CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Bugs (http://www.cfd-online.com/Forums/openfoam-bugs/)
-   -   Latest git 1.6.x: Crash when using inletOutlet for variable alpha1 in interFoam (http://www.cfd-online.com/Forums/openfoam-bugs/68464-latest-git-1-6-x-crash-when-using-inletoutlet-variable-alpha1-interfoam.html)

carsten September 21, 2009 09:07

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:

henry September 22, 2009 04:37

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

H

carsten September 22, 2009 07:04

1 Attachment(s)
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

henry September 23, 2009 03:16

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

carsten September 23, 2009 04:49

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

gschaider September 23, 2009 09:18

Quote:

Originally Posted by carsten (Post 230244)
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 ;)

carsten September 23, 2009 09:46

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


All times are GMT -4. The time now is 12:03.