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

FoamerrorprintStack

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   June 4, 2007, 08:06
Default hello all, I am using react
  #1
mayank
Guest
 
Posts: n/a
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:stream&)
#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.
  Reply With Quote

Old   June 4, 2007, 11:25
Default That means that it fails while
  #2
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
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.
__________________
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   June 5, 2007, 03:33
Default Hi Bernhard, I have a tetra
  #3
mayank
Guest
 
Posts: n/a
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
  Reply With Quote

Old   June 5, 2007, 03:45
Default I think I fixed it.I removed t
  #4
mayank
Guest
 
Posts: n/a
I think I fixed it.I removed the defaultFaces patch -which was set to empty- from the boundary file.Now the reactingFoam runs fine.
  Reply With Quote

Old   June 13, 2007, 10:46
Default Hi Running a simple 2d conf
  #5
New Member
 
abhishek k n
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 16
Rep Power: 8
knabhishek is on a distinguished road
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
knabhishek is offline   Reply With Quote

Old   June 13, 2007, 11:42
Default Hi! It happens at the first
  #6
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
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)
__________________
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   June 14, 2007, 02:39
Default Hallo, I get a similar error
  #7
New Member
 
Karl-Heinz Leitz
Join Date: Mar 2009
Posts: 16
Rep Power: 8
khleitz is on a distinguished road
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:stream&)
#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
khleitz is offline   Reply With Quote

Old   June 14, 2007, 08:03
Default Because this seems to be a ver
  #8
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
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
__________________
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   July 8, 2007, 23:17
Default Hi All, I get a similar err
  #9
Member
 
Shaun Cooper
Join Date: Mar 2009
Posts: 54
Rep Power: 8
coops is on a distinguished road
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:stream&)
#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
coops is offline   Reply With Quote

Old   July 9, 2007, 03:51
Default Hi everyone, Got the same t
  #10
Senior Member
 
Join Date: Mar 2009
Posts: 225
Rep Power: 9
paka is on a distinguished road
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
paka is offline   Reply With Quote

Old   July 9, 2007, 04:02
Default Your time step is 10e-11 secon
  #11
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,763
Rep Power: 21
hjasak will become famous soon enough
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
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   July 9, 2007, 16:02
Default Today, friend of mine more fam
  #12
Senior Member
 
Join Date: Mar 2009
Posts: 225
Rep Power: 9
paka is on a distinguished road
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 is offline   Reply With Quote

Old   July 9, 2007, 22:27
Default Mistake found. Will run it aga
  #13
Senior Member
 
Join Date: Mar 2009
Posts: 225
Rep Power: 9
paka is on a distinguished road
Mistake found. Will run it again and will see what happens.

But anyway, the robust code should produce something else than just error::printStack.
paka is offline   Reply With Quote

Old   July 29, 2007, 03:43
Default Hi all, I have a slightly d
  #14
Senior Member
 
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 10
braennstroem is on a distinguished road
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:stream&)
#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
braennstroem is offline   Reply With Quote

Old   July 29, 2007, 04:00
Default I bet it is a floating point e
  #15
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,763
Rep Power: 21
hjasak will become famous soon enough
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
mm.abdollahzadeh likes this.
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   July 29, 2007, 04:32
Default Hi Hrv, I did set the FOAM_
  #16
Senior Member
 
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 10
braennstroem is on a distinguished road
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
braennstroem is offline   Reply With Quote

Old   July 29, 2007, 04:38
Default What is the initial value of t
  #17
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,763
Rep Power: 21
hjasak will become famous soon enough
What is the initial value of the internal field?

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   July 29, 2007, 04:56
Default Uniform 300 for the internal a
  #18
Senior Member
 
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 10
braennstroem is on a distinguished road
Uniform 300 for the internal and 299 and 301 for the 6 inlets.

Fabian
braennstroem is offline   Reply With Quote

Old   July 31, 2007, 12:55
Default Hi, is there something else I
  #19
Senior Member
 
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 10
braennstroem is on a distinguished road
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
braennstroem is offline   Reply With Quote

Old   July 31, 2007, 13:22
Default Hi Fabian! As your calculat
  #20
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
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
__________________
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

Reply

Thread Tools
Display Modes

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 On
Pingbacks are On
Refbacks are On



All times are GMT -4. The time now is 04:08.