CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   FoamerrorprintStack (http://www.cfd-online.com/Forums/openfoam-solving/58320-foamerrorprintstack.html)

mayank June 4, 2007 08:06

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.

gschaider June 4, 2007 11:25

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.

mayank June 5, 2007 03:33

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

mayank June 5, 2007 03:45

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.

knabhishek June 13, 2007 10:46

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

gschaider June 13, 2007 11:42

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)

khleitz June 14, 2007 02:39

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

gschaider June 14, 2007 08:03

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

coops July 8, 2007 23:17

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

paka July 9, 2007 03:51

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

hjasak July 9, 2007 04:02

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

paka July 9, 2007 16:02

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

paka July 9, 2007 22:27

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.

braennstroem July 29, 2007 03:43

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

hjasak July 29, 2007 04:00

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

braennstroem July 29, 2007 04:32

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

hjasak July 29, 2007 04:38

What is the initial value of t
 
What is the initial value of the internal field?

Hrv

braennstroem July 29, 2007 04:56

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

Fabian

braennstroem July 31, 2007 12:55

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

gschaider July 31, 2007 13:22

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


All times are GMT -4. The time now is 14:54.