CFD Online Discussion Forums - Field value inside a boundary condition class

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Programming & Development (https://www.cfd-online.com/Forums/openfoam-programming-development/)

- - Field value inside a boundary condition class (https://www.cfd-online.com/Forums/openfoam-programming-development/74980-field-value-inside-boundary-condition-class.html)

Field value inside a boundary condition class

Hello Forum,

I'm using OF-1.5-dev in openSUSE 11.2. I want to implement a boundary condition class which depends on a field value at a point.

I used the parabolicVelocity class as start point. I modified it to fix the boundary value according to different parameters and it works fine.

The next step is to read a field value at a point and use it to modify the boundary value.

I read several post, but I can't understand how to know a field value at a point. These are the posts I read

http://www.cfd-online.com/Forums/ope...ary-point.html
http://openfoamwiki.net/index.php/Sn...value_at_point

Can somebody help me? Thanks in advance

Pablo

Hi Pablo
try the following code segment

point p(x,y,z) ;
label cellNo=mesh_.findCell(p);
//using the cell center value or make an interpolation
type value=Variable[cellNO];
If you want to do an interpolation, please see the following thread
http://www.cfd-online.com/Forums/ope...tml#post254038

regards,Junwei

Hi Junwei

thanks for your reply!

I read your idea before. The problem is that I want to do this evaluation inside a BC class, so I don't have any reference to mesh_ and Variable.

So, I think the improved question could be: How should I reference a Variable (like p or U) and mesh_ inside a BC class?

BTW: These are my first steps in OF programming.

Regards

Pablo

You have the access member function const objectRegistry& db() const. Accessing for example U is done by the code:

Code:

const volVectorField& U = db().lookupObject<volVectorField>("U");

For accessing the mesh: when creating a boundary condition, you have access to the patch. You can thus access the mesh with:

Code:

const fvMesh& mesh = patch().boundaryMesh().mesh();

Boundary Condition Using Information from Opposite Face

Hello,

I have a related question. I am using OpenFOAM-1.6, and I want to set up a boundary condition on velocity that requires knowledge of the velocity at the face opposite the boundary face. Is there a straightforward way to do this from within a derived fvPatchFields class? Or will I have to access the entire velocity volume field from within that derived fvPatchFields class and use something like "oppositeCellFace"? If I need to do the latter, can someone give some guidance, please?

Thank you,

Matt

Hi Cedric and Junwei

I want to thank you. I could implement my new boundary condition and is working now! :D

BTW, Cedric, As I told you these are my first steps. I found very difficult to understand and/or find functions and classes in OF Oxygen help. Is there another place to find a more user friendly help?

Thanks for your help!

Pablo

Quote:

Originally Posted by CedricVH (Post 254591)

You have the access member function const objectRegistry& db() const. Accessing for example U is done by the code:

Code:

const volVectorField& U = db().lookupObject<volVectorField>("U");

For accessing the mesh: when creating a boundary condition, you have access to the patch. You can thus access the mesh with:

Code:

const fvMesh& mesh = patch().boundaryMesh().mesh();

Quote:

Originally Posted by mchurchf (Post 254599)

Hi Matt

Is your "opposite boundary face" a boundary patch in your case? If it is, You can search the patch by its index or patch name.

label patchId=patch().boundaryMesh().lookupPatchID(patch Name);
and using the following code

const vectorField =U.boundaryField()[patchId];
.... // do your work

U can be obtained using credricVH's method mentioned above.(lookup using ObjectRegistry)

regards, Junwei

Accessing internal field and mesh from within boundary condition

Thank you all for your help,

I was able to implement my boundary condition as well. I used the following code to access the internal velocity field and the mesh two layers of cells inward from the boundary:

Code:

//  Set up access to the internal velocity field and mesh

    const volVectorField& U =

        db().objectRegistry::lookupObject<volVectorField>(UName_);

    const fvMesh& mesh = patch().boundaryMesh().mesh();



    forAll(patch(), facei)

    {

    // get global cell indices for cells adjacent to patch    

        label celli = patch().faceCells()[facei];



    // get global face indices for faces opposite patch face

    label oppFacei = mesh.cells()[celli].opposingFaceLabel(facei+patch().patch().start(),mesh.faces());



    // get coordinates of center of cell adjacent to patch (patch cells)

    vector cellCentreO = mesh.cellCentres()[mesh.owner()[oppFacei]];



    // get coordinates of center of cell on the side opposite the patch of

    // the patch cell

    vector cellCentreN = mesh.cellCentres()[mesh.neighbour()[oppFacei]];



    // get coordinates of center of face opposite the patch boundary face

    vector faceCentre  = mesh.faceCentres()[oppFacei];



    // get coordinates of center of patch boundary face;

    vector patchFaceCentre = mesh.faceCentres()[facei+patch().patch().start()];

    }

How can I access patch() function? I try to include it in my solver files with a compile error "patch is not defined in this scope". My wish is to inject a particle in each boundary cell of a patch. I have the code for particle generation, I just can not find the cell index for which to generate it.
I can not find the function lookupPatchID in the doxygen documentation, either. Though it may still work, I can not test it without first fixing the patch() error message.

Quote:

Originally Posted by mchurchf (Post 254946)

Code:

//  Set up access to the internal velocity field and mesh

    const volVectorField& U =

        db().objectRegistry::lookupObject<volVectorField>(UName_);

    const fvMesh& mesh = patch().boundaryMesh().mesh();



    forAll(patch(), facei)

    {

    // get global cell indices for cells adjacent to patch    

        label celli = patch().faceCells()[facei];



    // get global face indices for faces opposite patch face

    label oppFacei = mesh.cells()[celli].opposingFaceLabel(facei+patch().patch().start(),mesh.faces());



    // get coordinates of center of cell adjacent to patch (patch cells)

    vector cellCentreO = mesh.cellCentres()[mesh.owner()[oppFacei]];



    // get coordinates of center of cell on the side opposite the patch of

    // the patch cell

    vector cellCentreN = mesh.cellCentres()[mesh.neighbour()[oppFacei]];



    // get coordinates of center of face opposite the patch boundary face

    vector faceCentre  = mesh.faceCentres()[oppFacei];



    // get coordinates of center of patch boundary face;

    vector patchFaceCentre = mesh.faceCentres()[facei+patch().patch().start()];

    }

Hi

I follow your code, and write a code to test if it could work or not:

Quote:

#include "fvCFD.H"
#include "wallFvPatch.H"

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

int main(int argc, char *argv[])
{
timeSelector::addOptions();
#include "setRootCase.H"
#include "createTime.H"

Info<< "Create mesh, no clear-out\n" << endl;
fvMesh mesh
(
IOobject
(
fvMesh::defaultRegion,
runTime.timeName(),
runTime,
IOobject::MUST_READ
)
);

const fvPatchList& patches = mesh.boundary();

forAll(mesh.boundary(), patchi)
{
const fvPatch& patch = patches[patchi];
if (isA<wallFvPatch>(patch)) // is wall or not//
{
const fvMesh& mesh = patch.boundaryMesh().mesh();

forAll(patch, facei)
{
// get global cell indices for cells adjacent to patch
label celli = patch.faceCells()[facei];

// get global face indices for faces opposite patch face
label oppFacei = mesh.cells()[celli].opposingFaceLabel(facei+patch.patch.start(),mesh. faces());

Info<< facei << endl;
Info<< celli << endl;
Info<< oppFacei << endl;
Info<< ' ' << endl;
}

}

}

}

But I can not compile this code, some errors have happens in the opposiongFaceLabel. Do you have any suggestions about the code?

I figure it out, just delete one patch from opposingFaceLabel(facei+patch.patch.start(),mesh. faces());

Sorry to trouble you.

Hi, I'm trying to create my own boundary condition.

I'm modifying the Member Function from parabolicVelocityFvPatchVectorField.C(i.e, I chose parabolicVelocityFvPatchVectorField.C as the base)

When I tried to read field values like U or p on the boundary member function, compiling was successfully done, but I get the error message as belows when I run "setFields" on an example case based on interFoam.

Quote:

--> FOAM Warning :
From function dlLibraryTableOpen(const fileName& functionLibName)
in file db/dlLibraryTable/dlLibraryTable.C at line 85
could not load /home/lee/foam/lee-3.1/lib/linux64GccDPOpt/libmyfunctionfinal2.so: undefined symbol: _ZTVN4Foam15twoPhaseMixtureE

And then, when I run application(interFoam), an error message is shown :

Quote:

Reading field T

--> FOAM FATAL ERROR:
request for volVectorField U from objectRegistry region0 failed
available objects of type volVectorField are
1
(
T
)

From function objectRegistry::lookupObject<Type>(const word&) const
in file /home/lee/foam/foam-extend-3.1/src/foam/lnInclude/objectRegistryTemplates.C at line 139.
FOAM aborting
Aborted (core dumped)

I used these commans for reading the field values(U, phi, alpha1)

Quote:

const volVectorField& U = db().lookupObject<volVectorField>("U");
const surfaceScalarField& phi = db().lookupObject<surfaceScalarField>("phi");
const volScalarField& alpha1 = db().lookupObject<volScalarField>("alpha1");

I'm beginner in programming, so I guess I'm missing a simple thing...

this is a part of Member Function:

Quote:

void cbVelocityFvPatchVectorField::updateCoeffs()
{
if (updated())
{
return;
}
const fvMesh& mesh = dimensionedInternalField().mesh();
//const fvMesh& mesh = patch().boundaryMesh().mesh();
const word& patchName = this->patch().name();
const label patchID = mesh.boundaryMesh().findPatchID(patchName);
const volVectorField& U = db().lookupObject<volVectorField>("U");
const surfaceScalarField& phi = db().lookupObject<surfaceScalarField>("phi");
const volScalarField& alpha1 = db().lookupObject<volScalarField>(alphaName());
//volVectorField U("U", U);
//surfaceScalarField phi("phi", phi);
//volScalarField alpha1("alpha1", alpha1);
twoPhaseMixture twoPhaseProperties(U, phi, "alpha1");
autoPtr<incompressible::turbulenceModel> turbulence
(
incompressible::turbulenceModel::New(U, phi, twoPhaseProperties)
);
volSymmTensorField Reff(turbulence->devReff());

scalar rho = 1000;
scalar nu = 1e-06;
scalar mu = nu*rho;
scalar g = 9.81;
scalar s = 1.4;
scalar d = 0.005;
scalar shieldsc = 0.05;
scalar kappa = 0.8;
scalar c0 = 3;
//scalar Alpha1 = 0.8*mathematicalConstantPi;
scalar Alpha1 = 2;
scalarField wallShearStress = rho*mag((-mesh.Sf().boundaryField()[patchID]/mesh.magSf().boundaryField()[patchID]) & Reff.boundaryField()[patchID]);
scalarField shields = (wallShearStress)/(rho*(s-1)*g*d);
scalarField PEF = (pow((1+pow4((((1/6)*mathematicalConstantPi*mu)/(shields-shieldsc)))), -(1/4)));
scalarField linearC = sqrt(((sqr(kappa)*sqr(Alpha1))*(shields-shieldsc-((1/6)*mathematicalConstantPi*mu*PEF)))/(0.013*s*shields));
scalarField cb = c0/pow3((1+(1/linearC)));
vectorField n = patch().nf();
vectorFieldOperator=(-n*cb);

Any comments will help me a lot!
Thank you in advance!!

Access specific boundaries

I am trying to access only the z-direction boundaries of the Velocity field to set new boundary condition for the next timestep. Is there a way to do so ? I have separated the boundary fields in the input blockMeshDict file. But can we access it in the solver?

how to get field value in mesh two layers of cells inward from the boundary?

Quote:

Originally Posted by mchurchf (Post 254946)

Code:

//  Set up access to the internal velocity field and mesh

    const volVectorField& U =

        db().objectRegistry::lookupObject<volVectorField>(UName_);

    const fvMesh& mesh = patch().boundaryMesh().mesh();



    forAll(patch(), facei)

    {

    // get global cell indices for cells adjacent to patch    

        label celli = patch().faceCells()[facei];



    // get global face indices for faces opposite patch face

    label oppFacei = mesh.cells()[celli].opposingFaceLabel(facei+patch().patch().start(),mesh.faces());



    // get coordinates of center of cell adjacent to patch (patch cells)

    vector cellCentreO = mesh.cellCentres()[mesh.owner()[oppFacei]];



    // get coordinates of center of cell on the side opposite the patch of

    // the patch cell

    vector cellCentreN = mesh.cellCentres()[mesh.neighbour()[oppFacei]];



    // get coordinates of center of face opposite the patch boundary face

    vector faceCentre  = mesh.faceCentres()[oppFacei];



    // get coordinates of center of patch boundary face;

    vector patchFaceCentre = mesh.faceCentres()[facei+patch().patch().start()];

    }

I followed your code and it works! However, I want to get the field values from cells that 2 layers inward from the boundary. How can I access it?

Thanks in advance.

Hao

that's been very useful - thanks

Quote:

Originally Posted by CedricVH (Post 254591)

You have the access member function const objectRegistry& db() const. Accessing for example U is done by the code:

Code:

const volVectorField& U = db().lookupObject<volVectorField>("U");

For accessing the mesh: when creating a boundary condition, you have access to the patch. You can thus access the mesh with:

Code:

const fvMesh& mesh = patch().boundaryMesh().mesh();