ZN10StackTraceC1Ev error

[ananddoss2004]

Hello Experts,

I am getting the following error while running chtMultiRegionFoam. Can anyone help me sort out this error since it is not easily understandable.

ZN10StackTraceC1Ev [0x705c1465+0x25]
module: C:\PROGRA1\BLUECF1\ThirdParty-5.x\platforms\mingw_w64GccDPInt32\lib\libstack_trace.dll
ZN4Foam5error10printStackERNS_7OstreamE [0x11e1c88+0x218]
module: C:\PROGRA1\BLUECF1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\lib\libOpenFOAM.dll
ZN4Foam6sigFpe13sigFpeHandlerEi [0x11e2af3+0x33]
module: C:\PROGRA1\BLUECF1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\lib\libOpenFOAM.dll
(No symbol) [0x40684d]
module: C:\PROGRA1\BLUECF1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\chtMultiRegionFoam.exe
C_specific_handler [0x7ff853207ff8+0x98]
module: C:\WINDOWS\System32\msvcrt.dll
0_chkstk [0x7ff854af00ef+0x11f]
module: C:\WINDOWS\SYSTEM32\ntdll.dll
RtlRaiseException [0x7ff854a9b474+0x434]
module: C:\WINDOWS\SYSTEM32\ntdll.dll
KiUserExceptionDispatcher [0x7ff854aeec1e+0x2e]
module: C:\WINDOWS\SYSTEM32\ntdll.dll
ZN4FoamdvERKNS_5UListIdEES3 [0x11894f5+0x75]
module: C:\PROGRA1\BLUECF1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\lib\libOpenFOAM.dll
(No symbol) [0x401dba]
module: C:\PROGRA1\BLUECF1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\chtMultiRegionFoam.exe
(No symbol) [0x48de41]
module: C:\PROGRA1\BLUECF1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\chtMultiRegionFoam.exe
(No symbol) [0x4013f7]
module: C:\PROGRA1\BLUECF1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\chtMultiRegionFoam.exe
(No symbol) [0x40152b]
module: C:\PROGRA1\BLUECF1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\chtMultiRegionFoam.exe
BaseThreadInitThunk [0x7ff8543b6fd4+0x14]
module: C:\WINDOWS\System32\KERNEL32.DLL
RtlUserThreadStart [0x7ff854a9cec1+0x21]
module: C:\WINDOWS\SYSTEM32\ntdll.dll

[wyldckat]

Greetings @ananddoss2004,

The two errors that I can see from the stacktrace are the following:

1. ZN4Foam6sigFpe13sigFpeHandlerEi -> sigFpe

2. ZN4FoamdvERKNS_5UListIdEES3 -> Foam::UList

The second one seems a bit strange, but the first one indicates a sigFpe, namely "Signal Floating Point Error": https://en.wikipedia.org/wiki/Signal_(IPC)#SIGFPE

In order to get a more accurate indication of what exactly failed, please follow the instructions given here: https://github.com/blueCFD/Core/wiki/Quick-notes-on-how-to-update-build#setting-up-the-work-environment - which will tell you how to activate the X: drive, which will allow the stack tracer to get a more accurate depiction of what went wrong.

The run the solver once again and when it crashes, provide us with the full stack trace once again, including the lines of text that come before that.

Best regards,
Bruno

[ananddoss2004]

Greeting Bruno (wyldckat),

I followed your steps and attaching the full stack trace of the result below.

Build  : 5.x-963176928289
Exec   : C:/PROGRA~1/BLUECF~1/OpenFOAM-5.x/platforms/mingw_w64GccDPInt32Opt/bin/chtMultiRegionFoam.exe
Date   : Aug 10 2020
Time   : 22:36:47
Host   : "DESKTOP-IEFMJCU"
PID    : 6756
I/O    : uncollated
Case   : C:/Openfoam_Models/Meshing/check
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create fluid mesh for region domain0 for time = 0

Create solid mesh for region insideZone for time = 0

*** Reading fluid mesh thermophysical properties for region domain0

    Adding to thermoFluid

Selecting thermodynamics package
{
    type            heRhoThermo;
    mixture         pureMixture;
    transport       const;
    thermo          hConst;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleEnthalpy;
}

    Adding to rhoFluid

    Adding to UFluid

    Adding to phiFluid

    Adding to gFluid

    Adding to hRefFluid

    Adding to ghFluid

    Adding to ghfFluid

    Adding to turbulence

Selecting turbulence model type laminar
Selecting laminar stress model Stokes
Selecting radiationModel none
    Adding to KFluid

    Adding to dpdtFluid
    Adding MRF

No MRF models present

    Adding fvOptions

No finite volume options present

*** Reading solid mesh thermophysical properties for region insideZone

    Adding to thermos

Selecting thermodynamics package
{
    type            heSolidThermo;
    mixture         pureMixture;
    transport       constIso;
    thermo          hConst;
    equationOfState rhoConst;
    specie          specie;
    energy          sensibleEnthalpy;
}

    Adding to radiations

Selecting radiationModel none
    Adding fvOptions

Creating finite volume options from "system/fvOptions"

Selecting finite volume options model type scalarSemiImplicitSource
    Source: heat_Source
    - selecting all cells
    - selected 14396 cell(s) with volume 7.635318
Generating stack trace...


Backtrace:
        0__tcf_0 [0x705c1465+0x35] (stack_trace_win.C:169)
                 module: C:\PROGRA~1\BLUECF~1\ThirdParty-5.x\platforms\mingw_w64GccDPInt32\lib\libstack_trace.dll
        printStack [0x10f1c88+0x218] (printStack.C:96)
                 module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\lib\libOpenFOAM.dll
        sigFpeHandler [0x10f2af3+0x33] (signals\sigFpe.C:79)
                 module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\lib\libOpenFOAM.dll
        _gnu_exception_handler [0x40684d+0xcd] (C:\repo\mingw-w64-crt-git\src\mingw-w64\mingw-w64-crt\crt\crt_handler.c:                                                                                           270)
                 module: C:\PROGRA~1\BLUECF~1\OpenFOAM-.x\platforms\mingw_w64GccDPInt32Opt\bin\chtMultiRegionFoam.exe
        _C_specific_handler [0x7ff853207ff8+0x98]
                 module: C:\WINDOWS\System32\msvcrt.dll
        0_chkstk [0x7ff854af00ef+0x11f]
                 module: C:\WINDOWS\SYSTEM32\ntdll.dll
        RtlRaiseException [0x7ff854a9b474+0x434]
                 module: C:\WINDOWS\SYSTEM32\ntdll.dll
        KiUserExceptionDispatcher [0x7ff854aeec1e+0x2e]
                 module: C:\WINDOWS\SYSTEM32\ntdll.dll
        operator/ [0x10994f5+0x75]
                 module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\lib\libOpenFOAM.dll
        compressibleCourantNo [0x401dba+0xaa] (fluid\compressibleCourantNo.C:41)
                 module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\chtMultiRegionFoam.exe
        0000main [0x48de41+0x6671] (X:\OpenFOAM-5.x\src\OpenFOAM\primitives\Scalar\doubleFloat.H:107)
                 module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\chtMultiRegionFoam.exe
        __tmainCRTStartup [0x4013f7+0x247] (C:\repo\mingw-w64-crt-git\src\mingw-w64\mingw-w64-crt\crt\crtexe.c:343)
                 module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\chtMultiRegionFoam.exe
        mainCRTStartup [0x40152b+0x1b] (C:\repo\mingw-w64-crt-git\src\mingw-w64\mingw-w64-crt\crt\crtexe.c:221)
                 module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\chtMultiRegionFoam.exe
        BaseThreadInitThunk [0x7ff8543b6fd4+0x14]
                 module: C:\WINDOWS\System32\KERNEL32.DLL
        RtlUserThreadStart [0x7ff854a9cec1+0x21]
                 module: C:\WINDOWS\SYSTEM32\ntdll.dll

-attached the original file below.
check.zip

Regards,
Anand

[wyldckat]

Hi Anand,

This gives us a much clearer picture :)
The sigFPE still occurs, now indicating that it occurred due to a division gone wrong:

operator/ [0x10994f5+0x75]
compressibleCourantNo [0x401dba+0xaa] (fluid\compressibleCourantNo.C:41)

Since now we have a specific line where the issue occurs, we can go to the source code... namely line 41 goes wrong here: https://github.com/blueCFD/OpenFOAM-dev/blob/blueCFD-Core-5.x/applications/solvers/heatTransfer/chtMultiRegionFoam/fluid/compressibleCourantNo.C#L37

    scalarField sumPhi
    (
        fvc::surfaceSum(mag(phi))().primitiveField()
      / rho.primitiveField()
    );

So whatever is going on wrong, is because the rho field is zero or infinite.

Based on this information I've looked at the files in the 0 folder and the problem seems to be that you have the p_rgh field set to zero, which is prohibited in this version. Given that there is heat exchange, in OpenFOAM 5 you must use the absolute pressure values (minus the hydrostatic term for the p_rgh field), given that it will calculate the rho based on pressure and temperature, using absolute values.

Best regards,
Bruno

[ananddoss2004]

Hi Bruno,

Although it solve sigFpe error, now i have patch field error that i am posting below.

Build  : 5.x-963176928289
Exec   : C:/PROGRA~1/BLUECF~1/OpenFOAM-5.x/platforms/mingw_w64GccDPInt32Opt/bin/chtMultiRegionFoam.exe
Date   : Aug 11 2020
Time   : 21:40:07
Host   : "DESKTOP-IEFMJCU"
PID    : 10892
I/O    : uncollated
Case   : C:/Openfoam_Models/Meshing/check
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create fluid mesh for region domain0 for time = 0

Create solid mesh for region insideZone for time = 0

*** Reading fluid mesh thermophysical properties for region domain0

    Adding to thermoFluid

Selecting thermodynamics package
{
    type            heRhoThermo;
    mixture         pureMixture;
    transport       const;
    thermo          hConst;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleEnthalpy;
}

    Adding to rhoFluid

    Adding to UFluid

    Adding to phiFluid

    Adding to gFluid

    Adding to hRefFluid

    Adding to ghFluid

    Adding to ghfFluid

    Adding to turbulence

Selecting turbulence model type laminar
Selecting laminar stress model Stokes
Selecting radiationModel none
    Adding to KFluid

    Adding to dpdtFluid

    Adding MRF

No MRF models present

    Adding fvOptions

No finite volume options present

*** Reading solid mesh thermophysical properties for region insideZone

    Adding to thermos

Selecting thermodynamics package
{
    type            heSolidThermo;
    mixture         pureMixture;
    transport       constIso;
    thermo          hConst;
    equationOfState rhoConst;
    specie          specie;
    energy          sensibleEnthalpy;
}

    Adding to radiations

Selecting radiationModel none
    Adding fvOptions

Creating finite volume options from "system/fvOptions"

Selecting finite volume options model type scalarSemiImplicitSource
    Source: heat_Source
    - selecting all cells
    - selected 14396 cell(s) with volume 7.635318
Region: domain0 Courant Number mean: 0.004453225 max: 2.571433
Region: insideZone Diffusion Number mean: 0.00302761 max: 0.0232201
deltaT = 0.05813953
Region: domain0 Courant Number mean: 0.0005178169 max: 0.2990038
Region: insideZone Diffusion Number mean: 0.0003520477 max: 0.002700011
deltaT = 0.05813953
Time = 0.0581395

Pimple iteration 0

Solving for fluid region domain0
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCGStab:  Solving for Ux, Initial residual = 1, Final residual = 9.501474e-009, No Iterations 1
DILUPBiCGStab:  Solving for Uy, Initial residual = 1, Final residual = 8.782644e-009, No Iterations 1
DILUPBiCGStab:  Solving for Uz, Initial residual = 1, Final residual = 2.263775e-008, No Iterations 1


--> FOAM FATAL ERROR:
cannot be called for a calculatedFvPatchField
    on patch room of field h in file "C:/Openfoam_Models/Meshing/check/0/domain0/h"
    You are probably trying to solve for a field with a default boundary condition.

    From function Foam::tmp<Foam::Field<Type> > Foam::calculatedFvPatchField<Type>::gradientInternalCoeffs() const [with                                                                                            Type = double]
    in file fields/fvPatchFields/basic/calculated/calculatedFvPatchField.C at line 187.

FOAM aborting

Generating stack trace...


Backtrace:
        ZN10StackTraceC1Ev [0x705c1465+0x25]
                 module: C:\PROGRA~1\BLUECF~1\ThirdParty-5.x\platforms\mingw_w64GccDPInt32\lib\libstack_trace.dll
        ZN4Foam5error10printStackERNS_7OstreamE [0x1211c88+0x218]
                 module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\lib\libOpenFOAM.dll
        ZN4Foam5error5abortEv [0xfc5b5d+0x12d]
                 module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\lib\libOpenFOAM.dll
        ZNK4Foam22calculatedFvPatchFieldIdE22gradientInternalCoeffsEv [0x66539740+0x100]
                 module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\lib\libfiniteVolume.dll
        ZN4Foam2fv20gaussLaplacianSchemeIddE23fvmLaplacianUncorrectedERKNS_14GeometricFieldIdNS_13fvsPatchFieldENS_11sur                                                                                           faceMeshEEES8_RKNS3_IdNS_12fvPatchFieldENS_7volMeshEEE [0x66254f3a+0x73a]
                 module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\lib\libfiniteVolume.dll
        ZN4Foam2fv20gaussLaplacianSchemeIddE12fvmLaplacianERKNS_14GeometricFieldIdNS_13fvsPatchFieldENS_11surfaceMeshEEE                                                                                           RKNS3_IdNS_12fvPatchFieldENS_7volMeshEEE [0x65f8e48f+0x8f]
                 module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\lib\libfiniteVolume.dll
        ZN4Foam2fv15laplacianSchemeIddE12fvmLaplacianERKNS_14GeometricFieldIdNS_12fvPatchFieldENS_7volMeshEEES8_ [0x661c                                                                                           8085+0x55]
                 module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\lib\libfiniteVolume.dll
        (No symbol) [0x43d59e]
                 module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\chtMultiRegionFoam.exe
        (No symbol) [0x43d3c7]
                 module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\chtMultiRegionFoam.exe
        (No symbol) [0x43d11d]
                 module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\chtMultiRegionFoam.exe
        (No symbol) [0x48f08b]
                 module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\chtMultiRegionFoam.exe
        (No symbol) [0x4013f7]
                 module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\chtMultiRegionFoam.exe
        (No symbol) [0x40152b]
                 module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\chtMultiRegionFoam.exe
        BaseThreadInitThunk [0x7ff8543b6fd4+0x14]
                 module: C:\WINDOWS\System32\KERNEL32.DLL
        RtlUserThreadStart [0x7ff854a9cec1+0x21]
                 module: C:\WINDOWS\SYSTEM32\ntdll.dll

Regards,
Anand Doss

[wyldckat]

Hi Anand,

This actually is fairly verbal:

--> FOAM FATAL ERROR:
cannot be called for a calculatedFvPatchField
on patch room of field h in file "C:/Openfoam_Models/Meshing/check/0/domain0/h"
You are probably trying to solve for a field with a default boundary condition.

The h file in 0/domain0 cannot use the boundary condition calculated. In this specific field, it's an actual boundary that needs a condition, it cannot be merely a value calculated by the solver as a consequence of something like h=p*T.

Best regards,
Bruno

[ananddoss2004]

Hi Bruno,

Problem solved. As you said, my temperature boundary condition is set to calculated. I changed it to fixed value and it solved the problem. Many million thanks for your support. For now, you can close the issue and I wish your support in my future endeavors.

My feedback for you: 5/5.

Regards,
Anand Doss