how to change a volScalarField in bc?

Katl · January 5, 2012, 11:19

I need to add a source term in the time loop, which is calculated in one of my boundary conditions.

First I defined the following field in createFields.H:

Code:

 Info<< "Creating field sourceH\n" << endl;
    volScalarField sourceH
    (
        IOobject
        (
            "sourceH",
            runTime.timeName(),
            mesh,
            IOobject::READ_IF_PRESENT,
            IOobject::AUTO_WRITE
        ),
         Hclip/dim_s*0
    );

It is set to zero by "Hclip/dim_s*0" in the beginning and should be changed/updated in a specific boundary condition.

But how can I change the values of the field in the bc???

I tried the following:

Code:

scalarField sourceH = patch().lookupPatchField<volScalarField, scalar>("sourceH").patchInternalField();
scalar groundArea = 1.0; 
scalarField srcH = (HU.boundaryField()[patchNr]&n)/groundArea;
scalar cellSource = (gSum(srcH))/patch().size();
 for (int celli = 0; celli <= patch().size(); celli++) 
      {
       sourceH[celli]=cellSource;
      }

But "sourceH" is still zero...

marupio · January 5, 2012, 12:40

This type of issue has come up a few times before. The problem is access: the boundary condition only has const access to anything it looks up through the objectRegistry, and private data it creates cannot be accessed at the top level because the solver uses fvPatchField as an interface.

Does your solver need to change it? If not, the solution is fairly simple. Instead of creating the source term at the top level, give it to your custom bc. Then use objectRegistry::lookupObject to find it in your solver.

Katl · January 6, 2012, 08:34

Thanks David for your explanations!
The solver doesn't have change the scalarField, but just adding it as a source term.
To make sure I got you right:
Did you mean to calculate a scalarField sourceH in my boundary condition and the call it in the solver by something like:

Code:

const GeometricField<scalar, fvPatchField, volMesh>& Hquelle = objectRegistry::lookupObject<GeometricField<scalar, fvPatchField, volMesh> >("sourceH");

and add Hquelle as the source term?

I'm not really sure about this or in general how to directly call the scalarField from the bc in the solver....

marupio · January 6, 2012, 12:37

Very close. Instead of objectRegistry::lookupObject... use the name of the objectRegistry sourceH is registered to... you'll probably put it in the mesh, just like nearly everything else:

Code:

const volScalarField& Hquelle
(
    mesh.lookupObject<volScalarField>("sourceH")
);

And you have to make sure that your boundary condition has already created this sourceH object before the solver tries looking it up. So, make sourceH a member of your custom boundary condition, and initialize (to zero) it in all of the constructors.

Katl · January 10, 2012, 08:28

I have still problems with creating the volScalarField in my BC:
I tried it like this:

in the header file:

Code:

class abflussWehrDS
:
public
{
volScalarField sourceH_;
...

which gives me an error, that the field sourceH has an incomplete type

in the .C file:

Code:

Foam::
abflussWehrDS::
abflussWehrDS
(
    const fvPatch& p,
    const DimensionedField<vector, volMesh>& iF
)
:
    fixedValueFvPatchField<vector>(p, iF),
    HName_("H"),
    HUName_("HU"),
    sourceH_
(
  IOobject
 (
   "sourceH",
   runTime_.timeName(),
   mesh,
   IOobject::NO_READ,
   IOobject::AUTO_WRITE
  ),
    mesh,
    dimensionedScalar("zero", dimensionSet(0,1,-1,0,0,0,0), 0.0),
    "abflussWehrDS"
)
{}
Foam::
abflussWehrDS::
abflussWehrDS
(
    const abflussWehrDS& ptf,
    const fvPatch& p,
    const DimensionedField<vector, volMesh>& iF,
    const fvPatchFieldMapper& mapper
)
:
    fixedValueFvPatchField<vector>(ptf, p, iF, mapper),
    HName_(ptf.HName_),
    HUName_(ptf.HUName_),
    sonderBw_(ptf.sonderBw_),
    USpatch_(ptf.USpatch_)
    //sourceH_(ptf.sourceH_)
{}


Foam::
abflussWehrDS::
abflussWehrDS
(
    const fvPatch& p,
    const DimensionedField<vector, volMesh>& iF,
    const dictionary& dict
)
:
    fixedValueFvPatchField<vector>(p, iF, dict),
    HName_("H"),
    HUName_("HU"),
    sonderBw_(readScalar(dict.lookup("sonderBw"))),
    USpatch_(readScalar(dict.lookup("USpatch")))
//    sourceH_("sourceH")
{

    if (dict.found("H"))
    {
        dict.lookup("H") >> HName_;
    }
    if (dict.found("HU"))
    {
        dict.lookup("HU") >> HUName_;
    }
    if (dict.found("sourceH"))
    {
        dict.lookup("sourceH") >> sourceH_;
    }
}

Foam::
abflussWehrDS::
abflussWehrDS
(
    const abflussWehrDS& ptf
)
:
    fixedValueFvPatchField<vector>(ptf),
    HName_(ptf.HName_),
    HUName_(ptf.HUName_),
    sourceH_(ptf.sourceH_)
{}


Foam::
abflussWehrDS::
abflussWehrDS
(
    const abflussWehrDS& ptf,
    const DimensionedField<vector, volMesh>& iF
)
:
    fixedValueFvPatchField<vector>(ptf, iF),
    HName_(ptf.HName_),
    HUName_(ptf.HUName_),
    sourceH_(ptf.sourceH_)
{}

giving me the following errors:

Code:

abflussWehrDS.C: In constructor ‘Foam::abflussWehrDS::abflussWehrDS(const Foam::fvPatch&, const Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh>&)’:
abflussWehrDS.C:52: error: class ‘Foam::abflussWehrDS’ does not have any field named ‘sourceH_’
abflussWehrDS.C:57: error: ‘runTime_’ was not declared in this scope
abflussWehrDS.C:58: error: ‘mesh’ was not declared in this scope
abflussWehrDS.C: In constructor ‘Foam::abflussWehrDS::abflussWehrDS(const Foam::abflussWehrDS&, const Foam::fvPatch&, const Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh>&, const Foam::fvPatchFieldMapper&)’:
abflussWehrDS.C:84: error: class ‘Foam::abflussWehrDS’ does not have any field named ‘sourceH_’
abflussWehrDS.C:84: error: ‘const class Foam::abflussWehrDS’ has no member named ‘sourceH_’
abflussWehrDS.C: In constructor ‘Foam::abflussWehrDS::abflussWehrDS(const Foam::fvPatch&, const Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh>&, const Foam::dictionary&)’:
abflussWehrDS.C:102: error: class ‘Foam::abflussWehrDS’ does not have any field named ‘sourceH_’
abflussWehrDS.C:115: error: ‘sourceH_’ was not declared in this scope
abflussWehrDS.C: In copy constructor ‘Foam::abflussWehrDS::abflussWehrDS(const Foam::abflussWehrDS&)’:
abflussWehrDS.C:131: error: class ‘Foam::abflussWehrDS’ does not have any field named ‘sourceH_’
abflussWehrDS.C:131: error: ‘const class Foam::abflussWehrDS’ has no member named ‘sourceH_’
abflussWehrDS.C: In constructor ‘Foam::abflussWehrDS::abflussWehrDS(const Foam::abflussWehrDS&, const Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh>&)’:
abflussWehrDS.C:148: error: class ‘Foam::abflussWehrDS’ does not have any field named ‘sourceH_’
abflussWehrDS.C:148: error: ‘const class Foam::abflussWehrDS’ has no member named ‘sourceH_’
abflussWehrDS.C: In member function ‘virtual void Foam::abflussWehrDS::updateCoeffs()’:
abflussWehrDS.C:251: error: ‘sourceH’ was not declared in this scope
make: *** [Make/linux64GccDPOpt/abflussWehrDS.o] Fehler 1

I guess I have to include some files. But if I include createTime.H and createMesh.H it still wouldn't work.

marupio · January 10, 2012, 11:33

"does not have any field named sourceH_"

This is your first problem. It looks like your header file has problems... but you have only quoted a portion of it.

Code:

class abflussWehrDS
:
public <<-- public what?
{
volScalarField sourceH_;
...

It looks like you want to define what objects it inherits, but left them out. Use either:

Code:

class myClass
{
    // define myClass
};

or

Code:

class myClass
:
    public baseClass1,
    public baseClass2
{
    // define myClass
};

... or did you misquote your code?

Katl · January 11, 2012, 07:09

Sorry. You're right! I left something out in my quotation:

Code:

class abflussWehrDS
:
    public fixedValueFvPatchVectorField    
{
    volScalarField sourceH_;
    word HName_;
    word HUName_;
...

It worked fine with all the other variables, like HName_, that's why I don't understand that it has a problem with the volScalarField.

marupio · January 11, 2012, 13:38

There is probably an error where it complains in the header file that it doesn't know what volScalarField means. This could be an #include problem, or circular dependency.

Katl · January 19, 2012, 10:26

I tried to to solve this problem by adding

Code:

fixedValueFvPatchScalarField

as a second baseClass, like David mentioned. But all I got was an enormous amount of errors....

any other solutions to my initial problem? or is there still a possibility to do it this way?????

thanks in advance!!!!

marupio · January 19, 2012, 10:38

What are your errors?

Katl · January 19, 2012, 11:09

HTML Code:

abflussWehrDS.H:85: error: field ‘sourceH_’ has incomplete type
abflussWehrDS.H:131: error: invalid covariant return type for ‘virtual Foam::tmp<Foam::fvPatchField<Foam::Vector<double> > > Foam::abflussWehrDS::clone() const’
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.H:96: error:   overriding ‘Foam::tmp<Foam::fvPatchField<Type> > Foam::fixedValueFvPatchField<Type>::clone() const [with Type = double]’
abflussWehrDS.C: In constructor ‘Foam::abflussWehrDS::abflussWehrDS(const Foam::fvPatch&, const Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh>&)’:
abflussWehrDS.C:54: error: class ‘Foam::abflussWehrDS’ does not have any field named ‘sourceH_’
abflussWehrDS.C:59: error: request for member ‘db’ is ambiguous
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fvPatchField.C:158: error: candidates are: const Foam::objectRegistry& Foam::fvPatchField<Type>::db() const [with Type = double]
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fvPatchField.C:158: error:                 const Foam::objectRegistry& Foam::fvPatchField<Type>::db() const [with Type = Foam::Vector<double>]
abflussWehrDS.C:60: error: request for member ‘db’ is ambiguous
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fvPatchField.C:158: error: candidates are: const Foam::objectRegistry& Foam::fvPatchField<Type>::db() const [with Type = double]
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fvPatchField.C:158: error:                 const Foam::objectRegistry& Foam::fvPatchField<Type>::db() const [with Type = Foam::Vector<double>]
abflussWehrDS.C:64: error: ‘mesh’ was not declared in this scope
abflussWehrDS.C:67: error: no matching function for call to ‘Foam::fixedValueFvPatchField<double>::fixedValueFvPatchField()’
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:87: note: candidates are: Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fixedValueFvPatchField<Type>&, const Foam::DimensionedField<Type, Foam::volMesh>&) [with Type = double]
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:76: note:                 Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fixedValueFvPatchField<Type>&) [with Type = double]
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:66: note:                 Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fixedValueFvPatchField<Type>&, const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::volMesh>&, const Foam::fvPatchFieldMapper&) [with Type = double]
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:53: note:                 Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::volMesh>&, const Foam::dictionary&) [with Type = double]
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:41: note:                 Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::volMesh>&) [with Type = double]
abflussWehrDS.C: In constructor ‘Foam::abflussWehrDS::abflussWehrDS(const Foam::abflussWehrDS&, const Foam::fvPatch&, const Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh>&, const Foam::fvPatchFieldMapper&)’:
abflussWehrDS.C:86: error: class ‘Foam::abflussWehrDS’ does not have any field named ‘sourceH_’
abflussWehrDS.C:86: error: ‘const class Foam::abflussWehrDS’ has no member named ‘sourceH_’
abflussWehrDS.C:86: error: no matching function for call to ‘Foam::fixedValueFvPatchField<double>::fixedValueFvPatchField()’
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:87: note: candidates are: Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fixedValueFvPatchField<Type>&, const Foam::DimensionedField<Type, Foam::volMesh>&) [with Type = double]
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:76: note:                 Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fixedValueFvPatchField<Type>&) [with Type = double]
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:66: note:                 Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fixedValueFvPatchField<Type>&, const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::volMesh>&, const Foam::fvPatchFieldMapper&) [with Type = double]
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:53: note:                 Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::volMesh>&, const Foam::dictionary&) [with Type = double]
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:41: note:                 Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::volMesh>&) [with Type = double]
abflussWehrDS.C: In constructor ‘Foam::abflussWehrDS::abflussWehrDS(const Foam::fvPatch&, const Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh>&, const Foam::dictionary&)’:
abflussWehrDS.C:104: error: class ‘Foam::abflussWehrDS’ does not have any field named ‘sourceH_’
abflussWehrDS.C:105: error: expected identifier before ‘{’ token
abflussWehrDS.C:105: error: expected `(' before ‘{’ token
abflussWehrDS.C:105: error: no matching function for call to ‘Foam::fixedValueFvPatchField<double>::fixedValueFvPatchField()’
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:87: note: candidates are: Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fixedValueFvPatchField<Type>&, const Foam::DimensionedField<Type, Foam::volMesh>&) [with Type = double]
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:76: note:                 Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fixedValueFvPatchField<Type>&) [with Type = double]
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:66: note:                 Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fixedValueFvPatchField<Type>&, const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::volMesh>&, const Foam::fvPatchFieldMapper&) [with Type = double]
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:53: note:                 Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::volMesh>&, const Foam::dictionary&) [with Type = double]
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:41: note:                 Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::volMesh>&) [with Type = double]
abflussWehrDS.C:117: error: ‘sourceH_’ was not declared in this scope
abflussWehrDS.C: In copy constructor ‘Foam::abflussWehrDS::abflussWehrDS(const Foam::abflussWehrDS&)’:
abflussWehrDS.C:133: error: class ‘Foam::abflussWehrDS’ does not have any field named ‘sourceH_’
abflussWehrDS.C:133: error: ‘const class Foam::abflussWehrDS’ has no member named ‘sourceH_’
abflussWehrDS.C:126: warning: base class ‘class Foam::fixedValueFvPatchField<double>’ should be explicitly initialized in the copy constructor
abflussWehrDS.C:133: error: no matching function for call to ‘Foam::fixedValueFvPatchField<double>::fixedValueFvPatchField()’
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:87: note: candidates are: Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fixedValueFvPatchField<Type>&, const Foam::DimensionedField<Type, Foam::volMesh>&) [with Type = double]
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:76: note:                 Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fixedValueFvPatchField<Type>&) [with Type = double]
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:66: note:                 Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fixedValueFvPatchField<Type>&, const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::volMesh>&, const Foam::fvPatchFieldMapper&) [with Type = double]
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:53: note:                 Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::volMesh>&, const Foam::dictionary&) [with Type = double]
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:41: note:                 Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::volMesh>&) [with Type = double]
abflussWehrDS.C: In constructor ‘Foam::abflussWehrDS::abflussWehrDS(const Foam::abflussWehrDS&, const Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh>&)’:
abflussWehrDS.C:150: error: class ‘Foam::abflussWehrDS’ does not have any field named ‘sourceH_’
abflussWehrDS.C:150: error: ‘const class Foam::abflussWehrDS’ has no member named ‘sourceH_’
abflussWehrDS.C:150: error: no matching function for call to ‘Foam::fixedValueFvPatchField<double>::fixedValueFvPatchField()’
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:87: note: candidates are: Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fixedValueFvPatchField<Type>&, const Foam::DimensionedField<Type, Foam::volMesh>&) [with Type = double]
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:76: note:                 Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fixedValueFvPatchField<Type>&) [with Type = double]
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:66: note:                 Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fixedValueFvPatchField<Type>&, const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::volMesh>&, const Foam::fvPatchFieldMapper&) [with Type = double]
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:53: note:                 Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::volMesh>&, const Foam::dictionary&) [with Type = double]
/home/h17_2/student2/OpenFOAM/OpenFOAM-1.5/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:41: note:                 Foam::fixedValueFvPatchField<Type>::fixedValueFvPatchField(const Foam::fvPatch&, const Foam::DimensionedField<Type, Foam::volMesh>&) [with Type = double]

marupio · January 19, 2012, 16:13

"abflussWehrDS.H:85: error: field ‘sourceH_’ has incomplete type"

This is an #include problem. Either you didn't include the correct files that gives you the full definition of volScalarField, or you have circular dependency among your include files. The first option is likely, as volScalarField needs at least two files - the file that gives you the typedef volScalarField, and the one with the full definition.

I strongly dislike these kinds of problems.

Katl · January 20, 2012, 08:21

I tried it by including

Code:

#include "fvPatchFields.H"
#include "fixedValueFvPatchFields.H"

and with:

Code:

class abflussWehrDS
:
    public fixedValueFvPatchVectorField  
{
    // Private data

    word HName_;
    word HUName_;
    int sonderBw_;
    int USpatch_;
    volScalarField sourceH_;
    
public:

   //- Runtime type information
   TypeName("abflussWehrDS");
....

But the problem is still not solved:

Code:

abflussWehrDS.H:84: error: field ‘sourceH_’ has incomplete type
abflussWehrDS.C: In constructor ‘Foam::abflussWehrDS::abflussWehrDS(const Foam::fvPatch&, const Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh>&)’:
abflussWehrDS.C:54: error: class ‘Foam::abflussWehrDS’ does not have any field named ‘sourceH_’
abflussWehrDS.C: In constructor ‘Foam::abflussWehrDS::abflussWehrDS(const Foam::abflussWehrDS&, const Foam::fvPatch&, const Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh>&, const Foam::fvPatchFieldMapper&)’:
abflussWehrDS.C:86: error: class ‘Foam::abflussWehrDS’ does not have any field named ‘sourceH_’
abflussWehrDS.C:86: error: ‘const class Foam::abflussWehrDS’ has no member named ‘sourceH_’
abflussWehrDS.C: In constructor ‘Foam::abflussWehrDS::abflussWehrDS(const Foam::fvPatch&, const Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh>&, const Foam::dictionary&)’:
abflussWehrDS.C:104: error: class ‘Foam::abflussWehrDS’ does not have any field named ‘sourceH_’
abflussWehrDS.C:117: error: ‘sourceH_’ was not declared in this scope
abflussWehrDS.C: In copy constructor ‘Foam::abflussWehrDS::abflussWehrDS(const Foam::abflussWehrDS&)’:
abflussWehrDS.C:133: error: class ‘Foam::abflussWehrDS’ does not have any field named ‘sourceH_’
abflussWehrDS.C:133: error: ‘const class Foam::abflussWehrDS’ has no member named ‘sourceH_’
abflussWehrDS.C: In constructor ‘Foam::abflussWehrDS::abflussWehrDS(const Foam::abflussWehrDS&, const Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh>&)’:
abflussWehrDS.C:150: error: class ‘Foam::abflussWehrDS’ does not have any field named ‘sourceH_’
abflussWehrDS.C:150: error: ‘const class Foam::abflussWehrDS’ has no member named ‘sourceH_’
abflussWehrDS.C: In member function ‘virtual void Foam::abflussWehrDS::updateCoeffs()’:
abflussWehrDS.C:251: error: ‘sourceH’ was not declared in this scope
abflussWehrDS.C:253: error: ‘sourceH’ was not declared in this scope
make: *** [Make/linux64GccDPOpt/abflussWehrDS.o] Fehler 1

How can I find out which files are missing?

Fransje · January 26, 2012, 10:05

Quote:

Originally Posted by marupio

This type of issue has come up a few times before. The problem is access: the boundary condition only has const access to anything it looks up through the objectRegistry, and private data it creates cannot be accessed at the top level because the solver uses fvPatchField as an interface.

Does your solver need to change it? If not, the solution is fairly simple. Instead of creating the source term at the top level, give it to your custom bc. Then use objectRegistry::lookupObject to find it in your solver.

Dear Kathrin, dear David,

The problem of creating the source term / a variable in the boundary condition for use in the main solver, is that if you don't add it correctly to the database, it will be deleted out of it as soon as the fvPatchField is destroyed. This means, as soon as you exit the boundary condition code.

Anyways, the solution is quite simple. Let's say you want to store a scalarList in the database, for use anywhere (in the bc, the solver, etc) you would do:

Code:

scalarList your_scalar_list;

mesh.thisDb().store
(
    new IOList<scalar>
    (
        IOobject
        (
            "the_database_name_of_var",
            mesh,
            IOobject::NO_READ,
            IOobject::NO_WRITE
        ),
        your_scalar_list
    )
);

Checking it out will be done in the usual way:

Code:

const IOList<scalar>& dbScalarList
                = mesh.thisDb().lookupObject< IOList<scalar> >("the_database_name_of_var");

scalarList your_scalar_list = dbScalarList;

You could also use const scalarList& straight away as type, but the reason I use an IOList<scalar> is for the next step. Because once you've use your variable and updated it, you can now update it's value in the database (!!! This, although it theoretically is of const type, hence not modifiable

!!!).
You would do this using the following (perfectly legal) C++ trick:

Code:

const_cast<IOList<scalar>& >( dbScalarList ) = your_updated_scalar_list ;

I hope this helps!

Kind regards,

Francois

marupio · January 26, 2012, 10:10

Using const_cast is cheating!

gschaider · January 26, 2012, 13:42

Quote:

Originally Posted by marupio

Using const_cast is cheating!

"The first rule of the const_cast-club is: 'Don't talk about the const_cast!'"

Fransje · January 27, 2012, 10:32

Quote:

Originally Posted by gschaider

"The first rule of the const_cast-club is: 'Don't talk about the const_cast!'"

He he he!

Cheating..? Perhaps.. But most importantly: It works!

Katl · January 29, 2012, 09:25

Thank you all for your help. The const_cast works

But I have one more question:
Is it also possible to do this for a volScalarField. I could only find IOField<scalar>. Or is it possible to convert a scalarField into a volScalarField, which would also be sufficient.

Fransje · January 31, 2012, 12:06

Well, actually, it has been a while since I implemented this hack, but if I recall properly, the store() function can store any pointer to an IOobject.

So, since your volScalarField is already an IOobject, what you are trying to do should be very simple to do:

Code:

// with your_volScalarField created as it normally would be

mesh.thisDb().store
(
    new volScalarField
    (
        your_volScalarField
    )
);

And obviously you would do your const_cast with:

Code:

// with dbVolScalarField retrieved earlier from your database using lookupObject<volScalarField>()

const_cast<volScalarField& >( dbVolScalarField ) = your_updated_volScalarField ;

Kind regards,

Francois.

tomislav_maric · January 31, 2012, 15:51

From

OpenFOAM-1.6-ext/src/finiteVolume/fields/fvPatchFields/derived/parabolicVelocity

comes:

Code:

void parabolicVelocityFvPatchVectorField::updateCoeffs()
{
    if (updated())
    {
        return;
    }

    // Get range and orientation
    boundBox bb(patch().patch().localPoints(), true);

    vector ctr = 0.5*(bb.max() + bb.min());

    const vectorField& c = patch().Cf();

    // Calculate local 1-D coordinate for the parabolic profile
    scalarField coord = 2*((c - ctr) & y_)/((bb.max() - bb.min()) & y_);

    vectorField::operator=(n_*maxValue_*(1.0 - sqr(coord)));
}

This is called upcasting in C++: stripping the inherited object to the base class. All bcs are hidden *fields. No need for *_cast magic.

Just so you don't miss it , the key line is

Code:

vectorField::operator=  blah blah

, this converts "this" (the class, in this case parabolicBlah...) to a vectorField.

T.

January 5, 2012, 11:19	how to change a volScalarField in bc?	#1
Katl New Member Kathrin Join Date: Nov 2011 Posts: 15 Rep Power: 14	I need to add a source term in the time loop, which is calculated in one of my boundary conditions. First I defined the following field in createFields.H: Code: Info<< "Creating field sourceH\n" << endl; volScalarField sourceH ( IOobject ( "sourceH", runTime.timeName(), mesh, IOobject::READ_IF_PRESENT, IOobject::AUTO_WRITE ), Hclip/dim_s0 ); It is set to zero by "Hclip/dim_s0" in the beginning and should be changed/updated in a specific boundary condition. But how can I change the values of the field in the bc??? I tried the following: Code: scalarField sourceH = patch().lookupPatchField<volScalarField, scalar>("sourceH").patchInternalField(); scalar groundArea = 1.0; scalarField srcH = (HU.boundaryField()[patchNr]&n)/groundArea; scalar cellSource = (gSum(srcH))/patch().size(); for (int celli = 0; celli <= patch().size(); celli++) { sourceH[celli]=cellSource; } But "sourceH" is still zero... atulkjoy likes this.

January 5, 2012, 12:40		#2
marupio Senior Member David Gaden Join Date: Apr 2009 Location: Winnipeg, Canada Posts: 437 Rep Power: 22	This type of issue has come up a few times before. The problem is access: the boundary condition only has const access to anything it looks up through the objectRegistry, and private data it creates cannot be accessed at the top level because the solver uses fvPatchField as an interface. Does your solver need to change it? If not, the solution is fairly simple. Instead of creating the source term at the top level, give it to your custom bc. Then use objectRegistry::lookupObject to find it in your solver. randolph and Gerry Kan like this. __________________ ~~~ Follow me on twitter @DavidGaden

January 6, 2012, 12:37		#4
marupio Senior Member David Gaden Join Date: Apr 2009 Location: Winnipeg, Canada Posts: 437 Rep Power: 22	Very close. Instead of objectRegistry::lookupObject... use the name of the objectRegistry sourceH is registered to... you'll probably put it in the mesh, just like nearly everything else: Code: const volScalarField& Hquelle ( mesh.lookupObject<volScalarField>("sourceH") ); And you have to make sure that your boundary condition has already created this sourceH object before the solver tries looking it up. So, make sourceH a member of your custom boundary condition, and initialize (to zero) it in all of the constructors. __________________ ~~~ Follow me on twitter @DavidGaden

January 10, 2012, 11:33		#6
marupio Senior Member David Gaden Join Date: Apr 2009 Location: Winnipeg, Canada Posts: 437 Rep Power: 22	"does not have any field named sourceH_" This is your first problem. It looks like your header file has problems... but you have only quoted a portion of it. Code: class abflussWehrDS : public <<-- public what? { volScalarField sourceH_; ... It looks like you want to define what objects it inherits, but left them out. Use either: Code: class myClass { // define myClass }; or Code: class myClass : public baseClass1, public baseClass2 { // define myClass }; ... or did you misquote your code? __________________ ~~~ Follow me on twitter @DavidGaden

January 11, 2012, 07:09	misquote	#7
Katl New Member Kathrin Join Date: Nov 2011 Posts: 15 Rep Power: 14	Sorry. You're right! I left something out in my quotation: Code: class abflussWehrDS : public fixedValueFvPatchVectorField { volScalarField sourceH_; word HName_; word HUName_; ... It worked fine with all the other variables, like HName_, that's why I don't understand that it has a problem with the volScalarField.

January 6, 2012, 08:34		#3
Katl New Member Kathrin Join Date: Nov 2011 Posts: 15 Rep Power: 14	Thanks David for your explanations! The solver doesn't have change the scalarField, but just adding it as a source term. To make sure I got you right: Did you mean to calculate a scalarField sourceH in my boundary condition and the call it in the solver by something like: Code: const GeometricField<scalar, fvPatchField, volMesh>& Hquelle = objectRegistry::lookupObject<GeometricField<scalar, fvPatchField, volMesh> >("sourceH"); and add Hquelle as the source term? I'm not really sure about this or in general how to directly call the scalarField from the bc in the solver....

January 11, 2012, 13:38		#8
marupio Senior Member David Gaden Join Date: Apr 2009 Location: Winnipeg, Canada Posts: 437 Rep Power: 22	There is probably an error where it complains in the header file that it doesn't know what volScalarField means. This could be an #include problem, or circular dependency. __________________ ~~~ Follow me on twitter @DavidGaden

January 19, 2012, 10:26		#9
Katl New Member Kathrin Join Date: Nov 2011 Posts: 15 Rep Power: 14	I tried to to solve this problem by adding Code: fixedValueFvPatchScalarField as a second baseClass, like David mentioned. But all I got was an enormous amount of errors.... any other solutions to my initial problem? or is there still a possibility to do it this way????? thanks in advance!!!!

January 19, 2012, 10:38		#10
marupio Senior Member David Gaden Join Date: Apr 2009 Location: Winnipeg, Canada Posts: 437 Rep Power: 22	What are your errors? __________________ ~~~ Follow me on twitter @DavidGaden

January 19, 2012, 16:13		#12
marupio Senior Member David Gaden Join Date: Apr 2009 Location: Winnipeg, Canada Posts: 437 Rep Power: 22	"abflussWehrDS.H:85: error: field ‘sourceH_’ has incomplete type" This is an #include problem. Either you didn't include the correct files that gives you the full definition of volScalarField, or you have circular dependency among your include files. The first option is likely, as volScalarField needs at least two files - the file that gives you the typedef volScalarField, and the one with the full definition. I strongly dislike these kinds of problems. __________________ ~~~ Follow me on twitter @DavidGaden

January 26, 2012, 10:10		#15
marupio Senior Member David Gaden Join Date: Apr 2009 Location: Winnipeg, Canada Posts: 437 Rep Power: 22	Using const_cast is cheating! __________________ ~~~ Follow me on twitter @DavidGaden

January 29, 2012, 09:25	Thanks!!	#18
Katl New Member Kathrin Join Date: Nov 2011 Posts: 15 Rep Power: 14	Thank you all for your help. The const_cast works But I have one more question: Is it also possible to do this for a volScalarField. I could only find IOField<scalar>. Or is it possible to convert a scalarField into a volScalarField, which would also be sufficient.

January 31, 2012, 12:06		#19
Fransje Senior Member Francois Join Date: Jun 2010 Posts: 107 Rep Power: 20	Well, actually, it has been a while since I implemented this hack, but if I recall properly, the store() function can store any pointer to an IOobject. So, since your volScalarField is already an IOobject, what you are trying to do should be very simple to do: Code: // with your_volScalarField created as it normally would be mesh.thisDb().store ( new volScalarField ( your_volScalarField ) ); And obviously you would do your const_cast with: Code: // with dbVolScalarField retrieved earlier from your database using lookupObject<volScalarField>() const_cast<volScalarField& >( dbVolScalarField ) = your_updated_volScalarField ; Kind regards, Francois. Katl likes this.

January 31, 2012, 15:51		#20
tomislav_maric Senior Member Tomislav Maric Join Date: Mar 2009 Location: Darmstadt, Germany Posts: 284 Blog Entries: 5 Rep Power: 21	From OpenFOAM-1.6-ext/src/finiteVolume/fields/fvPatchFields/derived/parabolicVelocity comes: Code: void parabolicVelocityFvPatchVectorField::updateCoeffs() { if (updated()) { return; } // Get range and orientation boundBox bb(patch().patch().localPoints(), true); vector ctr = 0.5(bb.max() + bb.min()); const vectorField& c = patch().Cf(); // Calculate local 1-D coordinate for the parabolic profile scalarField coord = 2((c - ctr) & y_)/((bb.max() - bb.min()) & y_); vectorField::operator=(n_maxValue_(1.0 - sqr(coord))); } This is called upcasting in C++: stripping the inherited object to the base class. All bcs are hidden fields. No need for _cast magic. Just so you don't miss it , the key line is Code: vectorField::operator= blah blah , this converts "this" (the class, in this case parabolicBlah...) to a vectorField. T. Last edited by tomislav_maric; January 31, 2012 at 16:01. Reason: upcast, downcast...

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Solid/liquid phase change	fabian_roesler	OpenFOAM	10	December 24, 2012 06:37
Change cell zone index/thread during simulation	neilduffy1024	FLUENT	0	January 17, 2011 09:40
Is there a way to change the name a volScalarField	liu	OpenFOAM Running, Solving & CFD	2	October 18, 2007 17:49
no enthalpy change across the momentum source	Atit Koonsrisuk	CFX	2	December 19, 2005 02:33
Multicomponent fluid	Andrea	CFX	2	October 11, 2004 05:12