CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

reading transportProperties of multiphaseInterFoam Error

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

Like Tree1Likes
  • 1 Post By AbbasRahimi

Reply
 
LinkBack Thread Tools Display Modes
Old   February 3, 2016, 17:08
Default reading transportProperties of multiphaseInterFoam Error
  #1
New Member
 
Abbas Rahimi
Join Date: Jan 2013
Posts: 23
Rep Power: 5
AbbasRahimi is on a distinguished road
Hello everyone,

I'm trying to run multiphaseInterFoam for a case and I get this error. I wonder if anyone here can help me to overcome this error?

Thank you.



Create mesh for time = 0

Reading field p_rgh

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting incompressible transport model Newtonian
Selecting incompressible transport model Newtonian
Selecting incompressible transport model Newtonian
Selecting incompressible transport model Newtonian
#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 in "/lib64/libc.so.6"
#3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) at ??:?
#4 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam:perator/<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<doub le, Foam::fvPatchField, Foam::volMesh> > const&, Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&) at ??:?
#5 Foam::multiphaseMixture::multiphaseMixture(Foam::G eometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&) at ??:?
#6
at ??:?
#7 __libc_start_main in "/lib64/libc.so.6"
#8
at /usr/src/packages/BUILD/glibc-2.11.3/csu/../sysdeps/x86_64/elf/start.S:116
Floating exception
shincoast likes this.
AbbasRahimi is offline   Reply With Quote

Old   February 4, 2016, 05:27
Default
  #2
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,409
Rep Power: 24
alexeym will become famous soon enoughalexeym will become famous soon enough
Hi,

Answering your question: use correct initial conditions (or properties, maybe you have made a mistake there).

More detailed answer would be:

If you look at the error, you can find key word "divide":

Code:
#2 in "/lib64/libc.so.6"
#3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) at ??:?
#4 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam:perator/<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<doub le, Foam::fvPatchField, Foam::volMesh> > const&, Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&) at ??:?
In general this error happens when you try to divide something by 0. Error happened during construction of the mixture, so you go to $FOAM_APP/solvers/multiphase/multiphaseInterFoam/multiphaseMixture/multiphaseMixture.C and look into constructor of the class, the first division is here:

Code:
Foam::multiphaseMixture::multiphaseMixture
(
    const volVectorField& U,
    const surfaceScalarField& phi
)
:
...
    nu_
    (
        IOobject
        (
            "nu",
            mesh_.time().timeName(),
            mesh_
        ),
        mu()/rho()
    ),
...
and it means somewhere density is zero, so if you take a look at rho method:

Code:
Foam::tmp<Foam::volScalarField>
Foam::multiphaseMixture::rho() const
{
    PtrDictionary<phase>::const_iterator iter = phases_.begin();

    tmp<volScalarField> trho = iter()*iter().rho();

    for (++iter; iter != phases_.end(); ++iter)
    {
        trho() += iter()*iter().rho();
    }

    return trho;
}
iter() is alpha.phase_name volume field, tier().rho() is density of the phase, you have put into transportProperties. Which one is zero? I can only guess, yet you can try to find it in your case files.
alexeym is offline   Reply With Quote

Old   February 4, 2016, 05:41
Default
  #3
New Member
 
Abbas Rahimi
Join Date: Jan 2013
Posts: 23
Rep Power: 5
AbbasRahimi is on a distinguished road
Alexey,

Thank you for response. Your answer totally make sense but I double checked my transportProperties and couldn't find any rho=0 anywhere.


/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.3.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

phases
(
air
{
transportModel Newtonian;
nu nu [ 0 2 -1 0 0 0 0 ] 29.522;
rho rho [ 1 -3 0 0 0 0 0 ] 1129;
BirdCarreauCoeffs
{
nu0 nu0 [ 0 2 -1 0 0 0 0 ] 378.7336;
nuInf nuInf [ 0 2 -1 0 0 0 0 ] 8.9686e-07;
k k [ 0 0 1 0 0 0 0 ] 10;
n n [ 0 0 0 0 0 0 0 ] 0.2407;
}

}
base
{
transportModel Newtonian;
nu nu [ 0 2 -1 0 0 0 0 ] 295.22;
rho rho [ 1 -3 0 0 0 0 0 ] 1129;
BirdCarreauCoeffs
{
nu0 nu0 [ 0 2 -1 0 0 0 0 ] 262.65;
nuInf nuInf [ 0 2 -1 0 0 0 0 ] 0.000886;
k k [ 0 0 1 0 0 0 0 ] 10;
n n [ 0 0 0 0 0 0 0 ] 0.3005;
}

}
tcap
{
transportModel Newtonian;
nu nu [ 0 2 -1 0 0 0 0 ] 295.22;
rho rho [ 1 -3 0 0 0 0 0 ] 1129;
BirdCarreauCoeffs
{
nu0 nu0 [ 0 2 -1 0 0 0 0 ] 262.65;
nuInf nuInf [ 0 2 -1 0 0 0 0 ] 0.000886;
k k [ 0 0 1 0 0 0 0 ] 10;
n n [ 0 0 0 0 0 0 0 ] 0.3005;
}

}
bcap
{
transportModel Newtonian;
nu nu [ 0 2 -1 0 0 0 0 ] 295.22;
rho rho [ 1 -3 0 0 0 0 0 ] 1129;
BirdCarreauCoeffs
{
nu0 nu0 [ 0 2 -1 0 0 0 0 ] 262.65;
nuInf nuInf [ 0 2 -1 0 0 0 0 ] 0.000886;
k k [ 0 0 1 0 0 0 0 ] 10;
n n [ 0 0 0 0 0 0 0 ] 0.3005;
}

}
skirt
{
transportModel Newtonian;
nu nu [ 0 2 -1 0 0 0 0 ] 295.22;
rho rho [ 1 -3 0 0 0 0 0 ] 1129;
BirdCarreauCoeffs
{
nu0 nu0 [ 0 2 -1 0 0 0 0 ] 262.65;
nuInf nuInf [ 0 2 -1 0 0 0 0 ] 0.000886;
k k [ 0 0 1 0 0 0 0 ] 10;
n n [ 0 0 0 0 0 0 0 ] 0.3005;
}

}


);

refPhase tcap;

sigmas
(
(air tcap) 0.0
(air bcap) 0.0
(air skirt) 0.0
(air base) 0.0
(tcap bcap) 0.0
(tcap skirt) 0.0
(tcap base) 0.0
(bcap base) 0.0
(bcap skirt) 0.0
(base skirt) 0.0
);


// ************************************************** *********************** //
AbbasRahimi is offline   Reply With Quote

Old   February 4, 2016, 05:49
Default
  #4
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,409
Rep Power: 24
alexeym will become famous soon enoughalexeym will become famous soon enough
OK. You did not find it in transportProperties, search in 0/alpha.* files. Since you did not post your case, other people can only GUESS what is wrong. And, in general, guessing game is rather annoying.
alexeym is offline   Reply With Quote

Reply

Tags
multi phase flow, multiphaseinterfoam, transportproperties

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
decomposePar problem: Cell 0contains face labels out of range vaina74 OpenFOAM Pre-Processing 27 November 2, 2015 18:04
an error in Calculator's equation immortality OpenFOAM Paraview & paraFoam 11 September 3, 2013 16:18
How to install CGNS under windows xp? lzgwhy Main CFD Forum 1 January 11, 2011 19:44
Installation OF1.5-dev ttdtud OpenFOAM Installation 46 May 5, 2009 02:32
DecomposePar links against liblamso0 with OpenMPI jens_klostermann OpenFOAM Bugs 11 June 28, 2007 17:51


All times are GMT -4. The time now is 18:54.