Closed ananddoss2004 closed 2 years ago
Greetings @ananddoss2004,
The two errors that I can see from the stacktrace are the following:
ZN4Foam6sigFpe13sigFpeHandlerEi -> sigFpe
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
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
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
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
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
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
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:\PROGRA~1\BLUECF~1\ThirdParty-5.x\platforms\mingw_w64GccDPInt32\lib\libstack_trace.dll ZN4Foam5error10printStackERNS_7OstreamE [0x11e1c88+0x218] module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\lib\libOpenFOAM.dll ZN4Foam6sigFpe13sigFpeHandlerEi [0x11e2af3+0x33] module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\lib\libOpenFOAM.dll (No symbol) [0x40684d] module: C:\PROGRA~1\BLUECF~1\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 ZN4FoamdvERKNS5UListIdEES3 [0x11894f5+0x75] module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\lib\libOpenFOAM.dll (No symbol) [0x401dba] module: C:\PROGRA~1\BLUECF~1\OpenFOAM-5.x\platforms\mingw_w64GccDPInt32Opt\bin\chtMultiRegionFoam.exe (No symbol) [0x48de41] 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