hello all, I am using react
 

hello all,

I am using reactingFoam in a simple geometry with 2 inlets and a outlet.I have manually edited all the files of U,O2,etc.. but on solving with reactingFoam , I get the following error:

#0 Foam::error::printStack(Foam:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&)
#1 Foam::sigFpe::sigFpeHandler(int)
#2 ??
#3 Foam::polyMesh::calcDirections() const
#4 Foam::polyMesh::directions() const
#5 Foam::fvMatrix<foam::vector<double> >::solve(Foam::Istream&)
#6 Foam::lduMatrix::solverPerformance Foam::solve<foam::vector<double> >(Foam::tmp<foam::fvmatrix<foam::vector<double> > > const&)
#7 main
#8 __libc_start_main
#9 __gxx_personality_v0

What does this error mean?and how to resolve it?

Thanks.
Mayank.

That means that it fails while
 

That means that it fails while calling polyMesh::calcDirections() (the last Foam-code in the stack).

From the header of polyMesh we see that the purpose of this function is to "Calculate the valid directions in the mesh from the boundaries".

My guess is that you mesh has a problem. Did you do a checkMesh?

If you have a Debug-Version of OF-compiled the dump would also include the line number where it fails.

Hi Bernhard, I have a tetra
 

Hi Bernhard,

I have a tetrahedral mesh, and I did the the checkMesh which was working properly.Can you suggest some other alternative.

Thanks.
Mayank

I think I fixed it.I removed t
 

I think I fixed it.I removed the defaultFaces patch -which was set to empty- from the boundary file.Now the reactingFoam runs fine.

Hi Running a simple 2d conf
 

Hi

Running a simple 2d configuration with inlet/outlet and wall boundaries. The solver used is simple Foam with k-e model.
There is a error message

#1 Foam::sigFpe::sigFpeHandler(int)
#2 Uninterpreted: [0xffffe420]
#3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&)
#4 void Foam::divide<foam::fvpatchfield,>(Foam::GeometricF ield<double,>&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,> const&)
#5 Foam::tmp<foam::geometricfield<double,> > Foam::operator/<foam::fvpatchfield,>(Foam::tmp<foam::geometricfie ld<double,> > const&, Foam::GeometricField<double,> const&)
#6 Foam::turbulenceModels::kEpsilon::correct()
#7 main
#8 __libc_start_main

Hi! It happens at the first
 

Hi!

It happens at the first time-step, right?

Check k and epsilon. ALL their initial and boundary conditions should be non-zero (I think one of yours is zero and that's why you're getting a division by zero)

Hallo, I get a similar error
 

Hallo,
I get a similar error. I am using a modified multiphaseinterfoam solver and at the beginning it seems to run quite stable. But at once, after more than 20 timesteps, I get the following error message:
#0 Foam::error::printStack(Foam:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&)
#1 Foam::sigFpe::sigFpeHandler(int)
#2 Uninterpreted: [0xb7f75420]
#3 exp
#4 Foam::exp(Foam::Field<double>&, Foam::UList<double> const&)
#5 void Foam::exp<foam::fvpatchfield,>(Foam::GeometricFiel d<double,>&, Foam::GeometricField<double,> const&)
#6 Foam::tmp<foam::geometricfield<double,> > Foam::exp<foam::fvpatchfield,>(Foam::tmp<foam::geo metricfield<double,> > const&)
#7 main
#8 __libc_start_main
#9 Foam::regIOobject::readIfModified()
Can anybody tell me what this message means or give me a hint where I have to look for the mistake?
Greetings,
Karl-Heinz

Because this seems to be a ver
 

Because this seems to be a very popular topic I have added a (very sparse) entry to the FAQ:
http://openfoamwiki.net/index.php/Main_FAQ (currently section 8.2 - the Message-Board-Software doesn't allow me to post the comple URL)

@karl-heinz: Don't know what could be your concrete problem

Hi All, I get a similar err
 

Hi All,

I get a similar error when running my model (modified sonicFoam):

Courant Number mean: 0.11819 max: 0.567546
deltaT = 1
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG: Solving for Ux, Initial residual = 0.00509694, Final residual = 4.28543e-18, No Iterations 4
DILUPBiCG: Solving for Uy, Initial residual = 0.00546863, Final residual = 5.27391e-18, No Iterations 4
DILUPBiCG: Solving for Uz, Initial residual = 0.000589589, Final residual = 6.26821e-19, No Iterations 4
DILUPBiCG: Solving for e, Initial residual = 1.07501e-05, Final residual = 1.36064e-16, No Iterations 3
DILUPBiCG: Solving for p, Initial residual = 0.0236798, Final residual = 1.93664e-16, No Iterations 4
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 8.73984e-16, global = -4.91172e-16, cumulative = 1.227e-13
DILUPBiCG: Solving for p, Initial residual = 0.00283702, Final residual = 1.0908e-17, No Iterations 4
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.61059e-16, global = 2.10885e-17, cumulative = 1.22721e-13
#0 Foam::error::printStack(Foam:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&)
#1 Foam::sigFpe::sigFpeHandler(int)
#2 Uninterpreted: [0x271420]
#3 log10
#4 Foam::log10(Foam::Field<double>&, Foam::UList<double> const&)
#5 void Foam::log10<foam::fvpatchfield,>(Foam::GeometricFi eld<double,>&, Foam::GeometricField<double,> const&)
#6 Foam::tmp<foam::geometricfield<double,> > Foam::log10<foam::fvpatchfield,>(Foam::tmp<foam::g eometricfield<double,> > const&)
#7 main
#8 __libc_start_main
#9 Foam::regIOobject::readIfModified()
Floating point exception


Am I correct in saying it is an error with the value passed to the log10 function? The only error I can think of for this is a value <= 0. However, in my output leading up to the error the field of concern is increasing to large values. Is there a limit to the value that the log10 function can take?

Thanks

Shaun

Hi everyone, Got the same t
 

Hi everyone,

Got the same trouble, which is not good. Checked posted FAQ, but that DOES NOT help much.

I tried to run the same example twice on the cluster machine. Both times parallel computation stopped at the same time around 2.6 second.

Here I attach links to the last 200 output lines from both runs, so one can compare them. They generally look almost identical:
http://www2.hawaii.edu/~krystian/tankTest/sample
http://www2.hawaii.edu/~krystian/tankTest/sample2

Also, here is the TecPlot plot for the last step where data were written (2.6s). Computation actually broke for 2.617s.
http://www2.hawaii.edu/~krystian/tankTest/tankflume.png

Hope we will be able to solve that problem. Tomorrow, I will check the same example running on my Mac machine (no parallelization - single machine) - hope it finished.

Krystian

Your time step is 10e-11 secon
 

Your time step is 10e-11 seconds that's picoseconds, which is unlikely to be right. I think your simulation blew up beforehand (due to setup or choice of numerics errors) and this is just the automatic time-step control unsuccessfully trying to save you.

Have a CLOSE look at your case and the last results before delta t started going ridiculously small.

Hrv

Today, friend of mine more fam
 

Today, friend of mine more familiar with CFD is going to take a look at my results, so I could verify my setup.

However, I think there is something more which could be wrong.
The same example runs with OpenFOAM-1.3 on my Mac machine and it already passed the 2.617 threshold and runs further - however computation is very long, already 3 days, but I blame this on computer hardware.

I think the problem lies somewhere else.

Krystian

Mistake found. Will run it aga
 

Mistake found. Will run it again and will see what happens.

But anyway, the robust code should produce something else than just error::printStack.

Hi all, I have a slightly d
 

Hi all,

I have a slightly different error message for a buoyantSimpleFoam calcualation:

Time = 1

DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 7.69481e-06,
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 1.58066e-06,
DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 7.40929e-06,
#0 Foam::error::printStack(Foam:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&)
#1 Foam::sigFpe::sigFpeHandler(int)
#2 ??
#3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<d
#4 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::surfaceMesh
Field, Foam::surfaceMesh> const&, Foam::tmp<Foam::GeometricField<double, Foam::f
#5 main
#6 __libc_start_main
#7 __gxx_personality_v0 at ../sysdeps/i386/elf/start.S:122
Floating exception

Unfortunately, I am not quite sure, what it means!? I checked the initial and boundary conditions, but say look ok.
Does anyone have an idea, where I have to look at?

Regards!
Fabian

I bet it is a floating point e
 

I bet it is a floating point exception: division by zero. Try

setenv FOAM_SIGFPE 1

and run it again. Precisely why you are trying to divide by zero might be a bit more difficult to find.

Hrv

Hi Hrv, I did set the FOAM_
 

Hi Hrv,

I did set the FOAM_SIGFPE to one... it is the error message above.
I would say, the messages says, that the boundary condition for the temperature is wrong (at least it occurs, when starting to calculate the energy equation), but I set all temperatures around 300K for the initial field and the inlets. Strange!?

Regards!
Fabian

What is the initial value of t
 

What is the initial value of the internal field?

Hrv

Uniform 300 for the internal a
 

Uniform 300 for the internal and 299 and 301 for the 6 inlets.

Fabian

Hi, is there something else I
 

Hi,
is there something else I might have to look at? Maybe, I should set the initial field using an old simpleFoam calculation ... I'll try it...

Fabian

Hi Fabian! As your calculat
 

Hi Fabian!

As your calculation went through the UEqn.H it seems to me that the problem might be in hEqn.H. There are two divisions by rho (which in turn is computed from p, I think). Question: is it possible that your initial p-Field is zero somewhere? (a favourite with compressible solvers)

Bernhard

Hi Bernhard, the the intern
 

Hi Bernhard,

the the internal p-field is set to 100000; that is not the problem!?

Regards!
Fabian

P.S. Nice PyFoam-Tool!
Do you plan further version with more features? I am looking for a small python-gui which handles bc, importing, cloning, etc. :-)

sorry, for waisting your time.
 

sorry, for waisting your time...
but for 'compressible' I have to set the pressure outlets too. Stupid! Thanks for the help, it runs now ...

Hi Fabian! Yep. Boundaries
 

Hi Fabian!

Yep. Boundaries too. That's what I meant with 'somewhere' ;)

@PyFoam: Thanks. I am adapting PyFoam constantly on a as-needed basis for my projects and plan to publish new versions on the Wiki. My emphasis is on stuff that helps me to automatize tasks (==scripting) so right now I have nothing planned GUI-wise (there is a graphical blockMesh-viewer, that might be in the next version, but apart from that: no)

Hi Bernhard, @PyFoam: I am
 

Hi Bernhard,

@PyFoam:
I am actually a big fan of scripting too, but as more scripts one is creating, as worse it gets to handle them ... and then a fast keyboard driven gui can help a lot. Especially Python is 'wonderful' in this sense; you can easily connect the existing scripts together. I actually use an own keyboard -driven file manager, written in python-gtk, for collecting my small scripts. Actually I started to integrate your pyfoam-scripts, but I don't have any idea, how I could handle the setup of boundary conditions... the FoamX approach is pretty much mouse-driven.

Regards!
Fabian

Hi everybody, I'm a new Ope
 

Hi everybody,

I'm a new OpenFoam user. I think I have a problem in my analysis on a naca profile, maybe with the turbulence model k-e, since I get this message on the terminal when I try to start the code:

.....
Creating turbulence model

Selecting turbulence model kEpsilon
#0 Foam::error::printStack(Foam:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&) in "/home/nettis/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/nettis/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib64/libc.so.6"
#3 Foam::compressible::turbulenceModels::kEpsilon::kE psilon(Foam::GeometricField<do uble,> const&, Foam::GeometricField<foam::vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double,> const&, Foam::basicThermo&) in "/home/nettis/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libcompressibleTurbule nceModels.so"
#4 Foam::compressible::turbulenceModel::adddictionary ConstructorToTable<foam::compr essible::turbulencemodels::kepsilon>::New(Foam::Ge ometricField<double,> const&, Foam::GeometricField<foam::vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double,> const&, Foam::basicThermo&) in "/home/nettis/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libcompressibleTurbule nceModels.so"
#5 Foam::compressible::turbulenceModel::New(Foam::Geo metricField<double,> const&, Foam::GeometricField<foam::vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double,> const&, Foam::basicThermo&) in "/home/nettis/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libcompressibleTurbule nceModels.so"
#6 main in "/home/nettis/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linux64GccDPOpt/rhoTurbFo am"
#7 __libc_start_main in "/lib64/libc.so.6"
#8 Foam::regIOobject::readIfModified() in "/home/nettis/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linux64GccDPOpt/rhoTurbFo am"

Actually I do not know if everything is ok with the grid imported from gambit, but I'm not sure it
is the cause of this issue.
Thank you in advance.

Regards,

Dino

Check whether this is a case o
 

Check whether this is a case of "k or epsilon is zero on some boundary or as the initial condition and OF doesn't like this". That is a very popular mistake with beginners

Hi Bernhard, you were right
 

Hi Bernhard,

you were right!! but now I'm facing with another problem: which values of k and epsilon I have to set as initial condition?? Have you got some suggestions??
Thank you very much,

Dino

Hi everyone I'm using interFo
 

Hi everyone
I'm using interFoam. I turned off the adjustable timestep since it grew ridiculously small after some time and set it to 10e-4 (which was ok in Fluent). But after some time (0,09 seconds) the calculation stops giving this error message.

MULES: Solving for gamma
#0 Foam::error::printStack(Foam:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&) in "/opt/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/opt/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 __restore_rt at sigaction.c:0
#3 void Foam::MULES::limiter<foam::onefield,>(Foam::Field< double>&, Foam::oneField const&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,> const&, Foam::zeroField const&, Foam::zeroField const&, double, double, int) in "/opt/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so"
#4 void Foam::MULES::explicitSolve<foam::onefield,>(Foam:: oneField const&, Foam::GeometricField<double,>&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,>&, Foam::zeroField const&, Foam::zeroField const&, double, double) in "/opt/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so"
#5 Foam::MULES::explicitSolve(Foam::GeometricField<do uble,>&, Foam::GeometricField<double,> const&, Foam::GeometricField<double,>&, double, double) in "/opt/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libfiniteVolume.so"
#6 main in "/opt/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/interFoam"
#7 __libc_start_main in "/lib64/libc.so.6"
#8 Foam::regIOobject::readIfModified() in "/opt/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/interFoam"
Floating point exception

I can't figure out where the problem is. Maybe it has something to do with the timestep, since, as I already said, it turned very small when it was adjustable. But the small timestep is of no use to me either (it was about 10e-30 s), that'w why I turned it off and set it to a fix value.
Can anyone help me?
Cheers, Sara

error
 

Hi,
i am building a new solver for steady computation of electrohydrodynamic flow and for the purpose i have combined electrostatic solver and simpleFoam solver.I am getting the following error and i don't know how to solve it,so if anyone has any idea please let me know:
Starting iteration loop

Iteration = 1

smoothSolver: Solving for Ux, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver: Solving for Uy, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver: Solving for Uz, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0, global = 0, cumulative = 0
DICPCG: Solving for V, Initial residual = 1, Final residual = 0.192654, No Iterations 2
#0 Foam::error::printStack(Foam::Ostream&) in "/home/rahul/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/rahul/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Uninterpreted:
#3 Foam::DILUPreconditioner::calcReciprocalD(Foam::Fi eld<double>&, Foam::lduMatrix const&) in "/home/rahul/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#4 Foam::DILUPreconditioner::DILUPreconditioner(Foam: :lduMatrix::solver const&, Foam::dictionary const&) in "/home/rahul/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#5 Foam::lduMatrix::preconditioner::addasymMatrixCons tructorToTable<Foam::DILUPreconditioner>::New(Foam ::lduMatrix::solver const&, Foam::dictionary const&) in "/home/rahul/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#6 Foam::lduMatrix::preconditioner::New(Foam::lduMatr ix::solver const&, Foam::dictionary const&) in "/home/rahul/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#7 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/rahul/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#8 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/home/rahul/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libfiniteVolume.so"
#9 Foam::lduMatrix::solverPerformance Foam::solve<double>(Foam::tmp<Foam::fvMatrix<doubl e> > const&) in "/home/rahul/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxGccDPOpt/ehdFoam"
#10 main in "/home/rahul/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxGccDPOpt/ehdFoam"
#11 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#12 _start at /build/buildd/eglibc-2.10.1/csu/../sysdeps/i386/elf/start.S:122
Floating point exception

Previously I built an unsteady solver for the same problem and mesh,and it works fine,so there shouldn't be any mesh related trouble like aspect ratio...
thanks and regards,
rudy

Hi OF-users,

I have recently installed OpenFOAM-1.6.x with Linux 11.2.

I think that the installation is fine.

I am not able to run the MRFSimpleFoam solver. So I have decided to check with the mixervessel2D tutorial.

I have the following error message when running the mixer 2D tutorial :

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.6.x |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 1.6.x-f3456b234025
Exec : MRFSimpleFoam
Date : Jan 06 2010
Time : 16:42:36
Host : cfs10
PID : 16108
Case : /shared/sanchi/mixerVessel2D
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

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

Create mesh for time = 0

Reading field p

#0 Foam::error::printStack(Foam::Ostream&) in "/shared/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigSegv::sigSegvHandler(int) in "/shared/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib64/libc.so.6"

Advices are welcome. Need help !

I need help to solve this problem.

Best regards,

Stephane

Hi,

Inside the mixervessel2D directory when I do ./Allrun I get the following error message :

[170]cfs10-sanchi /shared/sanchi/mixerVessel2D_1.6.x % ./Allrun
+ m4
+ blockMesh
+ cellSet
+ setsToZones -noFlipMap
Running MRFSimpleFoam on /shared/sanchi/mixerVessel2D_1.6.x
/shared/OpenFOAM/OpenFOAM-1.6.x/bin/tools/RunFunctions: line 38: 13644 Segmentation fault $APP_RUN $* > log.$APP_NAME 2>&1

I hope that it could help to solve my problem !!!

Thanks,

Stephane

Hi,

I discover the problem.

For OpenFOAM-1.6.x and OpenSUSE 11.2 I have to use the system compiler.

So I just have forgotten to recompile MRFSimpleFoam too.

cd ~/OpenFOAM/OpenFOAM-1.6.x/tutorials/incompressible/MRFSimpleFoam
wmake

and now MRFSimpleFoam works again.

Regards,

Stephane.

Same Problem with my solver
 

Hi everybody,
I have same problem too. I have just developed my own reacting solver for a specific case( combustion). And I get the same floating point exception error. Can any body help me with this.
My solver is based on IcoFoam, plus there is one property transport equations for Temperature, and three different equations for N2, Fuel, O2. the heat source is based on Arrhenious formula for rate of reaction, and simmilar sink term for Fuel and O2, But I get the same error. Can any body tell me what the problem is, and how I can fix this. The mesh is 2d, and this error happens when the temperature rises and reaction happens, If I keep the temperature low, no reaction happens and There will be no error.
The Error message is:

#0 Foam::error:: printStack(Foam::Ostream&) in "/home/harish/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/harish/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Uninterpreted:
#3 ?? in "/lib/tls/i686/cmov/libm.so.6"
#4 pow in "/lib/tls/i686/cmov/libm.so.6"
#5 Foam:: pow(Foam::Field<double>&, Foam::UList<double> const&, double const&) in "/home/harish/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#6 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::pow<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<doub le, Foam::fvPatchField, Foam::volMesh> > const&, Foam::dimensioned<double> const&) in "/home/harish/OpenFOAM/harish-1.6/applications/bin/linuxGccDPOpt/MyIncombFoam"
#7 main in "/home/harish/OpenFOAM/harish-1.6/applications/bin/linuxGccDPOpt/MyIncombFoam"
#8 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#9 _start in "/home/harish/OpenFOAM/harish-1.6/applications/bin/linuxGccDPOpt/MyIncombFoam"
Floating point exception

Hi friends,
I try to run RANS. I input a 3D meshed geometry into Open-Foam.
after runing for few time step, it gives me eror.
I am a new user (OpenFoam 1.6x), pleas help me.

the errors are as follows:

Starting time loop

Time = 1

DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.000508485, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.000139666, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.000140066, No Iterations 1
DICPCG: Solving for p, Initial residual = 1, Final residual = 0.00925416, No Iterations 123
DICPCG: Solving for p, Initial residual = 0.012907, Final residual = 0.000126943, No Iterations 27
DICPCG: Solving for p, Initial residual = 0.00398529, Final residual = 3.14156e-05, No Iterations 116
DICPCG: Solving for p, Initial residual = 0.00182828, Final residual = 1.79837e-05, No Iterations 26
DICPCG: Solving for p, Initial residual = 0.00074565, Final residual = 6.59969e-06, No Iterations 114
DICPCG: Solving for p, Initial residual = 0.000358352, Final residual = 3.48877e-06, No Iterations 24
time step continuity errors : sum local = 3.17637e-05, global = -1.50157e-06, cumulative = -1.50157e-06
#0 Foam::error::printStack(Foam::Ostream&) in "/home/azadeh/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/azadeh/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib/libc.so.6"
#3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/home/azadeh/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 void Foam::divide<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/home/azadeh/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#5 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::operator/<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<doub le, Foam::fvPatchField, Foam::volMesh> > const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/home/azadeh/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#6 Foam::incompressible::RASModels::kEpsilon::correct () in "/home/azadeh/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#7 main in "/home/azadeh/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/simpleFoam"
#8 __libc_start_main in "/lib/libc.so.6"
#9 _start at /build/buildd/eglibc-2.10.1/csu/../sysdeps/x86_64/elf/start.S:116
Floating point exception

I FOUND IT :)
Just "k" ahouldn't be 0.

hi,
i have the same error message like some guys before me. I was reading in the forum, but i don´t understand the error.

poopak999 sayed that k don´t can be zero. When i go to the 0-Folder in the k-file my k has the value "uniform 3.75e-04". so it isen´t zero.

Maybe someone can help me?

greets

almir

Hello all,

I successfully ran a series of simulations using simpleFoam to set up my case, and now I want to complicate things by moving to sonicFoam. 9 iterations ran successfully, but #10 produced an impressive series of errors:

Later on it says "floating point exception".

That's not the half of it... I included the whole log file in the attachment. Can anyone suggest what the problem might be? After reviewing the previous posts, I have already verified that all of my turbulence coeffs and pressures are non-zero.

Thanks,

Dan

On the meaning of the stack-trace and how to get more detailed information (by compiling a debug-version) see:
http://openfoamwiki.net/index.php/Ma...:Ostream.26.29
(and the point above it).

Anyway. You seem to have a parallel run there. Try running it in serial and see if the problem is also there.

Apart from that there is much I can tell you (maybe some kind soul has a look at your log-file)

Thank you for your assistance, Bernhard. It turns out that the simulation ran just fine in serial. I implemented one change each to /etc/config/settings.sh and /etc/bashrc in accordance with the references below, and now it appears to run well.

Regards,

Dan

Ref 1: http://www.cfd-online.com/Forums/ope...-problems.html
Ref 2: http://www.cfd-online.com/Forums/ope...exception.html