[zhxter]

Hi all,

I am now modifying the "oscillatingFixedValue" and apply this modified boundary to the velocity field. However, in the modified boundary, I need to call the alpha.water value at the same patch. And the sentences of codes for calling alpha.water is given as follows,

this->patch().template lookupPatchField<volScalarField, scalar>
(
"alpha.water"
);

When I compile the modified boundary, there is no error. However, when I execute the solver interFoam, the error is given as follows,
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.4.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.4.0-f0842aea0e77
Exec : interFoam
Date : Apr 27 2017
Time : 01:10:38
Host : "ubuntu"
PID : 18706
Case : /home/zhxt/waves2Foam/research/OEpaper1/l3m/l3mT1scalculation
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

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

Create mesh for time = 1.64


PIMPLE: Operating solver in PISO mode

Reading field p_rgh

Reading field U



--> FOAM FATAL ERROR:

request for volScalarField alpha.water from objectRegistry region0 failed
available objects of type volScalarField are
1(p_rgh)

From function objectRegistry::lookupObject<Type>(const word&) const
in file /home/openfoam/OpenFOAM/OpenFOAM-2.4.0/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 198.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const& Foam:bjectRegistry::lookupObject<Foam::Geometric Field<double, Foam::fvPatchField, Foam::volMesh> >(Foam::word const&) const at ??:?
#3 Foam:amBreakInflowBoundaryFvPatchField:amBreak InflowBoundaryFvPatchField(Foam::fvPatch const&, Foam:imensionedField<Foam::Vector<double>, Foam::volMesh> const&, Foam::dictionary const&) at ??:?
#4 Foam::fvPatchField<Foam::Vector<double> >::adddictionaryConstructorToTable<Foam:amBreakI nflowBoundaryFvPatchField>::New(Foam::fvPatch const&, Foam:imensionedField<Foam::Vector<double>, Foam::volMesh> const&, Foam::dictionary const&) at ??:?
#5 Foam::fvPatchField<Foam::Vector<double> >::New(Foam::fvPatch const&, Foam:imensionedField<Foam::Vector<double>, Foam::volMesh> const&, Foam::dictionary const&) at ??:?
#6 Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::readField( Foam:imensionedField<Foam::Vector<double>, Foam::volMesh> const&, Foam::dictionary const&) at ??:?
#7 Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>::readFields(Foam::dictionary const&) at ??:?
#8 Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>::readFields() at ??:?
#9 Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>::GeometricField(Foam::IOobject const&, Foam::fvMesh const&) at ??:?
#10 ? at ??:?
#11 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#12 ? at ??:?
Aborted (core dumped)

It seems that the error is that the alpha.water is not registered. And Then I look at the creatFields.h file. The p_rgh and U field are registered. However, it seems that the alpha1 (water phase) is called using the definition : volScalarField& alpha1(mixture.alpha1()); So how should I call the alpha.water field in my modified boundary?? Any help will be greatly appreciated!

Info<< "Reading field p_rgh\n" << endl;
volScalarField p_rgh
(
IOobject
(
"p_rgh",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);

Info<< "Reading field U\n" << endl;
volVectorField U
(
IOobject
(
"U",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);

#include "createPhi.H"


Info<< "Reading transportProperties\n" << endl;
immiscibleIncompressibleTwoPhaseMixture mixture(U, phi);

volScalarField& alpha1(mixture.alpha1());
volScalarField& alpha2(mixture.alpha2());

const dimensionedScalar& rho1 = mixture.rho1();
const dimensionedScalar& rho2 = mixture.rho2();

[Phicau]

Hi Zhang,

it might not be registered in region0, but it needs to be in the database. Try the following:

https://github.com/phicau/OLAFOAM/bl...orField.C#L352

    const volScalarField& alpha = 
        db().lookupObject<volScalarField>("alpha.water");

It works for me.

Best,

Pablo

[zhxter]

Hi Pablo,
Thanks for your reply. According to your suggestion, the code of calling alpha.water is modified as follows,

const volScalarField& alpha = db().lookupObject<volScalarField> ("alpha.water");
const fvMesh& mesh=alpha.mesh();
const word patchName = this->patch().name();
const label patchID = mesh.boundaryMesh().findPatchID(patchName);
const scalarField alphaB=alpha.boundaryField()[patchID];

Also the compilation has no problem. However, when running interFoam, the same error still exists, i.e.
Create time

Create mesh for time = 1.64


PIMPLE: Operating solver in PISO mode

Reading field p_rgh

Reading field U



--> FOAM FATAL ERROR:

request for volScalarField alpha.water from objectRegistry region0 failed
available objects of type volScalarField are
1(p_rgh)

From function objectRegistry::lookupObject<Type>(const word&) const
in file /home/openfoam/OpenFOAM/OpenFOAM-2.4.0/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 198.

FOAM aborting

Do you know the reason?
Many thanks
Xiantao

[zhxter]

Hi Pablo,

The problem has been solved. The problem is that I add the following code line:

const volScalarField& alpha = db().lookupObject<volScalarField> ("alpha.water");
const fvMesh& mesh=alpha.mesh();
const word patchName = this->patch().name();
const label patchID = mesh.boundaryMesh().findPatchID(patchName);
const scalarField alphaB=alpha.boundaryField()[patchID];

in both updateCoeff() and constructors. It seem that if I delete the above line in constructors, then there is no problems

Kind Regards
Xiantao

[Pavithra]

Hello,

Although my question is not directly related to this thread, I have a question that is similar to this problem.

I am trying to modify icoReactingMultiphaseInterFoam to model multicomponent evaporation in the presence of electric field. In order to solve the electrostatic equations, I need to define dielectric properties as a function of phase fractions. I am unable to access the alpha fields.

Could some one direct me how to access the alpha fields in domain ? I have three phases air, water and vapour. I want to access the phase fractions of these phases. If I want to use the method stated in this thread, which file should I modify ?

Thank You.

-Pavithra.