Latest git 1.6.x: Crash when using inletOutlet for variable alpha1 in interFoam
 

Hi there,

as stated above, interFoam crashes if an inletOutlet-BC is used with for alpha1. The output is below. The same case works fine with zeroGradient.

Thanks for your time and efforts,

Carsten



thorenz@w3pc079: interFoam
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / 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-341652c705cd
Exec : interFoam
Date : Sep 21 2009
Time : 15:04:12
Host : w3pc079
PID : 10096
Case : /nfs/data_fsD/wasserbau/w3/_projekte_unix/thorenz/OpenFOAM/thorenz-1.6/run/rbtest2
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

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

Create mesh for time = 0


Reading g
Reading field p

Reading field alpha1

Reading field U

Reading/calculating face flux field phi

Reading transportProperties

Selecting incompressible transport model Newtonian
Selecting incompressible transport model Newtonian
Selecting turbulence model type laminar
time step continuity errors : sum local = 0, global = 0, cumulative = 0
GAMGPCG: Solving for pcorr, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0, global = 0, cumulative = 0
Courant Number mean: 0 max: 0

Starting time loop

Courant Number mean: 0 max: 0
deltaT = 0.00012
Time = 0.00012

#0 Foam::error::printStack(Foam::Ostream&) in "/home/thorenz/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/thorenz/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib64/libc.so.6"
#3 Foam::LimitedScheme<double, Foam::vanLeerLimiter<Foam::NVDTVD>, Foam::limitFuncs::magSqr>::limiter(Foam::Geometric Field<double, Foam::fvPatchField, Foam::volMesh> const&) const in "/home/thorenz/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libfiniteVolume.so"
#4 Foam::limitedSurfaceInterpolationScheme<double>::w eights(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) const in "/home/thorenz/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libinterfaceProperties.so"
#5 Foam::surfaceInterpolationScheme<double>::interpol ate(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) const in "/home/thorenz/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libinterfaceProperties.so"
#6 Foam::fv::gaussConvectionScheme<double>::interpola te(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) const in "/home/thorenz/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libfiniteVolume.so"
#7 Foam::fv::gaussConvectionScheme<double>::flux(Foam ::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) const in "/home/thorenz/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libfiniteVolume.so"
#8 Foam::tmp<Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> > Foam::fvc::flux<double>(Foam::GeometricField<doubl e, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::word const&) in "/home/thorenz/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/interFoam"
#9 main in "/home/thorenz/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/interFoam"
#10 __libc_start_main in "/lib64/libc.so.6"
#11 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/home/thorenz/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/interFoam"
Gleitkomma-Ausnahme
thorenz@w3pc079:

I am unable to reproduce the problem you are having with your case on the cases I have.

H

Hi Henry,

I can reproduce it on different machines. I attached a small test case (which is physically meaningless ...).

Please run

blockMesh
interFoam

in order to try to reproduce it.

Thank you for your time,

Carsten

In your specification of the inletOutlet BC for alpha1 you provide

value uniform -1.e9;

This is unphysical and causes the crash. If set to a physical value your case runs.

H

Sorry Henry,

but I do not understand. From my understanding the inletOutlet-BC uses "inletValue" for the definition of the value for the Dirichlet-personality of the BC, whereas the value for the Neumann-personality is always set to zero. Thus I assumed, "value" is a dummy with no meaning and can be set to any value. Obviously I was wrong here.

After looking into the source I have the impression that "value" superimposes "inletValue". But when running an example with both "value" and "inletValue" actually inletValue is beeing used. So why the crash if I set "value" to a ridiculous number?

Bye,

Carsten

The value IS used for the initial calculations (am not exactly an expert on the interFoam solver but I guess at least the density for the initial timestep is calculated by it) so always using physical conditions is a good idea ;)

Thanks Bernhard.

So it sets the initial conditions for the boundary patches. If it is used to compute initial densities, shouldn't there be a limiter? Hmm. Anyhow I'm not sure if this kind of crash should occur. But at least now I know how to avoid it :)

Thanks,

Carsten