears to be some issue with the wall-distance calculation.

Steps to reproduce

Convert the overPimpleDyMFoam/cylinder tutorial to use the kOmegaSST TM and run in v2406.

Example case

Please find case as described attached.

What is the current bug behaviour?

Running with full-debug, reveals it is attempting to access an element in a zero-size list.

What is the expected correct behavior?

No error!

Relevant logs and/or images

On the first full time-step in the example case, the following is output:

Time = 0.005

DICPCG:  Solving for cellDisplacementx, Initial residual = 0, Final residual = 0, No Iterations 0
DICPCG:  Solving for cellDisplacementz, Initial residual = 1, Final residual = 9.83456e-07, No Iterations 25
inverseDistance : detected 2 mesh regions
    zone:0 nCells:7200  voxels:(89 1 89) bb:(-5.00002 -0.0500161 -4.00002) (9.00002 0.0500161 4.0
0002)
    zone:1 nCells:750  voxels:(89 1 89) bb:(-1.19895 -0.0500034 -1.18974) (1.2 0.0500034 1.20974)
Overset analysis : nCells : 7950
    calculated   : 7769
    interpolated : 106 (from local:106  mixed local/remote:0  remote:0)
    hole         : 75



--> FOAM FATAL ERROR: (openfoam-2406)
attempt to access element 0 from zero sized list

    From void Foam::UList<T>::checkIndex(Foam::label) const [with T = int; Foam::label = int]
    in file /home/dludlow/OpenFOAM/OpenFOAM-v2406/src/OpenFOAM/lnInclude/UListI.H at line 200.

FOAM aborting

[stack trace]
=============
#1  Foam::error::simpleExit(int, bool) at ~/OpenFOAM/OpenFOAM-v2406/src/OpenFOAM/lnInclude/error.C:313
#2  Foam::error::exiting(int, bool) at ~/OpenFOAM/OpenFOAM-v2406/src/OpenFOAM/lnInclude/error.C:271
#3  Foam::error::abort() at ~/OpenFOAM/OpenFOAM-v2406/src/OpenFOAM/lnInclude/error.C:375
#4  Foam::Ostream& Foam::operator<< <Foam::error>(Foam::Ostream&, Foam::errorManip<Foam::error>) at ~/OpenFOAM/OpenFOAM-v2406A/src/OpenFOAM/lnInclude/errorManip.H:93 (discriminator 4)
#5  Foam::UList<int>::checkIndex(int) const at ~/OpenFOAM/OpenFOAM-v2406/src/OpenFOAM/lnInclude/UListI.H:202
#6  Foam::UList<int>::operator[](int) const at ~/OpenFOAM/OpenFOAM-v2406/src/OpenFOAM/lnInclude/UListI.H:384
#7  void Foam::oversetFvMeshBase::addInterpolation<double>(Foam::fvMatrix<double>&, Foam::Field<double> const&, bool, double const&) const at ~/OpenFOAM/OpenFOAM-v2406/src/overset/lnInclude/oversetFvMeshBaseTemplates.C:520
#8  Foam::oversetFvPatchField<double>::manipulateMatrix(Foam::fvMatrix<double>&) at ~/OpenFOAM/OpenFOAM-v2406/src/overset/oversetPolyPatch/oversetFvPatchField.C:812
#9  Foam::fvMatrix<double>::boundaryManipulate(Foam::GeometricBoundaryField<double, Foam::fvPatchField, Foam::volMesh>&) at ~/OpenFOAM/OpenFOAM-v2406/src/finiteVolume/lnInclude/fvMatrix.C:1273 (discriminator 2)
#10  Foam::SolverPerformance<double> Foam::oversetFvMeshBase::solveOverset<double>(Foam::fvMatrix<double>&, Foam::dictionary const&) const at ~/OpenFOAM/OpenFOAM-v2406/src/overset/lnInclude/oversetFvMeshBaseTemplates.C:809
#11  Foam::dynamicOversetFvMesh::solve(Foam::fvMatrix<double>&, Foam::dictionary const&) const at ~/OpenFOAM/OpenFOAM-v2406A/src/overset/oversetFvMesh/dynamicOversetFvMesh/dynamicOversetFvMesh.H:169
#12  Foam::fvMatrix<double>::solve(Foam::dictionary const&) at ~/OpenFOAM/OpenFOAM-v2406/src/finiteVolume/lnInclude/fvMatrixSolve.C:331
#13  Foam::fvMatrix<double>::solve() at ~/OpenFOAM/OpenFOAM-v2406/src/finiteVolume/lnInclude/fvMatrixSolve.C:360
#14  Foam::patchDistMethods::advectionDiffusion::correct(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>&) at ~/OpenFOAM/OpenFOAM-v2406/src/finiteVolume/fvMesh/wallDist/patchDistMethods/advectionDiffusion/advectionDiffusionPatchDistMethod.C:199 (discriminator 1)
#15  Foam::patchDistMethods::advectionDiffusion::correct(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&) at ~/OpenFOAM/OpenFOAM-v2406/src/finiteVolume/fvMesh/wallDist/patchDistMethods/advectionDiffusion/advectionDiffusionPatchDistMethod.C:91
#16  Foam::wallDist::movePoints() at ~/OpenFOAM/OpenFOAM-v2406/src/finiteVolume/fvMesh/wallDist/wallDist/wallDist.C:216
#17  void Foam::meshObject::movePoints<Foam::fvMesh>(Foam::objectRegistry&) at ~/OpenFOAM/OpenFOAM-v2406/src/OpenFOAM/lnInclude/MeshObject.C:260
#18  Foam::fvMesh::movePoints(Foam::Field<Foam::Vector<double> > const&) at ~/OpenFOAM/OpenFOAM-v2406/src/finiteVolume/fvMesh/fvMesh.C:998
#19  Foam::dynamicMotionSolverListFvMesh::update() at ~/OpenFOAM/OpenFOAM-v2406/src/dynamicFvMesh/dynamicMotionSolverListFvMesh/dynamicMotionSolverListFvMesh.C:183 (discriminator 6)
#20  Foam::dynamicOversetFvMesh::update() at ~/OpenFOAM/OpenFOAM-v2406/src/overset/oversetFvMesh/dynamicOversetFvMesh/dynamicOversetFvMesh.C:63
#21  ? at ~/OpenFOAM/OpenFOAM-v2406/applications/solvers/incompressible/pimpleFoam/overPimpleDyMFoam/overPimpleDyMFoam.C:100
#22  ? in /lib64/libc.so.6
#23  __libc_start_main in /lib64/libc.so.6
#24  ? in ~/OpenFOAM/OpenFOAM-v2406/platforms/linux64Gcc85DPInt32Debug/bin/overPimpleDyMFoam
=============

In v2312, the iteration completes the yWall solve before the inverse-distance calculation (see LOG below). Note that in v2406 there is no yWall solve at this time-step before the inverseDistance calculation.

Time = 0.005

DICPCG:  Solving for cellDisplacementx, Initial residual = 0, Final residual = 0, No Iterations 0
DICPCG:  Solving for cellDisplacementz, Initial residual = 1, Final residual = 9.83456e-07, No Iterations 25
DILUPBiCGStab:  Solving for yWall, Initial residual = 0.000314587, Final residual = 3.1983e-05, No Iterations 16
inverseDistance : detected 2 mesh regions
    zone:0 nCells:7200  voxels:(89 1 89) bb:(-5.00002 -0.0500161 -4.00002) (9.00002 0.0500161 4.00002)
    zone:1 nCells:750  voxels:(89 1 89) bb:(-1.19895 -0.0500034 -1.18974) (1.2 0.0500034 1.20974)
Overset analysis : nCells : 7950
    calculated   : 7769
    interpolated : 106 (from local:106  mixed local/remote:0  remote:0)
    hole         : 75

PIMPLE: iteration 1
DILUPBiCGStab:  Solving for p, Initial residual = 1, Final residual = 8.3394e-07, No Iterations 113
time step continuity errors : sum local = 9.63552e-10, global = 9.45475e-10, cumulative = 9.45475e-10
DILUPBiCGStab:  Solving for p, Initial residual = 0.020414, Final residual = 9.4636e-07, No Iterations 92
time step continuity errors : sum local = 2.90706e-08, global = -1.88234e-09, cumulative = -9.36862e-10
smoothSolver:  Solving for omega, Initial residual = 0.028511, Final residual = 5.59543e-07, No Iterations 7
smoothSolver:  Solving for k, Initial residual = 1, Final residual = 2.01972e-07, No Iterations 7
ExecutionTime = 0.47 s  ClockTime = 0 s

Environment information

OpenFOAM version : v2406
Operating system : Centos/Rocky
Hardware info :
Compiler : gcc

Possible fixes

The line of code where the error occurs is:

~/OpenFOAM/OpenFOAM-v2406/src/overset/lnInclude/oversetFvMeshBaseTemplates.C:520

and suggests the "stencilPatches_" class member isn't allocated correctly at the time of access. This list needs to be allocated correctly before-hand.

cylinderkOmegaSST2406.gz