[mathslw]

Hi all,

I want to use the velocity at boundary cells and velocity at the boundary face.
I found that this code "const fvPatchField<vector>& Up = patch().lookupPatchField<volVectorField, vector>("U");" could obtain the velocity vector at the boundary face.
Is there any similar code to obtain the velocity vector at the boundary cell? or other methods?

Many thanks!

Mathslw

[ybapat]

Hello,

patch.faceCells() will give you list of cells adjecent to boundary. To get adjecent cell for a face, do patch.faceCells()[facei]. Using this cell id and volVectorField U you can access value of velocity in the cell.

Regards,
-Yogesh

[Arnoldinho]

Another way to directly access the patch-nearest cells is to use U.boundaryField()[patchi].patchInternalField(), whereas patchi is your patch id which is found using const label patchi = mesh.boundaryMesh().findPatchID("bottom").

[mathslw]

Originally Posted by ybapat

Hello,

patch.faceCells() will give you list of cells adjecent to boundary. To get adjecent cell for a face, do patch.faceCells()[facei]. Using this cell id and volVectorField U you can access value of velocity in the cell.

Regards,
-Yogesh

Hi Yogesh,

According you your suggestion, I write the following:
const labelList cells = patch().faceCells();
vectorField Uac = Ua[cells];
Is that right?

Thanks!

Wei

[mathslw]

Originally Posted by Arnoldinho

Another way to directly access the patch-nearest cells is to use U.boundaryField()[patchi].patchInternalField(), whereas patchi is your patch id which is found using const label patchi = mesh.boundaryMesh().findPatchID("bottom").

Do you mean "U.boundaryField()[patchi].patchInternalField()" is the velocity vector?
Thanks!

Wei

[mathslw]

Originally Posted by ybapat

Hello,

patch.faceCells() will give you list of cells adjecent to boundary. To get adjecent cell for a face, do patch.faceCells()[facei]. Using this cell id and volVectorField U you can access value of velocity in the cell.

Regards,
-Yogesh

Hi Yogesh,

According you your suggestion, I write the following:

const fvPatchField<vector>& Uf =
patch().lookupPatchField<volVectorField, vector>("U");
const labelList cells = patch().faceCells();
vectorField Uc = U[cells];

Is that right?

Thanks!

Wei

[ybapat]

Hello Wei,

You need to loop over cellList to access value of individual cell.
forAll(cells,celli)
{
vector Ui = U[celli]
}

If you need directly field of boundary velocities, better option is suggested by Arne in his post.

Regards,
-Yogesh

[mathslw]

Originally Posted by ybapat

Hello Wei,

You need to loop over cellList to access value of individual cell.
forAll(cells,celli)
{
vector Ui = U[celli]
}

If you need directly field of boundary velocities, better option is suggested by Arne in his post.

Regards,
-Yogesh

Hi Yogesh,

Actually, I want to modify the boudary condition define in the adjointShapeOptimizationFoam. The original code is as following:

const fvsPatchField<scalar>& phiap =
patch().lookupPatchField<surfaceScalarField, scalar>("phia");
const fvPatchField<vector>& Up =
patch().lookupPatchField<volVectorField, vector>("U");
scalarField Un(mag(patch().nf() & Up));
vectorField UtHat((Up - patch().nf()*Un)/(Un + SMALL));
vectorField Uan(patch().nf()*(patch().nf() & patchInternalField()));
vectorField:perator=(phiap*patch().Sf()/sqr(patch().magSf()) + UtHat);

In this code, it uses the velocity on the boundary face and there is no loop. Then I want to use the velocity at the boundary cell, in the same way, I think there should not have any loop. Do you have any idea about that? Moreover, I also need the gradient of the velocity at the boundary cell, can I use volTensorField gradUc=fvc::grad(Uc) if Uc is the velocity at the boundary cell.

Many thanks!

Wei

[mathslw]

Originally Posted by ybapat

Hello Wei,

You need to loop over cellList to access value of individual cell.
forAll(cells,celli)
{
vector Ui = U[celli]
}

If you need directly field of boundary velocities, better option is suggested by Arne in his post.

Regards,
-Yogesh

Hi Yogesh,

Actually, I am trying to program a BC class.
I found that the following code could obtain the velocity at the boundary cell:

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

What about if I want the gradient of this velocity at the boundary cell?

Thanks!

Wei

[ybapat]

Hello Wei,

const volVectorField& Uc = db().lookupObject<volVectorField>("U") would give you velocity field over entire domain. To get at boundary you need to do as Arne suggested in his post

U.boundaryField()[patchi].patchInternalField().

About gradient I am not very sure, but I think you need to calculate it and then use it by accessing its patch internalField in the same way as for velocity.

Regards,
-Yogesh

[mathslw]

Originally Posted by ybapat

Hello Wei,

const volVectorField& Uc = db().lookupObject<volVectorField>("U") would give you velocity field over entire domain. To get at boundary you need to do as Arne suggested in his post

U.boundaryField()[patchi].patchInternalField().

About gradient I am not very sure, but I think you need to calculate it and then use it by accessing its patch internalField in the same way as for velocity.

Regards,
-Yogesh

Hi Yogesh,

Thanks for your reply!
If I use U.boundaryField()[patchi].patchInternalField(), the code would be:

vectorField& Uac = U.boundaryField()[patch()].patchInternalField();?

Since this is in the BC class, can I use patch() here?
When I compiled, I was told ‘U’ was not declared in this scope. Then how can I declare the U here.

Many thanks!

Wei

[hawkeye321]

Is there any way (any function) to get the value of a parameter at the east and north of a specific cell?

[alimea]

Hi
Basikly, how can I access to value of a quantity like U in a cell?

thanks

[fedvasu]

Originally Posted by alimea

Hi
Basikly, how can I access to value of a quantity like U in a cell?

thanks

const scalarField& UCells = U.internalField();

forAll(UCells,CellI)
{
UCells[CellI];
}

you can find it in many places in OpenFOAM source.

is that what you want?

[alimea]

Originally Posted by fedvasu

const scalarField& UCells = U.internalField();

forAll(UCells,CellI)
{
UCells[CellI];
}

you can find it in many places in OpenFOAM source.

is that what you want?

Yes, thank you my friend