rhoSimpleFoam error
 

I can't make heads or tails of this:

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.1.0-0bc225064152
Exec : rhoSimpleFoam
Date : Jun 05 2012
Time : 18:14:23
Host : "ubufoam"
PID : 2126
Case : /home/mihai/OpenFOAM/mihai-2.1.0/run/comprestud/sduct-vanes_100_inlet_vel_smoothallVG
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

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

Create mesh for time = 0


SIMPLE: convergence criteria
field p tolerance 1e-05
field U tolerance 1e-05
field k tolerance 1e-05
field omega tolerance 1e-05

Reading thermophysical properties

Selecting thermodynamics package hPsiThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<perfectGas>>>>>
Reading field U

Reading/calculating face flux field phi

Creating turbulence model

Selecting RAS turbulence model kEpsilon
#0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam210/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam210/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#2 Uninterpreted:
#3 Foam::compressible::RASModels::mutkWallFunctionFvP atchScalarField::calcMut() const in "/opt/openfoam210/platforms/linuxGccDPOpt/lib/libcompressibleRASModels.so"
#4 Foam::compressible::RASModels::mutkWallFunctionFvP atchScalarField::updateCoeffs() in "/opt/openfoam210/platforms/linuxGccDPOpt/lib/libcompressibleRASModels.so"
#5 Foam::fvPatchField<double>::evaluate(Foam::UPstrea m::commsTypes) in "/opt/openfoam210/platforms/linuxGccDPOpt/bin/rhoSimpleFoam"
#6 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::evaluate() in "/opt/openfoam210/platforms/linuxGccDPOpt/bin/rhoSimpleFoam"
#7 Foam::compressible::RASModels::kEpsilon::kEpsilon( Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&, Foam::word const&, Foam::word const&) in "/opt/openfoam210/platforms/linuxGccDPOpt/lib/libcompressibleRASModels.so"
#8 Foam::compressible::RASModel::adddictionaryConstru ctorToTable<Foam::compressible::RASModels::kEpsilo n>::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&, Foam::word const&) in "/opt/openfoam210/platforms/linuxGccDPOpt/lib/libcompressibleRASModels.so"
#9 Foam::compressible::RASModel::New(Foam::GeometricF ield<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&, Foam::word const&) in "/opt/openfoam210/platforms/linuxGccDPOpt/lib/libcompressibleRASModels.so"
#10
in "/opt/openfoam210/platforms/linuxGccDPOpt/bin/rhoSimpleFoam"
#11 __libc_start_main in "/lib/i386-linux-gnu/libc.so.6"
#12
in "/opt/openfoam210/platforms/linuxGccDPOpt/bin/rhoSimpleFoam"
Floating point exception


extract from my mut:

note that this occurs even when I delete the mut file to let openfoam create it

What do you want to do with entries like

value nonuniform 0();

Shouldn't it be "uniform 0;". Note that 0() indicates a list with zero elements and the format would be different (using the List keyword).

Hello,

As pointed out by Alberto, you probably have some troubles with your mesh. Try at least to check it with checkMesh. You should not have patches without faces.

A question: have you created mut yourself or was it generated by OpenFOAM?

Regards

Thanks for the replies.
Using the squarebend tutroial for inspiration I got it running and then ....

Time = 95

GAMG: Solving for Ux, Initial residual = 0.0114881, Final residual = 0.000226671, No Iterations 1
GAMG: Solving for Uy, Initial residual = 0.00116554, Final residual = 7.37184e-05, No Iterations 1
GAMG: Solving for Uz, Initial residual = 0.00832338, Final residual = 0.000335954, No Iterations 1
GAMG: Solving for p, Initial residual = 0.00431245, Final residual = 0.000296092, No Iterations 3
time step continuity errors : sum local = 0.520895, global = 0.309596, cumulative = -102.181
rho max/min : 1 0.1
GAMG: Solving for h, Initial residual = 0.00496736, Final residual = 0.000138371, No Iterations 1
#0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::hPsiThermo<Foam::pureMixture<Foam::sutherlan dTransport<Foam::specieThermo<Foam::hConstThermo<F oam::perfectGas> > > > >::calculate() in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#4 Foam::hPsiThermo<Foam::pureMixture<Foam::sutherlan dTransport<Foam::specieThermo<Foam::hConstThermo<F oam::perfectGas> > > > >::correct() in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"



The crash coincides with a drop in rho min from 0.36 to 0.1

I introduced a cell limiter which has worked well before for a similar issue (see picture of rho at time 90 without cell limiter) and now it crashes at time 7 with rho min dropping precipitously.

Time = 6

GAMG: Solving for Ux, Initial residual = 0.145982, Final residual = 0.0052821, No Iterations 2
GAMG: Solving for Uy, Initial residual = 0.0834204, Final residual = 0.00275481, No Iterations 2
GAMG: Solving for Uz, Initial residual = 0.238371, Final residual = 0.00817188, No Iterations 2
GAMG: Solving for p, Initial residual = 0.0487939, Final residual = 0.00479841, No Iterations 4
time step continuity errors : sum local = 9.63164, global = 4.62693, cumulative = -66.2753
rho max/min : 1 0.951644
GAMG: Solving for h, Initial residual = 0.166241, Final residual = 0.0139909, No Iterations 1
GAMG: Solving for epsilon, Initial residual = 0.0241813, Final residual = 0.000738986, No Iterations 2
GAMG: Solving for k, Initial residual = 0.0415477, Final residual = 0.00268973, No Iterations 2
ExecutionTime = 357.6 s ClockTime = 371 s

Time = 7

GAMG: Solving for Ux, Initial residual = 0.115854, Final residual = 0.00403452, No Iterations 2
GAMG: Solving for Uy, Initial residual = 0.0659571, Final residual = 0.00218564, No Iterations 2
GAMG: Solving for Uz, Initial residual = 0.198465, Final residual = 0.00700925, No Iterations 2
GAMG: Solving for p, Initial residual = 0.0440085, Final residual = 0.00437184, No Iterations 41
time step continuity errors : sum local = 32.504, global = 0.667329, cumulative = -65.608
rho max/min : 1 0.2635
GAMG: Solving for h, Initial residual = 0.294754, Final residual = 0.0228699, No Iterations 1
#0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::hPsiThermo<Foam::pureMixture<Foam::sutherlan dTransport<Foam::specieThermo<Foam::hConstThermo<F oam::perfectGas> > > > >::calculate() in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#4 Foam::hPsiThermo<Foam::pureMixture<Foam::sutherlan dTransport<Foam::specieThermo<Foam::hConstThermo<F oam::perfectGas> > > > >::correct() in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#5
in "/opt/openfoam210/platforms/linux64GccDPOpt/bin/rhoSimplecFoam"
#6 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7
in "/opt/openfoam210/platforms/linux64GccDPOpt/bin/rhoSimplecFoam"
Floating point exception

the screenshot is of the density field an outlet with fixed pressure.

fixed it, I had zerogradient for Temperature at inlet and fixed value at outlet and it didn't like that, kinda "duh!" , switched them around and now it ran past the point where it was crashing.

Hello Mihai,

Happy for you that you fix the trouble. About the boundary conditions, when setting them, you always have to remember a basic rule:
For all fields except pressure, a value should be provided at the inlet (the code cannot know what's outside your domain ;) ). And at outlet, you should let the field go out - so usually zero gradient.
For the pressure it's the opposite due to the coupling velocity-pressure (the velocity is linked to the pressure gradient).

Regards,

yes, definitely!
I think that's what I had in mind, from the beginning, but I switched my patches by mistake.
To be honest, I haven't been spending much time looking at OpenFOAM input files lately, because I automated the case generation process for incompressible flows.
So when I got back to editing files, to make it work for compressible flows with SIMPLEC, I didn't realize that the outlet was listed before the inlet :)