|
[Sponsors] |
sonicFoam - Floating point eception (core dumped) |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
November 17, 2014, 12:04 |
sonicFoam - Floating point eception (core dumped)
|
#1 |
New Member
Marc
Join Date: Nov 2014
Location: Barcelona, Catalonia (still Spain)
Posts: 7
Rep Power: 12 |
Hello everyone!
I am working with a 3D nozzle. First of all I ran simpleFoam with no further issues but after introducing compressibility and turbulence it's when problems appear. The error is ot FOAM FATAL ERROR as usual. The exact script is the following: //////////////////////////////////////////////////////////////////////////////////////////////////////////////////////////// Create time Create mesh for time = 0 Reading thermophysical properties Selecting thermodynamics package ePsiThermo<pureMixture<constTransport<specieThermo <eConstThermo<perfectGas>>>>> Reading field U Reading/calculating face flux field phi Creating turbulence model Selecting turbulence model type RASModel Selecting RAS turbulence model laminar Starting time loop Time = 0.05 #0 Foam::error:: PrintStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/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 "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #4 Foam:: operator/(Foam::UList<double> const&, Foam::UList<double> const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #5 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/sonicFoam" #6 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" #7 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/sonicFoam" Floating point exception (core dumped) /////////////////////////////////////////////////////////////////////////////////////////////////////////////////////////////// I've seen in other posts that dicreasing the deltaT sometimes works but already tried with no better results. Does ayone know what's this all about and how could I solve this? Thank you very much! Marc |
|
November 17, 2014, 12:31 |
|
#2 |
Senior Member
|
Hi,
as the error happens during Courant number calculation (according to your output) Code:
scalarField sumPhi ( fvc::surfaceSum(mag(phi))().internalField() / rho.internalField() ); CoNum = 0.5*gMax(sumPhi/mesh.V().field())*runTime.deltaTValue(); meanCoNum = 0.5*(gSum(sumPhi)/gSum(mesh.V().field()))*runTime.deltaTValue(); |
|
November 17, 2014, 14:04 |
|
#3 |
New Member
Marc
Join Date: Nov 2014
Location: Barcelona, Catalonia (still Spain)
Posts: 7
Rep Power: 12 |
Thank you Alexey.
So, assuming (and hoping) it's not a 0-volume-cell problem (simpleFoam ran with no problem and it would have appeared then too, isn't it?) it most probably is a problem with density. Then, how can I fix it? is it just due to a certain value I should increase or decrease or it comes from combining pressure, velocity and temperature to satisfy Bernoulli's equation? Thank you, Marc |
|
November 17, 2014, 15:02 |
|
#4 |
Senior Member
|
Well, if we take a look at createFields.H:
Code:
Info<< "Reading thermophysical properties\n" << endl; autoPtr<psiThermo> pThermo ( psiThermo::New(mesh) ); psiThermo& thermo = pThermo(); thermo.validate(args.executable(), "e"); volScalarField& p = thermo.p(); volScalarField& e = thermo.he(); const volScalarField& psi = thermo.psi(); volScalarField rho ( IOobject ( "rho", runTime.timeName(), mesh ), thermo.rho() ); Code:
Foam::tmp<Foam::volScalarField> Foam::psiThermo::rho() const { return p_*psi_; } |
|
November 17, 2014, 18:45 |
|
#5 |
New Member
Marc
Join Date: Nov 2014
Location: Barcelona, Catalonia (still Spain)
Posts: 7
Rep Power: 12 |
But, as p is set as fixedValue and psi is the compressibility (psi=(rho*T*R)/W where rho is density, T temperature, R is the constant of gases and W not 100% sure what it exactly is but its units must be 1/mol) and all the variables come from the thermoPhysicalProperties document and those are constants, the only option is that at the very begining of the iterative process (this is why the terminal crashes at the first time loop), rho is set as 0 and it leads to psi=0 so rho* is again =0 and it makes my core dump.
Thank you very much Alexey! But now (and this is the very last issue I bother you with, I hope) where can I change this initial value of rho? |
|
November 18, 2014, 03:12 |
|
#6 |
Senior Member
|
Well,
post your 0 folder and thermophysicalProperties, otherwise it'll be just speculations. |
|
November 18, 2014, 04:42 |
|
#7 |
Senior Member
Join Date: Oct 2013
Posts: 397
Rep Power: 19 |
Without having looked very much into your problem, crashes can occur because of too large time steps or in unconverged solutions. Did you try lowering the time step size?
|
|
November 18, 2014, 06:28 |
|
#8 |
New Member
Marc
Join Date: Nov 2014
Location: Barcelona, Catalonia (still Spain)
Posts: 7
Rep Power: 12 |
Hello Chris, yes, I already tried but that's not the problem. Thank you anyway for taking a look at my post and try to help.
Alexey, here I leave you my 0 folder and the thermophysicalProperties (this is directly copied from the sonicFoam airfiol tutorial, though) |
|
November 18, 2014, 06:52 |
|
#9 |
Senior Member
|
Hi,
if you take a look at your p file: Code:
... dimensions [0 2 -2 0 0 0 0]; internalField uniform 0; ... |
|
November 19, 2014, 05:22 |
|
#10 |
New Member
Marc
Join Date: Nov 2014
Location: Barcelona, Catalonia (still Spain)
Posts: 7
Rep Power: 12 |
Oh dear... it sounded so stupid and so obvious that seemed it had to work but didn't... It's true that we could go a bit forward. Following the steps sonicFoam follows when solving I've seen it crashes when it tries to calculate density
(or just after it but without having the right value (it leaves rho=0) and has to divide by it. Dividing by 0 -> core dumped). Now the code is: // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Reading thermophysical properties Selecting thermodynamics package ePsiThermo<pureMixture<constTransport<specieThermo <eConstThermo<perfectGas>>>>> Reading field U Reading/calculating face flux field phi Creating turbulence model Selecting turbulence model type RASModel Selecting RAS turbulence model laminar Starting time loop Time = 5e-05 Courant Number mean: 0.000373442 max: 0.00330131 #0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/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 "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #4 Foam:perator/(Foam::UList<double> const&, Foam::UList<double> const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #5 Foam::diagonalSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #6 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so" #7 Foam::fvMatrix<double>::solve() in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/sonicFoam" #8 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/sonicFoam" #9 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" #10 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/sonicFoam" Floating point exception (core dumped) ////////////////////////////////////////////////////////////////////////////////////////////////////////////// I've been trying to find where the error is and changed some parameters but ,sadly, it was not effective. I am sure there is another stupid mistake like the one with the pressure but I am not able to find it. I leave you here the full case so you can take a look at it (if you can). I removed polyMesh and trisurface from the constant folder just due to a folder-size problem Thank you! |
|
November 19, 2014, 07:03 |
|
#11 |
Senior Member
|
Well, sonicFoam is transient solver, not quite sure it likes this
Code:
ddtSchemes { default steadyState; } |
|
November 19, 2014, 16:54 |
|
#12 |
New Member
Marc
Join Date: Nov 2014
Location: Barcelona, Catalonia (still Spain)
Posts: 7
Rep Power: 12 |
Awesome!
After changing it to Euler and adjusting FvSchemes and FvSolution to it, finally worked! I am really really grateful Thank you very much Alexey! Marc |
|
August 4, 2015, 06:10 |
|
#13 |
New Member
Ipos
Join Date: Feb 2015
Posts: 7
Rep Power: 11 |
Hi
I have a problem with running rhoPorousSimpleFoam. I used Gambit to generated mesh and export 3D mesh to OpenFoam. #0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam221/platforms/linuxGccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam221/platforms/linuxGccDPOpt/lib/libOpenFOAM.so" #2 Uninterpreted: #3 Foam::heRhoThermo<Foam::rhoThermo, Foam:ureMixture<Foam::sutherlandTransport<Foam:: species::thermo<Foam::hConstThermo<Foam:erfectGa s<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::calculate() in "/opt/openfoam221/platforms/linuxGccDPOpt/lib/libfluidThermophysicalModels.so" #4 Foam::heRhoThermo<Foam::rhoThermo, Foam:ureMixture<Foam::sutherlandTransport<Foam:: species::thermo<Foam::hConstThermo<Foam:erfectGa s<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::correct() in "/opt/openfoam221/platforms/linuxGccDPOpt/lib/libfluidThermophysicalModels.so" #5 in "/opt/openfoam221/platforms/linuxGccDPOpt/bin/rhoPorousSimpleFoam" #6 __libc_start_main in "/lib/i386-linux-gnu/libc.so.6" #7 in "/opt/openfoam221/platforms/linuxGccDPOpt/bin/rhoPorousSimpleFoam" Floating point exception (core dumped) |
|
Tags |
core dumped, floating point, sonicfoam |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
icoFoam - Floating point exception (core dumped) | File | OpenFOAM Running, Solving & CFD | 26 | March 6, 2021 05:26 |
[snappyHexMesh] How to define to right point for locationInMesh | Mirage12 | OpenFOAM Meshing & Mesh Conversion | 7 | March 13, 2016 15:07 |
Floating point exception (core dumped) | Punt3r | OpenFOAM Running, Solving & CFD | 1 | September 3, 2013 09:51 |
Floating point error and divergence detected | aannjj | FLUENT | 0 | July 2, 2013 04:44 |
a reconstructPar issue | immortality | OpenFOAM Post-Processing | 8 | June 16, 2013 12:25 |