CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Bugs

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

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 21, 2009, 09:07
Default Latest git 1.6.x: Crash when using inletOutlet for variable alpha1 in interFoam
  #1
Member
 
Carsten Thorenz
Join Date: Mar 2009
Location: Germany
Posts: 34
Rep Power: 8
carsten is on a distinguished road
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:
carsten is offline   Reply With Quote

Old   September 22, 2009, 04:37
Default
  #2
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
I am unable to reproduce the problem you are having with your case on the cases I have.

H
henry is offline   Reply With Quote

Old   September 22, 2009, 07:04
Default
  #3
Member
 
Carsten Thorenz
Join Date: Mar 2009
Location: Germany
Posts: 34
Rep Power: 8
carsten is on a distinguished road
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
Attached Files
File Type: zip inletOutlet_problem.zip (14.5 KB, 19 views)
carsten is offline   Reply With Quote

Old   September 23, 2009, 03:16
Default
  #4
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
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
henry is offline   Reply With Quote

Old   September 23, 2009, 04:49
Default
  #5
Member
 
Carsten Thorenz
Join Date: Mar 2009
Location: Germany
Posts: 34
Rep Power: 8
carsten is on a distinguished road
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

Last edited by carsten; September 23, 2009 at 07:04.
carsten is offline   Reply With Quote

Old   September 23, 2009, 09:18
Default
  #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
Quote:
Originally Posted by carsten View Post
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
gschaider is offline   Reply With Quote

Old   September 23, 2009, 09:46
Default
  #7
Member
 
Carsten Thorenz
Join Date: Mar 2009
Location: Germany
Posts: 34
Rep Power: 8
carsten is on a distinguished road
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

Last edited by carsten; September 23, 2009 at 10:02.
carsten 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


Similar Threads
Thread Thread Starter Forum Replies Last Post
Latest git 1.6.x : cellDistFuncs.H podallaire OpenFOAM Bugs 4 December 11, 2009 09:03


All times are GMT -4. The time now is 20:16.