CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

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

Register Blogs Community New Posts Updated Threads Search

Like Tree24Likes

Reply
Page 1 of 3 1 23
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 23, 2011, 12:08
Default Foam::error::printStack(Foam::Ostream&) with simpleFoam -parallel
  #1
New Member
 
Ulrich Golling
Join Date: Oct 2010
Posts: 7
Rep Power: 16
U.Golling is on a distinguished road
Hello everybody,

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

[8] #0 Foam::error:rintStack(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:rintStack(Foam::Ostream&)[4] #0 Foam::error:rintStack(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:rintStack(Foam::Ostream&)[2] #0 Foam::error:rintStack(Foam::Ostream&) in "/share/apps/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so"
[8] #7 [5] #0 Foam::error:rintStack(Foam::Ostream&)[3] #0 Foam::error:rintStack(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 . (The whole log-file is also attended).
That would be very nice.

Thank you,
Best Regards

Uli
U.Golling is offline   Reply With Quote

Old   February 23, 2011, 12:26
Default
  #2
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by U.Golling View Post
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 . (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
hogsonik, calf.Z and nicktobin like this.
gschaider is offline   Reply With Quote

Old   February 24, 2011, 10:21
Default
  #3
New Member
 
Ulrich Golling
Join Date: Oct 2010
Posts: 7
Rep Power: 16
U.Golling is on a distinguished road
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:rintStack(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
U.Golling is offline   Reply With Quote

Old   February 24, 2011, 13:53
Default
  #4
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by U.Golling View Post
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:rintStack(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
Last edited by gschaider; February 24, 2011 at 17:09.
gschaider is offline   Reply With Quote

Old   March 3, 2011, 12:11
Default
  #5
New Member
 
Ulrich Golling
Join Date: Oct 2010
Posts: 7
Rep Power: 16
U.Golling is on a distinguished road
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:rintStack(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
U.Golling is offline   Reply With Quote

Old   March 3, 2011, 13:31
Default
  #6
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by U.Golling View Post
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:rintStack(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
gschaider is offline   Reply With Quote

Old   April 20, 2011, 13:24
Default
  #7
Member
 
Join Date: Nov 2010
Posts: 54
Rep Power: 16
usergk is on a distinguished road
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:rintStack(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:siChemistryModel, Foam::sutherlandTransport<Foam::specieThermo<Foam: :janafThermo<Foam:erfectGas> > > >:mega(Foam::Reaction<Foam::sutherlandTranspor t< Foam::specieThermo<Foam::janafThermo<Foam:erfect 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:siChemistryModel, Foam::sutherlandTransport<Foam::specieThermo<Foam: :janafThermo<Foam:erfectGas> > > >::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 ***
usergk is offline   Reply With Quote

Old   November 25, 2012, 04:36
Default
  #8
Member
 
ehk
Join Date: Sep 2012
Posts: 30
Rep Power: 14
ehsankf is on a distinguished road
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:rintStack(Foam::Ostream&)Foam::error :rintStack(Foam::Ostream&)#0 Foam::error:rintStack(Foam::Ostream&)[9] [11] #0 Foam::error:rintStack(Foam::Ostream&)[8] #0 Foam::error:rintStack(Foam::Ostream&)[14] #0 Foam::error:rintStack(Foam::Ostream&)#0 Foam::error:rintStack(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
ehsankf is offline   Reply With Quote

Old   November 25, 2012, 05:21
Default
  #9
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by ehsankf View Post
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
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   January 2, 2013, 16:23
Thumbs down
  #10
Member
 
ehk
Join Date: Sep 2012
Posts: 30
Rep Power: 14
ehsankf is on a distinguished road
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
ehsankf is offline   Reply With Quote

Old   January 5, 2013, 19:11
Default
  #11
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by ehsankf View Post
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:rintStack(Foam::Ostream&)Foam::error :rintStack(Foam::Ostream&)[6] #0 Foam::error:rintStack(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)
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   February 22, 2013, 12:13
Default
  #12
Senior Member
 
Bobby
Join Date: Oct 2012
Location: Michigan
Posts: 454
Rep Power: 16
babakflame is on a distinguished road
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 mean: 3.01006e-05 max: 0.0379248

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 max: 0.0379248
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
babakflame is offline   Reply With Quote

Old   February 22, 2013, 12:46
Default
  #13
New Member
 
ebrahim
Join Date: Oct 2012
Posts: 5
Rep Power: 14
ebrahim27 is on a distinguished road
Hello babak

you can see : http://openfoamwiki.net/index.php/HowTo_debugging
ebrahim27 is offline   Reply With Quote

Old   February 22, 2013, 13:50
Default
  #14
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by babakflame View Post
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.
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   February 22, 2013, 14:14
Default
  #15
Senior Member
 
Bobby
Join Date: Oct 2012
Location: Michigan
Posts: 454
Rep Power: 16
babakflame is on a distinguished road
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
babakflame is offline   Reply With Quote

Old   February 22, 2013, 16:30
Default
  #16
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by babakflame View Post
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
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   February 23, 2013, 10:47
Default
  #17
Senior Member
 
Bobby
Join Date: Oct 2012
Location: Michigan
Posts: 454
Rep Power: 16
babakflame is on a distinguished road
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.

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
Last edited by babakflame; February 23, 2013 at 11:03.
babakflame is offline   Reply With Quote

Old   February 23, 2013, 17:05
Default
  #18
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,982
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
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
__________________
wyldckat is offline   Reply With Quote

Old   February 24, 2013, 08:46
Default
  #19
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by babakflame View Post
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
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   February 24, 2013, 11:50
Default
  #20
Senior Member
 
Bobby
Join Date: Oct 2012
Location: Michigan
Posts: 454
Rep Power: 16
babakflame is on a distinguished road
Dear Bruno and Bernhard
Hi
Thanks for your hints. I will try to solve my problem according to your hints.

Regards
Bobi
babakflame is offline   Reply With Quote

Reply
Page 1 of 3 1 23

« Previous Thread | Next Thread »

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts
BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
SimpleFoam run in Parallel jayrup OpenFOAM 9 July 26, 2019 01:00
Script to Run Parallel Jobs in Rocks Cluster asaha OpenFOAM Running, Solving & CFD 12 July 4, 2012 23:51
Error running simpleFoam in parallel skabilan OpenFOAM Running, Solving & CFD 2 August 29, 2008 10:42
Own boundary condition modified simpleFoam erorr in parallel execution sponiar OpenFOAM Running, Solving & CFD 1 August 27, 2008 10:16
Parallel Computing Classes at San Diego Supercomputer Center Jan. 20-22 Amitava Majumdar Main CFD Forum 0 January 5, 1999 13:00


All times are GMT -4. The time now is 00:59.

Contact Us - CFD Online - Privacy Statement - Top