CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   Foam::error::printStack(Foam::Ostream&) with simpleFoam -parallel (http://www.cfd-online.com/Forums/openfoam/85341-foam-error-printstack-foam-ostream-simplefoam-parallel.html)

U.Golling February 23, 2011 12:08

Foam::error::printStack(Foam::Ostream&) with simpleFoam -parallel
 
Hello everybody,

Could someone please help me to understand the reason for the error in my simpleFoam -parallel run:

[8] #0 Foam::error::printStack(Foam::Ostream&) in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
[8] #1 Foam::sigFpe::sigFpeHandler(int) in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
[8] #2 __restore_rt at sigaction.c:0
[8] #3 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::mag<Foam::SymmTensor<double>, Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<Foam ::SymmTensor<double>, Foam::fvPatchField, Foam::volMesh> > const&) in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so"
[8] #4 Foam::incompressible::RASModels::kOmegaSST::kOmega SST(Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&) in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so"
[8] #5 Foam::incompressible::RASModel::adddictionaryConst ructorToTable<Foam::incompressible::RASModels::kOm egaSST>::New(Foam::GeometricField<Foam::Vector<dou ble>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&)[10] #0 Foam::error::printStack(Foam::Ostream&)[4] #0 Foam::error::printStack(Foam::Ostream&) in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so"
[8] #6 Foam::incompressible::RASModel::New(Foam::Geometri cField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&)[9] #0 Foam::error::printStack(Foam::Ostream&)[2] #0 Foam::error::printStack(Foam::Ostream&) in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so"
[8] #7 [5] #0 Foam::error::printStack(Foam::Ostream&)[3] #0 Foam::error::printStack(Foam::Ostream&) in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
.
.
.
[8] #8 __libc_start_main in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so"
.
.
.
[8] #9 in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so".
.
.
.
[compute-0-1:25845] *** Process received signal ***
[compute-0-1:25845] Signal: Floating point exception (8)
[compute-0-1:25845] Signal code: (-6)
[compute-0-1:25845] Failing at address: 0x1fe000064f5
[compute-0-1:25845] [ 0] /lib64/libc.so.6 [0x3bcda302d0]
[compute-0-1:25845] [ 1] /lib64/libc.so.6(gsignal+0x35) [0x3bcda30265]
[compute-0-1:25845] [ 2] /lib64/libc.so.6 [0x3bcda302d0]
[compute-0-1:25845] [ 3] /share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so(_ZN4Foam3magINS_10Sy mmTensorIdEENS_12fvPatchFieldENS_7volMeshEEENS_3tm pINS_14GeometricFieldIdT0_T1_EEEERKNS5_INS6_IT_S7_ S8_EEEE+0x180) [0x2b7cc5f9b010]
[compute-0-1:25845] [ 4] /share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so(_ZN4Foam14incompress ible9RASModels9kOmegaSSTC1ERKNS_14GeometricFieldIN S_6VectorIdEENS_12fvPatchFieldENS_7volMeshEEERKNS3 _IdNS_13fvsPatchFieldENS_11surfaceMeshEEERNS_14tra nsportModelE+0xd55) [0x2b7cc5f90d95]
[compute-0-1:25845] [ 5] /share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so(_ZN4Foam14incompress ible8RASModel31adddictionaryConstructorToTableINS0 _9RASModels9kOmegaSSTEE3NewERKNS_14GeometricFieldI NS_6VectorIdEENS_12fvPatchFieldENS_7volMeshEEERKNS 6_IdNS_13fvsPatchFieldENS_11surfaceMeshEEERNS_14tr ansportModelE+0x47) [0x2b7cc5f9da97]
[compute-0-1:25845] [ 6] /share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so(_ZN4Foam14incompress ible8RASModel3NewERKNS_14GeometricFieldINS_6Vector IdEENS_12fvPatchFieldENS_7volMeshEEERKNS2_IdNS_13f vsPatchFieldENS_11surfaceMeshEEERNS_14transportMod elE+0x1dc) [0x2b7cc5f101fc]
[compute-0-1:25845] [ 7] simpleFoam [0x4141f5]
[compute-0-1:25845] [ 8] /lib64/libc.so.6(__libc_start_main+0xf4) [0x3bcda1d994]
[compute-0-1:25845] [ 9] simpleFoam(_ZNK4Foam11regIOobject11writeObjectENS_ 8IOstream12streamFormatENS1_13versionNumberENS1_15 compressionTypeE+0xb9) [0x4139e9]
[compute-0-1:25845] *** End of error message ***
in "/share/apps/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64GccDPOpt/simpleFoam"
[3] #8 __libc_start_mainmain--------------------------------------------------------------------------
mpiexec noticed that process rank 8 with PID 25845 on node compute-0-1.local exited on signal 8 (Floating point exception).
--------------------------------------------------------------------------

I am just "understanding" some parts of that, but its not enough to find out whats wrong. I don't know what i should change in my files.
So maybe you could explain to me a little bit, what OF wants to explain to me :confused:. (The whole log-file is also attended).
That would be very nice.

Thank you,
Best Regards

Uli

gschaider February 23, 2011 12:26

Quote:

Originally Posted by U.Golling (Post 296584)
Hello everybody,

Could someone please help me to understand the reason for the error in my simpleFoam -parallel run:

<snip>

I am just "understanding" some parts of that, but its not enough to find out whats wrong. I don't know what i should change in my files.
So maybe you could explain to me a little bit, what OF wants to explain to me :confused:. (The whole log-file is also attended).
That would be very nice.

Thank you,
Best Regards

Uli

A bit more information would be nice:
- does this problem also occur when you run the case in serial
- when does it happen (during the construction of the turbulence model, but I deduced that from your stack-trace)
- line numbers would be nice, but you'll need a Debug-version of OF for that

My guess is that this is (again) the old "I set k/epsilon/omega to 0 in the initial conditions (or on a boundary) and the turbulence model divides by it"-problem

Bernhard

U.Golling February 24, 2011 10:21

Hello Bernhard,

here is the context of the error:

Build : 1.6-f802ff2d6c5a
Exec : simpleFoam -parallel
Date : Feb 22 2011
Time : 10:04:18
Host : compute-0-1.local
PID : 25837
Case : /home/mb6484/OpenFOAM/mb6484/Rollbdabs_alt_ganz_3
nProcs : 12
Slaves :
11
(
compute-0-1.local.25838
compute-0-1.local.25839
compute-0-1.local.25840
compute-0-1.local.25841
compute-0-1.local.25842
compute-0-1.local.25843
compute-0-1.local.25844
compute-0-1.local.25845
compute-0-1.local.25846
compute-0-1.local.25847
compute-0-1.local.25848
)

Pstream initialized with:
floatTransfer : 0
nProcsSimpleSum : 0
commsType : nonBlocking
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

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

Create mesh for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting RAS turbulence model kOmegaSST
[8] #0 Foam::error::printStack(Foam::Ostream&) in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
[8] #1 Foam::sigFpe::sigFpeHandler(int)
...

The error occurs in a serial run, too. It also ends with the same error, a floating point exception.

My case is a solar thermal absorber. In principle a system of pipes with Inlet, Outlet and Pipe-wall.
I know about the "old problem k/omaga set to 0". My settings are non-sero (type inletOutlet) at Inlet/Outlet and kqRWallFunction/omegaWallFunction at the wall.

Another theory:
First i worked on my PC with OF 1.7.1 and i had no Problems. But now i have to solve a bigger case. The cluster, i can use, works with OF 1.6. I think i changed all relevant files. Exspecially the turbulenceProperties are to define diverse from OF1.6 to 1.7.!?! All other files seem to look the same!?
But probably i forgot to do change something.

What are other "common" reasons, that invalid floating point numbers can occur?

Thank you.

Uli

gschaider February 24, 2011 13:53

Quote:

Originally Posted by U.Golling (Post 296733)
Hello Bernhard,

here is the context of the error:

Build : 1.6-f802ff2d6c5a
Exec : simpleFoam -parallel
Date : Feb 22 2011
Time : 10:04:18
Host : compute-0-1.local
PID : 25837
Case : /home/mb6484/OpenFOAM/mb6484/Rollbdabs_alt_ganz_3
nProcs : 12
Slaves :
11
(
compute-0-1.local.25838
compute-0-1.local.25839
compute-0-1.local.25840
compute-0-1.local.25841
compute-0-1.local.25842
compute-0-1.local.25843
compute-0-1.local.25844
compute-0-1.local.25845
compute-0-1.local.25846
compute-0-1.local.25847
compute-0-1.local.25848
)

Pstream initialized with:
floatTransfer : 0
nProcsSimpleSum : 0
commsType : nonBlocking
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

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

Create mesh for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting RAS turbulence model kOmegaSST
[8] #0 Foam::error::printStack(Foam::Ostream&) in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
[8] #1 Foam::sigFpe::sigFpeHandler(int)
...

The error occurs in a serial run, too. It also ends with the same error, a floating point exception.

My case is a solar thermal absorber. In principle a system of pipes with Inlet, Outlet and Pipe-wall.
I know about the "old problem k/omaga set to 0". My settings are non-sero (type inletOutlet) at Inlet/Outlet and kqRWallFunction/omegaWallFunction at the wall.

Another theory:
First i worked on my PC with OF 1.7.1 and i had no Problems. But now i have to solve a bigger case. The cluster, i can use, works with OF 1.6. I think i changed all relevant files. Exspecially the turbulenceProperties are to define diverse from OF1.6 to 1.7.!?! All other files seem to look the same!?
But probably i forgot to do change something.

What are other "common" reasons, that invalid floating point numbers can occur?

Thank you.

Uli

OK. If it happens in serial too then please post stack-traces from the serial run
a) then it is sure that it is not a parallel-problem
b) the stack-traces are easier to read

Other common reasons for FPE are when functions are used in a way that doesn't produce a number. Like sqrt(-2), exp(1000000). No idea what could be the problem in your case. Try running the case with a Debug version of OF (http://openfoamwiki.net/index.php/Ho...on_of_OpenFOAM). That way the stack-traces have line-numbers and it will be easy to pinpoint the problem.

About the versions: try running it on your local machine with 1.6 to make sure that you havn't run into some weird compiler-issue

Bernhard

U.Golling March 3, 2011 12:11

Hello,
Sorry for the long time i didn`t answer.
Here is at least the serial run simpleFoam log. But i am a little bit confused, where are there other stack-traces as in the parallel run log? I hope i am posting the right thing here, sorry, if not.

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

Create mesh for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting RAS turbulence model kOmegaSST
#0 Foam::error::printStack(Foam::Ostream&) in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 __restore_rt at sigaction.c:0
#3 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::mag<Foam::SymmTensor<double>, Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<Foam ::SymmTensor<double>, Foam::fvPatchField, Foam::volMesh> > const&) in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#4 Foam::incompressible::RASModels::kOmegaSST::kOmega SST(Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&) in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#5 Foam::incompressible::RASModel::adddictionaryConst ructorToTable<Foam::incompressible::RASModels::kOm egaSST>::New(Foam::GeometricField<Foam::Vector<dou ble>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&) in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#6 Foam::incompressible::RASModel::New(Foam::Geometri cField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&) in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#7 main in "/share/apps/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64GccDPOpt/simpleFoam"
#8 __libc_start_main in "/lib64/libc.so.6"
#9 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/share/apps/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64GccDPOpt/simpleFoam"
[1]+ Done snappyHexMesh -overwrite > log
Floating point exception


You see, i am not as firm in OpenFoam until now, but i am working on it.
greets
Uli

gschaider March 3, 2011 13:31

Quote:

Originally Posted by U.Golling (Post 297814)
Hello,
Sorry for the long time i didn`t answer.
Here is at least the serial run simpleFoam log. But i am a little bit confused, where are there other stack-traces as in the parallel run log? I hope i am posting the right thing here, sorry, if not.

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

Create mesh for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting RAS turbulence model kOmegaSST
#0 Foam::error::printStack(Foam::Ostream&) in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 __restore_rt at sigaction.c:0
#3 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::mag<Foam::SymmTensor<double>, Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<Foam ::SymmTensor<double>, Foam::fvPatchField, Foam::volMesh> > const&) in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#4 Foam::incompressible::RASModels::kOmegaSST::kOmega SST(Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&) in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#5 Foam::incompressible::RASModel::adddictionaryConst ructorToTable<Foam::incompressible::RASModels::kOm egaSST>::New(Foam::GeometricField<Foam::Vector<dou ble>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&) in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#6 Foam::incompressible::RASModel::New(Foam::Geometri cField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&) in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#7 main in "/share/apps/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64GccDPOpt/simpleFoam"
#8 __libc_start_main in "/lib64/libc.so.6"
#9 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/share/apps/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64GccDPOpt/simpleFoam"
[1]+ Done snappyHexMesh -overwrite > log
Floating point exception


You see, i am not as firm in OpenFoam until now, but i am working on it.
greets
Uli

It would have been easier with line-numbers. But according to your stack trace (#3) the problem is the mag in this line of the constructor:

nut_ = a1_*k_/max(a1_*omega_, F2()*mag(symm(fvc::grad(U_))));

My guess is that grad(U) produces a weird value and it goes downhill from there. But no idea what the concrete problem might be. I guess it is a problem with the case-setup

usergk April 20, 2011 12:24

Hello,

I am trying to implement combustion in OpenFOAM and while the solver works well for equivalence ratio = 0.84, for other values (such as 0.66), I get the error below. This happens mid-way during the simulation, after a few time steps.

Any idea why this could be occurring? I am relatively new to using OpenFOAM, so any information would be appreciated.

Thanks!
gk

PS. I posted this as a new thread, but haven't got replies. Hoping this may help!

[24] #0 Foam::error::printStack(Foam::Ostream&) in "/home/gk/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
[24] #1 Foam::sigFpe::sigFpeHandler(int) in "/home/gk/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
[24] #2 in "/lib/libc.so.6"
[24] #3 in "/lib/libm.so.6"
[24] #4 pow in "/lib/libm.so.6"
[24] #5 Foam::ODEChemistryModel<Foam::psiChemistryModel, Foam::sutherlandTransport<Foam::specieThermo<Foam: :janafThermo<Foam::perfectGas> > > >::omega(Foam::Reaction<Foam::sutherlandTranspor t< Foam::specieThermo<Foam::janafThermo<Foam::perfect Gas> > > > const&, Foam::Field<double> const&, double, double, double&, double&, int&, double&, double&, int&) const in "/home/gk/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libchemistryModel.so"
[24] #6 Foam::ODEChemistryModel<Foam::psiChemistryModel, Foam::sutherlandTransport<Foam::specieThermo<Foam: :janafThermo<Foam::perfectGas> > > >::tc() const in "/home/gk/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libchemistryModel.so"
[24] #7
[24] in "/home/gk/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/pFoam"
[24] #8 __libc_start_main in "/lib/libc.so.6"
[24] #9
[24] in "/home/gk/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/pFoam"
[node69:00818] *** Process received signal ***
[node69:00818] Signal: Floating point exception (8)
[node69:00818] Signal code: (-6)
[node69:00818] Failing at address: 0x58f800000332
[node69:00818] [ 0] /lib/libc.so.6(+0x33af0) [0x2b0cdf0abaf0]
[node69:00818] [ 1] /lib/libc.so.6(gsignal+0x35) [0x2b0cdf0aba75]
[node69:00818] [ 2] /lib/libc.so.6(+0x33af0) [0x2b0cdf0abaf0]
[node69:00818] [ 3] /lib/libm.so.6(+0x13e81) [0x2b0cdebf0e81]
[node69:00818] [ 4] /lib/libm.so.6(pow+0x15) [0x2b0cdec02765]
[node69:00818] [ 5] /home/gk/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libchemistryModel.so(_ZNK4Foam17ODEChemistryModelI NS_17psiChemistryModelENS_19sutherlandTransportINS _12specieThermoINS_11janafThermoINS_10perfectGasEE EEEEEE5omegaERKNS_8ReactionIS8_EERKNS_5FieldIdEEdd RdSI_RiSI_SI_SJ_+0x285) [0x2b0cdd978ff5]
[node69:00818] [ 6] /home/gk/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libchemistryModel.so(_ZNK4Foam17ODEChemistryModelI NS_17psiChemistryModelENS_19sutherlandTransportINS _12specieThermoINS_11janafThermoINS_10perfectGasEE EEEEEE2tcEv+0x57e) [0x2b0cdd98424e]
[node69:00818] [ 7] pFoam() [0x426bf3]
[node69:00818] [ 8] /lib/libc.so.6(__libc_start_main+0xfd) [0x2b0cdf096c4d]
[node69:00818] [ 9] pFoam() [0x421119]
[node69:00818] *** End of error message ***

ehsankf November 25, 2012 04:36

Hello everybody,

Could someone please help me to understand the reason for the error in my simpleFoam -parallel run:


[2] [4] #0 [6] #0 Foam::error::printStack(Foam::Ostream&)Foam::error ::printStack(Foam::Ostream&)#0 Foam::error::printStack(Foam::Ostream&)[9] [11] #0 Foam::error::printStack(Foam::Ostream&)[8] #0 Foam::error::printStack(Foam::Ostream&)[14] #0 Foam::error::printStack(Foam::Ostream&)#0 Foam::error::printStack(Foam::Ostream&)--------------------------------------------------------------------------
An MPI process has executed an operation involving a call to the
"fork()" system call to create a child process. Open MPI is currently
operating in a condition that could result in memory corruption or
other system errors; your MPI job may hang, crash, or produce silent
data corruption. The use of fork() (or system() or other calls that
create child processes) is strongly discouraged.

The process that invoked fork was:

Local host: mmm012 (PID 16754)
MPI_COMM_WORLD rank: 6

If you are *absolutely sure* that your application will successfully
and correctly survive a call to fork(), you may disable this warning
by setting the mpi_warn_on_fork MCA parameter to 0.
--------------------------------------------------------------------------
in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1 in "/home/ekazemif/OpenFOAM/OpenFOAM-2 in "/ho.1/platforms/linux64GccDPOpt/lib/libOpenFOAM..1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[6] #1 so"
[4] #1 Foam::sigFpe::sigHandler(int)me/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
Foam::sigFpe::sigHandler(int)[2] #1 Foam::sigFpe::sigHandler(int) in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[4] #2 in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[2] #2 in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[6] #2 in "/lib64/libc.so.6"
[4] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/lib64/libc.so.6"
[2] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/lib64/libc.so.6"
[6] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[6] #4 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platf in "/home/ekorms/linux64GccDPOpt/lib/libOpenFOAM.so"
[2] #4 azemif/OpenFOAM/OpenFOAM-2.1.1/platformsFoam::fvMatrix<double>::solve(Foam::dicti onary const&)/linux64GccDPOpt/lib/libOpenFOAM.so"
[4] #4 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
[2] #5 Foam::fvMatrix<double>::solve() in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
[6] #5 Foam::fvMatrix<double>::solve() in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
[4] #5 Foam::fvMatrix<double>::solve() in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libincompressibleLESModels.so"
[6] #6 Foam::incompressible::LESModels::unified_smooth_vd ::correct(Foam::tmp<Foam::GeometricField<Foam::Ten sor<double>, Foam::fvPatchField, Foam::volMesh> > const&) in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libincompressibleLESModels.so"
[4] #6 Foam::incompressible::LESModels::unified_smooth_vd ::correct(Foam::tmp<Foam::GeometricField<Foam::Ten sor<double>, Foam::fvPatchField, Foam::volMesh> > const&) in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libincompressibleLESModels.so"
[2] #6 Foam::incompressible::LESModels::unified_smooth_vd ::correct(Foam::tmp<Foam::GeometricField<Foam::Ten sor<double>, Foam::fvPatchField, Foam::volMesh> > const&) in "/home/ekazemif/OpenFOAM/ekazemif-2.1.1/platforms/linux64GccDPOpt/lib/libmyIncompressibleUnifiedModels.so"
[6] #7 Foam::incompressible::LESModel::correct() in "/home/ekazemif/OpenFOAM/ekazemif-2.1.1/platforms/linux64GccDPOpt/lib/libmyIncompressibleUnifiedModels.so"
[4] #7 Foam::incompressible::LESModel::correct() in "/home/ekazemif/OpenFOAM/ekazemif-2.1.1/platforms/linux64GccDPOpt/lib/libmyIncompressibleUnifiedModels.so"
[2] #7 Foam::incompressible::LESModel::correct() in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libincompressibleLESModels.so"
[6] #8 in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libincompressibleLESModels.so"
[4] #8 in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/ in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[8] #1 in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lplatforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[14] #1 Foam::sigFpe::sigHandler(int)Foam::sigFpe::sigHand ler(int)ib/libOpenFOAM.so"
[11] #1 Foam::sigFpe::sigHandler(int) in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libincompressibleLESModels.so"
[2] #8 in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[9] #1 Foam::sigFpe::sigHandler(int)


in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[8] #2 [4] in "/home/ekazemif/OpenFOAM/ekazemif-2.1.1/platforms/linux64GccDPOpt/bin/EkmanFoamCf"
[4] #9 __libc_start_main[6] in "/home/ekazemif/OpenFOAM/ekazemif-2.1.1/platforms/linux64GccDPOpt/bin/EkmanFoamCf"
[6] #9 __libc_start_main in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[11] #2 in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[9] #2 in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[14] #2 in "/lib64/libc.so.6"
[8] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/lib64/libc.so.6"
[4] #10 in "/lib64/libc.so.6"
[11] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const[2] in "/home/ekazemif/OpenFOAM/ekazemif-2.1.1/platforms/linux64GccDPOpt/bin/EkmanFoamCf"
[2] #9 __libc_start_main in "/lib64/libc.so.6"
[9] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/lib64/libc.so.6"
[14] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/lib64/libc.so.6"
[6] #10

in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[8] #4 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[11] #4 in Foam::fvMatrix<double>::solve(Foam::dictionary const&)"/lib64/libc.so.6"
[2] #10 in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[9] #4 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[14] #4 Foam::fvMatrix<double>::solve(Foam::dictionary const&)[4] in "/home/ekazemif/OpenFOAM/ekazemif-2.1.1/platforms/linux64GccDPOpt/bin/EkmanFoamCf"
[mmm012:16752] *** Process received signal ***
[mmm012:16752] Signal: Floating point exception (8)
[mmm012:16752] Signal code: (-6)
[mmm012:16752] Failing at address: 0x4e3f00004170
[mmm012:16752] [ 0] /lib64/libc.so.6(+0x32920) [0x2b4415a5d920]
[mmm012:16752] [ 1] /lib64/libc.so.6(gsignal+0x35) [0x2b4415a5d8a5]
[mmm012:16752] [ 2] /lib64/libc.so.6(+0x32920) [0x2b4415a5d920]
[mmm012:16752] [ 3] /home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZNK4Foam5PBiCG5solveERNS_5FieldIdE ERKS2_h+0xf05) [0x2b4414bdb825]
[mmm012:16752] [ 4] /home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libfiniteVolume.so(_ZN4Foam8fvMatrixIdE5solveERKNS _10dictionaryE+0x153) [0x2b4413b8ca03]
[mmm012:16752] [ 5] /home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libincompressibleLESModels.so(_ZN4Foam8fvMatrixIdE 5solveEv+0xea) [0x2b4412f59a5a]
[mmm012:16752] [ 6] /home/ekazemif/OpenFOAM/ekazemif-2.1.1/platforms/linux64GccDPOpt/lib/libmyIncompressibleUnifiedModels.so(_ZN4Foam14inco mpressible9LESModels17unified_smooth_vd7correctERK NS_3tmpINS_14GeometricFieldINS_6TensorIdEENS_12fvP atchFieldENS_7volMeshEEEEE+0x2a03) [0x2b442d854793]
[mmm012:16752] [ 7] /home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libincompressibleLESModels.so(_ZN4Foam14incompress ible8LESModel7correctEv+0x35) [0x2b4412efece5]
[mmm012:16752] [ 8] EkmanFoamCf() [0x41b66b]
[mmm012:16752] [ 9] /lib64/libc.so.6(__libc_start_main+0xfd) [0x2b4415a49cdd]
[mmm012:16752] [10] EkmanFoamCf() [0x419de9]
[mmm012:16752] *** End of error message ***
[6] in "/home/ekazemif/OpenFOAM/ekazemif-2.1.1/platforms/linux64GccDPOpt/bin/EkmanFoamCf"
[mmm012:16754] *** Process received signal ***
[mmm012:16754] Signal: Floating point exception (8)
[mmm012:16754] Signal code: (-6)
[mmm012:16754] Failing at address: 0x4e3f00004172

[mmm012:16754] [ 0] /lib64/libc.so.6(+0x32920) [0x2b0b6f0c4920]
[mmm012:16754] [ 1] /lib64/libc.so.6(gsignal+0x35) [0x2b0b6f0c48a5]
[mmm012:16754] [ 2] /lib64/libc.so.6(+0x32920) [0x2b0b6f0c4920]
[mmm012:16754] [ 3] /home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZNK4Foam5PBiCG5solveERNS_5FieldIdE ERKS2_h+0xf05) [0x2b0b6e242825]
[mmm012:16754] [ 4] /home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libfiniteVolume.so(_ZN4Foam8fvMatrixIdE5solveERKNS _10dictionaryE+0x153) [0x2b0b6d1f3a03]
[mmm012:16754] [ 5] /home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libincompressibleLESModels.so(_ZN4Foam8fvMatrixIdE 5solveEv+0xea) [0x2b0b6c5c0a5a]
[mmm012:16754] [ 6] /home/ekazemif/OpenFOAM/ekazemif-2.1.1/platforms/linux64GccDPOpt/lib/libmyIncompressibleUnifiedModels.so(_ZN4Foam14inco mpressible9LESModels17unified_smooth_vd7correctERK NS_3tmpINS_14GeometricFieldINS_6TensorIdEENS_12fvP atchFieldENS_7volMeshEEEEE+0x2a03) [0x2b0b85854793]
[mmm012:16754] [ 7] /home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libincompressibleLESModels.so(_ZN4Foam14incompress ible8LESModel7correctEv+0x35) [0x2b0b6c565ce5]
[mmm012:16754] [ 8] EkmanFoamCf() [0x41b66b]
[mmm012:16754] [ 9] /lib64/libc.so.6(__libc_start_main+0xfd) [0x2b0b6f0b0cdd]
[mmm012:16754] [10] EkmanFoamCf() [0x419de9]
[mmm012:16754] *** End of error message ***
[2] in "/home/ekazemif/OpenFOAM/ekazemif-2.1.1/platforms/linux64GccDPOpt/bin/EkmanFoamCf"
[mmm012:16750] *** Process received signal ***
[mmm012:16750] Signal: Floating point exception (8)
[mmm012:16750] Signal code: (-6)
[mmm012:16750] Failing at address: 0x4e3f0000416e
[mmm012:16750] [ 0] /lib64/libc.so.6(+0x32920) [0x2b6674268920]
[mmm012:16750] [ 1] /lib64/libc.so.6(gsignal+0x35) [0x2b66742688a5]
[mmm012:16750] [ 2] /lib64/libc.so.6(+0x32920) [0x2b6674268920]
[mmm012:16750] [ 3] /home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZNK4Foam5PBiCG5solveERNS_5FieldIdE ERKS2_h+0xf05) [0x2b66733e6825]
[mmm012:16750] [ 4] /home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libfiniteVolume.so(_ZN4Foam8fvMatrixIdE5solveERKNS _10dictionaryE+0x153) [0x2b6672397a03]
[mmm012:16750] [ 5] /home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libincompressibleLESModels.so(_ZN4Foam8fvMatrixIdE 5solveEv+0xea) [0x2b6671764a5a]
[mmm012:16750] [ 6] /home/ekazemif/OpenFOAM/ekazemif-2.1.1/platforms/linux64GccDPOpt/lib/libmyIncompressibleUnifiedModels.so(_ZN4Foam14inco mpressible9LESModels17unified_smooth_vd7correctERK NS_3tmpINS_14GeometricFieldINS_6TensorIdEENS_12fvP atchFieldENS_7volMeshEEEEE+0x2a03) [0x2b668d854793]
[mmm012:16750] [ 7] /home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libincompressibleLESModels.so(_ZN4Foam14incompress ible8LESModel7correctEv+0x35) [0x2b6671709ce5]
[mmm012:16750] [ 8] EkmanFoamCf() [0x41b66b]
[mmm012:16750] [ 9] /lib64/libc.so.6(__libc_start_main+0xfd) [0x2b6674254cdd]
[mmm012:16750] [10] EkmanFoamCf() [0x419de9]
[mmm012:16750] *** End of error message ***
in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
[8] #5 Foam::fvMatrix<double>::solve()--------------------------------------------------------------------------
mpirun noticed that process rank 4 with PID 16752 on node mmm012 exited on signal 8 (Floating point exception).
--------------------------------------------------------------------------
in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
[9] #5 Foam::fvMatrix<double>::solve()[mmm012:16747] 6 more processes have sent help message help-mpi-runtime.txt / mpi_init:warn-fork
[mmm012:16747] Set MCA parameter "orte_base_help_aggregate" to 0 to see all help / error messages

gschaider November 25, 2012 05:21

Quote:

Originally Posted by ehsankf (Post 394023)
Hello everybody,

Could someone please help me to understand the reason for the error in my simpleFoam -parallel run:

<snip>

[8] #5 Foam::fvMatrix<double>::solve()--------------------------------------------------------------------------
mpirun noticed that process rank 4 with PID 16752 on node mmm012 exited on signal 8 (Floating point exception).
--------------------------------------------------------------------------
in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
[9] #5 Foam::fvMatrix<double>::solve()[mmm012:16747] 6 more processes have sent help message help-mpi-runtime.txt / mpi_init:warn-fork
[mmm012:16747] Set MCA parameter "orte_base_help_aggregate" to 0 to see all help / error messages

Seems like some (not all) of the processes encountered a floating point exception. These processors are now on different parts of the program (the exception handler) and therefor won't communicate properly with the others

ehsankf January 2, 2013 16:23

Could anyone please help me to understand this problem in parallel run.
I do not encounter any problem in serial running.
[31] [46] ##00 Foam::error::printStack(Foam::Ostream&)Foam::error ::printStack(Foam::Ostream&)[6] #0 Foam::error::printStack(Foam::Ostream&)[23] #0 Foam::error::printStack(Foam::Ostream&)[37] [60] [26] #0 Foam::error::printStack(Foam::Ostream&)[45] #0 Foam::error::printStack(Foam::Ostream&)#[27] #0#0 0 Foam::error::printStack(Foam::Ostream&) Foam::error::printStack(Foam::Ostream&)Foam::error ::printStack(Foam::Ostream&)[16] #0 Foam::error::printStack(Foam::Ostream&)[22] #0 Foam::error::printStack(Foam::Ostream&)[34] #0 Foam::error::printStack(Foam::Ostream&)[18] #0 Foam::error::printStack(Foam::Ostream&)[25] #0 Foam::error::printStack(Foam::Ostream&)[47] #0 Foam::error::printStack(Foam::Ostream&)[5] #0 Foam::error::printStack(Foam::Ostream&)[51] #0 Foam::error::printStack(Foam::Ostream&)[41] #0 --------------------------------------------------------------------------
An MPI process has executed an operation involving a call to the
"fork()" system call to create a child process. Open MPI is currently
operating in a condition that could result in memory corruption or
other system errors; your MPI job may hang, crash, or produce silent
data corruption. The use of fork() (or system() or other calls that
create child processes) is strongly discouraged.

The process that invoked fork was:

Local host: mmm067 (PID 27278)
MPI_COMM_WORLD rank: 46

If you are *absolutely sure* that your application will successfully
and correctly survive a call to fork(), you may disable this warning
by setting the mpi_warn_on_fork MCA parameter to 0.
--------------------------------------------------------------------------
[55] Foam::error::printStack(Foam::Ostream&)#0 [1] #0 [15] #0 Foam::error::printStack(Foam::Ostream&)Foam::error ::printStack(Foam::Ostream&)Foam::error::printStac k(Foam::Ostream&)[8] #0 Foam::error::printStack(Foam::Ostream&)[2] #0 [12] #0 Foam::error::printStack(Foam::Ostream&)Foam::error ::printStack(Foam::Ostream&)[21] #0 Foam::error::printStack(Foam::Ostream&)[53] #0 Foam::error::printStack(Foam::Ostream&)[52] #0 [63] #Foam::error::printStack(Foam::Ostream&)[58] #0 0 Foam::error::printStack(Foam::Ostream&)Foam::error ::printStack(Foam::Ostream&)[29] #0 Foam::error::printStack(Foam::Ostream&)[20] #0 Foam::error::printStack(Foam::Ostream&)[57] #0 Foam::error::printStack(Foam::Ostream&)[39] #0 Foam::error::printStack(Foam::Ostream&)[28] #0 Foam::error::printStack(Foam::Ostream&)[10] #0 Foam::error::printStack(Foam::Ostream&)[24] #0 Foam::error::printStack(Foam::Ostream&)[30] #0 Foam::error::printStack(Foam::Ostream&)[17] #0 Foam::error::printStack(Foam::Ostream&)[19] #0 Foam::error::printStack(Foam::Ostream&)[7] #0 Foam::error::printStack(Foam::Ostream&)[43] #0 Foam::error::printStack(Foam::Ostream&)[9] #0 Foam::error::printStack(Foam::Ostream&)[13] #0 Foam::error::printStack(Foam::Ostream&)[4] #0 Foam::error::printStack(Foam::Ostream&) addr2line failed
[46] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[18] #1 Foam::sigFpe::sigHandler(int)[62] #0 Foam::error::printStack(Foam::Ostream&)[38] #0 Foam::error::printStack(Foam::Ostream&)[14] #0 Foam::error::printStack(Foam::Ostream&) addr2line failed
[31] #1 Foam::sigFpe::sigHandler(int)[0] #0 Foam::error::printStack(Foam::Ostream&)[11] #0 Foam::error::printStack(Foam::Ostream&) addr2line failed
[16] #1 Foam::sigFpe::sigHandler(int)[32] #0 Foam::error::printStack(Foam::Ostream&)[3] #0 Foam::error::printStack(Foam::Ostream&)[49] #0 Foam::error::printStack(Foam::Ostream&) addr2line failed
[26] #1 Foam::sigFpe::sigHandler(int)[40] #0 Foam::error::printStack(Foam::Ostream&)[35] #0 Foam::error::printStack(Foam::Ostream&) addr2line failed
[53] #1 Foam::sigFpe::sigHandler(int)[33] #0 Foam::error::printStack(Foam::Ostream&) addr2line failed
[25] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[29] #1 Foam::sigFpe::sigHandler(int)[36] #0 addr2line failed
[27] #1 Foam::sigFpe::sigHandler(int)Foam::error::printSta ck(Foam::Ostream&)[44] #0 Foam::error::printStack(Foam::Ostream&)[42] #0 Foam::error::printStack(Foam::Ostream&) addr2line failed
[41] #1 Foam::sigFpe::sigHandler(int)[59] #0 Foam::error::printStack(Foam::Ostream&) addr2line failed
[22] #1 Foam::sigFpe::sigHandler(int)[56] #0 Foam::error::printStack(Foam::Ostream&)[50] #0 Foam::error::printStack(Foam::Ostream&)[48] #0 Foam::error::printStack(Foam::Ostream&)[61] #0 Foam::error::printStack(Foam::Ostream&) addr2line failed
[51] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[55] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[39] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[34] #1 addr2line failed
[20] #1 Foam::sigFpe::sigHandler(int)Foam::sigFpe::sigHand ler(int) addr2line failed
[21] #1 Foam::sigFpe::sigHandler(int)[54] #0 Foam::error::printStack(Foam::Ostream&) addr2line failed
[28] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[57] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[45] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[43] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[24] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[38] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[58] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[30] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[32] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[63] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[23] #1 addr2line failed
[46] #2 addr2line failed
[52] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[37] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[19] #1 Foam::sigFpe::sigHandler(int)Foam::sigFpe::sigHand ler(int) addr2line failed
[17] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[40] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[47] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[62] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[18] #2 addr2line failed
[31] #2 addr2line failed
[33] #1 addr2line failed
[60] #1 Foam::sigFpe::sigHandler(int) Foam::sigFpe::sigHandler(int) addr2line failed
[35] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[16] #2 addr2line failed
[41] #2 in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #1 Foam::sigFpe::sigHandler(int) in "/home/ekazemif/ in "/hom addr2line failed
[42] #1 Foam::sigFpe::sigHandler(int)OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/libe/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[15] #/libOpenFOAM.so"
[8] #1 1 Foam::sigFpe::sigHandler(int)Foam::sigFpe::sigHand ler(int) in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[2] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[25] #2 addr2line failed
[36] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[49] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[26] #2 addr2line failed
[59] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[29] #2 addr2line failed
[53] #2 addr2line failed
[27] #2 addr2line failed
[56] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[61] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[55] #2 in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" in in "/home/ekazemif/O
[5] #1 penFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt"/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOFoam::sigFpe::sigHandler(int)/lib/libOpenFOAM.so"
[12] #pt/lib/libOpenFOAM.so"
addr2line failed
[50] #1 Foam::sigFpe::sigHandler(int)[6] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[21] #2 1 Foam::sigFpe::sigHandler(int) in "/home/ekazemif/OpenFOA in "/home/ekazemif/OpenFOAM/O addr2line failed
[51] #penFOAM-2.1.1/platforms/linux64GccDPOpt/lib/ addr2line failed
[20] #2 addr2line failed
[48] #1M/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFlibOpenFOAM.so"
[7] #1 Foam::sigFpe::sigHandler(int)2 OAM.so"
Foam::sigFpe::sigHandler(int)[10] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[57] #2 in "/home/ekazemif/Open addr2line failed
[22] #2 FOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[9] #1 Foam::sigFpe::sigHandler(int) in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[14] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[44] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[52] #2 addr2line failed
[28] #2 addr2line failed
[30] #2 addr2line failed
[54] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[58] #2 in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[4] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[62] #2 addr2line failed
[24] #2 in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[3] #1 addr2line failed
[34] #2 Foam::sigFpe::sigHandler(int) addr2line failed
[63] #2 in "/homeOpenFOAM in "/home/OpenFOAM/OpenFOAM-2.1.1/platforms/linu/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
x64GccDPOpt/lib/libOpenFOAM.so"
[11] #1 Foam::sigFpe::sigHandler(int)[13] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[45] #2 addr2line failed
addr2line failed
[39] #2 [43] #2 addr2line failed
[23] #2 addr2line failed
[32] #2 addr2line failed
[17] #2 addr2line failed
[19] #2 addr2line failed
[46] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[38] #2 addr2line failed
[31] #3 addr2line failed Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const
[16] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[18] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[40] #2 addr2line failed
[33] #2 addr2line failed
[49] #2 addr2line failed
[37] #2 addr2line failed
[59] #2 addr2line failed
[41] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[61] #2 addr2line failed
[42] #2 in "/home/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[0] #1 Foam::sigFpe::sigHandler(int) addr2line failed
[25] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[35] #2 in "/home/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[8] #2 addr2line failed
[29] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[26] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[36] #2 addr2line failed
[56] #2 addr2line failed
[57] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[55] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[60] #2 addr2line failed
[44] #2 addr2line failed
[21] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[27] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[47] #2 addr2line failed
[20] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[34] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[51] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[28] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[30] #3 in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #2 addr2line failed
[22] # addr2line failed
[43] #3 3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) constFoam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[15] #2 addr2line failed
[23] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[58] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[45] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[53] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[48] #2 addr2line failed
[50] #2 in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[2] #2 addr2line failed
[19] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[17] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[24] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[31] #4 addr2line failed
[32] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[16] #4 addr2line failed
[38] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[18] #4 addr2line failed
[63] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[52] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[25] #4 addr2line failed
[49] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[29] #4 addr2line failed
[46] #4 addr2line failed
[39] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[61] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[40] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[54] #2 in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[10] # addr2line failed
[26] #4 2 addr2line failed
[41] #4 addr2line failed
[62] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/homeOpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
in "/home/OpenFOAM/OpenFOAM-2.1.1/p[11] #2 latforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[5] #2 addr2line failed
[20] #4 in "/home/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[12] #2 addr2line failed
[35] #3 in "/home/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFO addr2line failed
[21] #4 addr2line failed
[33] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) constAM.so"
[6] #2 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[27] #4 addr2line failed
[37] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[59] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[28] #4 addr2line failed
[30] #4 addr2line failed
[56] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[47] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/ekazemif/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[9] #2 addr2line failed
[23] #4 in "/home/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[14] #2 addr2line failed
[55] #4 addr2line failed
[43] #4 addr2line failed
[58] #4 addr2line failed
[44] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[34] #4 addr2line failed
[42] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[57] #4 addr2line failed
[48] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[51] #4 addr2line failed
[19] #4 addr2line failed
[53] #4 addr2line failed
[36] #3 in "/home/ekazemif/OpenFOAM/OpenFOFoam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) constAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[7] #2 addr2line failed
[22] #4 addr2line failed
[32] #4 addr2line failed
[17] #4 addr2line failed
[38] #4 addr2line failed
[63] #4
[31]
[31] #5 addr2line failed
[50] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[52] #4 in "/lib64/libc.so.6"
[8] # addr2line failed
[45] #4 3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[3] #2 addr2line failed
[49] #4 in "/home/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[13] #2 addr2line failed
[24] #4
[18]
[18] #5
[41]
[41] #5 in "/lib64/libc.so.6"
[2] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const
[46]
[46] #5 in "/lib64/libc.so.6"
[16]
[16] #5
[1] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[39] #4
[29]
[29] #5 addr2line failed
[33] #4 addr2line failed
[60] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/OpenFOAM/OpenFOAM-
[26]
[26] #5 2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
addr2line failed
[40] #[0] #2 4
[25]
[25] #5 addr2line failed
[54] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[4] #2 in "/lib64/libc.so.6"
[10] #3
[20]
[20] #5 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const
[21]
[21] #5 addr2line failed
[61] #4
[43]
[43] #5 addr2line failed
[35] #4 in "/lib64/libc.so.6"
[15] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[62] #4 addr2line failed
[37] #4 addr2line failed
[47] #4 in "/lib64/libc.so.6"
[11] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const addr2line failed
[59] #4
[27]
[27] #5 in "/lib64/libc.so.6"
[6] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const
[28]
[28] #5
[34]
[34] #5 addr2line failed
[42] #4 addr2line failed
[44] #4
[32]
[32] #5 addr2line failed
[36] #4
[55]
[55] #5
[38]
[38] #5
[58]
[58] #5 in "/lib64/libc.so.6"
[5] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const
[30]
[30] #5 addr2line failed
[56] #4
[41]
[41] #6 in "/lib64/libc.so.6"
[12] #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const

gschaider January 5, 2013 19:11

Quote:

Originally Posted by ehsankf (Post 399818)
Could anyone please help me to understand this problem in parallel run.
I do not encounter any problem in serial running.
[31] [46] ##00 Foam::error::printStack(Foam::Ostream&)Foam::error ::printStack(Foam::Ostream&)[6] #0 Foam::error::printStack(Foam::Ostream&)[23] #0

Story is simple: on at least one processor the linear solver PbiCG experienced a floating point error and this made the run fail. What actually caused the error is hard to tell without at least some basic information (OS version, OF version, whether the error occurred at the first timestep) but probably a bit more info will be needed (solver, BCs etc)

babakflame February 22, 2013 12:13

Dear Bernhard
Hi
I have a same problem like the others, However I am trying to run a solver with the changes I made to it. would you please take a look at my error and hint me:

PHP Code:

Creating turbulence model

Selecting turbulence model type LESModel
Selecting LES turbulence model oneEqEddy
oneEqEddyCoeffs
{
    
ce              1.048;
    
Prt             1;
    
ck              0.094;
}

Creating field dpdt

Creating field kinetic energy K

Reading flamelet dictionary

Preparing field Qrad 
(radiative heat transfer)

Courant Number mean3.01006e-05 max0.0379248

PIMPLE
Operating solver in PISO mode


Starting time loop

Reading
/calculating field UMean

Reading
/calculating field pMean

Reading
/calculating field UPrime2Mean

Reading
/calculating field pPrime2Mean

fieldAverage
starting averaging at time 0

Courant Number mean
3.01006e-05 max0.0379248
deltaT 
1.2e-06
Time 
1.2e-06

#0  Foam::error::printStack(Foam::Ostream&) in "/home/babak/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/home/babak/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/home/babak/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4  Foam::operator/(Foam::UList<double> const&, Foam::UList<double> const&) in "/home/babak/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5  Foam::diagonalSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/babak/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6  Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/home/babak/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#7  Foam::fvMatrix<double>::solve() in "/home/babak/OpenFOAM/babak-2.1.x/platforms/linux64GccDPOpt/bin/turbulentFlameletRhoPimpleFoam"
#8  
 
in "/home/babak/OpenFOAM/babak-2.1.x/platforms/linux64GccDPOpt/bin/turbulentFlameletRhoPimpleFoam"
#9  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#10  
 
in "/home/babak/OpenFOAM/babak-2.1.x/platforms/linux64GccDPOpt/bin/turbulentFlameletRhoPimpleFoam"
Floating point exception
rm
cannot remove `pro*': No such file or directory 

Regards
Bobi

ebrahim27 February 22, 2013 12:46

Hello babak

you can see : http://openfoamwiki.net/index.php/HowTo_debugging

gschaider February 22, 2013 13:50

Quote:

Originally Posted by babakflame (Post 409561)
Dear Bernhard
Hi
I have a same problem like the others, However I am trying to run a solver with the changes I made to it. would you please take a look at my error and hint me:

There is not even the most basic information here. For instance "which solver". The title of the thread says "simpleFoam" but the output is clearly not from that solver.

From the stack-trace ("diagonalSolver") my bet is that you set a pressure to 0 in a compressible solver.

babakflame February 22, 2013 14:14

Dear Bernhard
Hi
I have used RhoPimpleFoam solver combined with flamelet code from Cuocci et al.
I am trying to model a free jet flame. In my boundary condition, I have Fuel inlet, air inlet , outlet , walls.
I am using OF version 2.1.0
If more information is needed, Just let me know.

Best Regards
Bobi

gschaider February 22, 2013 16:30

Quote:

Originally Posted by babakflame (Post 409580)
Dear Bernhard
Hi
I have used RhoPimpleFoam solver combined with flamelet code from Cuocci et al.
I am trying to model a free jet flame. In my boundary condition, I have Fuel inlet, air inlet , outlet , walls.
I am using OF version 2.1.0
If more information is needed, Just let me know.

Best Regards
Bobi

Have you read the second paragraph of my posting: my guess is that you set a boundary condition somewhere to 0

babakflame February 23, 2013 10:47

Dear Bernhard
Hi
I checked the boundary condition of P
It's as Follows:

HTML Code:

dimensions          [ 1 -1 -2 0 0 0 0 ];

internalField  uniform 101325;

boundaryField
{
    inletfuel         
    {
        type            zeroGradient;
    }

    inletair         
    {
        type            zeroGradient;
    }

    "outlet"
    {
        type            fixedValue;
        value          $internalField;
    }

    "wall.*"
    {
    type        zeroGradient;
    }

    front   
    {
        type            wedge;
    }

    back 
    {
        type            wedge;
    }

    axis
    {
        type            empty;
    }
}

Although when I add these lines to the end of fvSolution file, the error changes.:rolleyes::confused::confused:

These are the added lines:

HTML Code:

residualControl
    {
        p    5e-5;
        csi    1e-5;
        H    1e-5;
    }

Then the error is as follows:

HTML Code:

--> FOAM FATAL ERROR:
Residual data for p must be specified as a dictionary

    From function bool Foam::solutionControl::read()
    in file cfdTools/general/solutionControl/solutionControl/solutionControl.C at line 79.

FOAM exiting

Would You PLZ help me body?:):)

I have pasted the fvSolution of the cuooci code, also the rhoPimple solver of OpenFoam And what I have made for the cuooci code with LES in order.

HTML Code:

solvers
{
    U
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance      1e-07;
        relTol          0.1;
    }

    p
    {
        solver          GAMG;
        tolerance        1e-8;
        relTol          0.001;

        smoother        GaussSeidel;

        cacheAgglomeration  true;
        nCellsInCoarsestLevel 10;
        agglomerator    faceAreaPair;
        mergeLevels      1;
    }

    csi
    {
    solver        PBiCG;
        preconditioner  DILU;
        tolerance        1e-07;
        relTol          0.1;
    }

    csiv2
    {
    solver        PBiCG;
        preconditioner  DILU;
        tolerance        1e-07;
        relTol          0.1;
    }

    H
    {
    solver        PBiCG;
        preconditioner  DILU;
        tolerance        1e-07;
        relTol          0.1;
    }

    k
    {
    solver        PBiCG;
        preconditioner  DILU;
        tolerance        1e-07;
        relTol          0.01;
    }

    epsilon
    {
    solver        PBiCG;
        preconditioner  DILU;
        tolerance        1e-07;
        relTol          0.01;
    }

}


SIMPLE
{
        nNonOrthogonalCorrectors 0;
    pMin pMin [1 -1 -2 0 0 0 0]  100;

        rhoMin rhoMin [1 -3 0 0 0 0 0] 0.1;
    rhoMax rhoMax [1 -3 0 0 0 0 0] 2;

    residualControl
    {
        p    5e-5;
        csi    1e-5;
        H    1e-5;
    }
}

relaxationFactors
{
    fields
    {
        p              0.4;
    }
    equations
    {
        U              0.4;
        k              0.3;
        epsilon        0.3;
        H              0.4;
        csi            0.4;
        csiv2          0.1;
    }
}

HTML Code:

solvers
{
    "(p|rho)"
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance      1e-6;
        relTol          0.01;
    }

    "(p|rho)Final"
    {
        $p;
        relTol          0;
    }

    "(U|h|k|nuTilda)"
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance      1e-6;
        relTol          0.01;
    }

    "(U|h|k|nuTilda)Final"
    {
        $U;
        relTol          0;
    }
}

PIMPLE
{
    momentumPredictor yes;
    nOuterCorrectors 3;
    nCorrectors    1;
    nNonOrthogonalCorrectors 0;
    rhoMin          rhoMin [ 1 -3 0 0 0 ] 0.5;
    rhoMax          rhoMax [ 1 -3 0 0 0 ] 2.0;
}

relaxationFactors
{
    fields
    {
    }
    equations
    {
        "(U|h|k|epsilon|omega).*"  1;
    }
}


HTML Code:

solvers
{
  rho
  {
        solver          PCG;
        preconditioner  DIC;
        tolerance      1e-06;
        relTol          0.1;
    }

    rhoFinal
    {
        $rho;
        tolerance      1e-06;
        relTol          0;
    }
    csi
    {
    solver        PBiCG;
        preconditioner  DILU;
        tolerance        1e-07;
        relTol          0.1;
    }
    csiFinal
    {
        $csi;
        tolerance      1e-07;
        relTol          0;
    }

    csiv2
    {
    solver        PBiCG;
        preconditioner  DILU;
        tolerance        1e-07;
        relTol          0.1;
    }

    csiv2Final
    {
        $csiv2;
        tolerance      1e-07;
        relTol          0;
    }

    H
    {
    solver        PBiCG;
        preconditioner  DILU;
        tolerance        1e-07;
        relTol          0.1;
    }
   
    HFinal
    {
        $H;
        tolerance      1e-07;
        relTol          0;
    }

    p
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance        1e-6;
        relTol          0.1;
    }

    pFinal
    {
        $p;
        tolerance        1e-6;
        relTol          0.0;
    }

    "(U|k|epsilon)"
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance      1e-07;
        relTol          0.01;
    }

    "(U|k|epsilon)Final"
    {
        $U;
        relTol          0;
    }
       
}
PIMPLE
{
    momentumPredictor no;
    nOuterCorrectors  1;
    nCorrectors    2;
    nNonOrthogonalCorrectors 0;
    pMin pMin [1 -1 -2 0 0 0 0]  100;

    rhoMin rhoMin [1 -3 0 0 0 0 0] 0.1;
    rhoMax rhoMax [1 -3 0 0 0 0 0] 2;

    residualControl
    {
        p    5e-6;
        csi    1e-6;
        H    1e-6;
    }
 
}




Best Regards
Bobi

wyldckat February 23, 2013 17:05

Greetings to all!

@Bobi: I got your private message and I've seen your questions and the answers given to you.

Right now, the error with the residual control is rather simple and I'll show you how I found the solution for it:
  1. Go into "tutorials" folder:
    Code:

    cd $FOAM_TUTORIALS
  2. Search for the files "fv*" that have "residualControl" in them:
    Code:

    find . -name "fv*" | xargs grep -sl residualControl
  3. From the list that appeared, I chose the closest one I could find for your solver:
    Code:

    ./compressible/rhoPimpleFoam/ras/angledDuct/system/fvSolution
  4. Inside the file you can find:
    Code:

    PIMPLE
    {
        momentumPredictor yes;
        nOuterCorrectors 50;
        nCorrectors    1;
        nNonOrthogonalCorrectors 0;
        rhoMin          rhoMin [ 1 -3 0 0 0 ] 0.5;
        rhoMax          rhoMax [ 1 -3 0 0 0 ] 2.0;

        residualControl
        {
            "(U|k|epsilon)"
            {
                relTol          0;
                tolerance      0.0001;
            }
        }
    }

    It's the same as defining:
    Code:

    PIMPLE
    {
        momentumPredictor yes;
        nOuterCorrectors 50;
        nCorrectors    1;
        nNonOrthogonalCorrectors 0;
        rhoMin          rhoMin [ 1 -3 0 0 0 ] 0.5;
        rhoMax          rhoMax [ 1 -3 0 0 0 ] 2.0;

        residualControl
        {
            U
            {
                relTol          0;
                tolerance      0.0001;
            }

            k
            {
                relTol          0;
                tolerance      0.0001;
            }

            epsilon
            {
                relTol          0;
                tolerance      0.0001;
            }
        }
    }

Best regards,
Bruno

gschaider February 24, 2013 08:46

Quote:

Originally Posted by babakflame (Post 409684)
Dear Bernhard
Hi
I checked the boundary condition of P
It's as Follows:

HTML Code:

dimensions          [ 1 -1 -2 0 0 0 0 ];

internalField  uniform 101325;

boundaryField
{
    inletfuel         
    {
        type            zeroGradient;
    }

    inletair         
    {
        type            zeroGradient;
    }

    "outlet"
    {
        type            fixedValue;
        value          $internalField;
    }

    "wall.*"
    {
    type        zeroGradient;
    }

    front   
    {
        type            wedge;
    }

    back 
    {
        type            wedge;
    }

    axis
    {
        type            empty;
    }
}


These boundary conditions look OK.

As the solver is a non-stock (self developed) solver I'd suggest that you compile a Debug-version of OpenFOAM and run the solver in that. The stack-trace will then give you line-numbers and you won't have to guess which part actually id the problematic one.

About the other problems. No idea

babakflame February 24, 2013 11:50

Dear Bruno and Bernhard
Hi
Thanks for your hints. I will try to solve my problem according to your hints.

Regards
Bobi


All times are GMT -4. The time now is 03:11.