[hjasak]

That's because you're in the code you are setting the patch value of the fixedGradientFvPatchScalar field:

fixedGradientFvPatchScalarField& buffer=
refCast<fixedgradientfvpatchscalarfield>(T.boundar yField()[patchI]);
forAll (buffer, faceI)
{
buffer[faceI] = 0.1*(293.-T.boundaryField()[patchI][faceI]);
}

and you should be setting the gradient() instead. Have a look at fixedGradientFvPatchField.H.

So:

fixedGradientFvPatchScalarField& buffer=
refCast<fixedgradientfvpatchscalarfield>(T.boundar yField()[patchI]);
scalarField& grad = buffer.gradient();

forAll (grad, faceI)
{
grad[faceI] = 0.1*(293.-T.boundaryField()[patchI][faceI]);

}

(if that is what you want).

Enjoy,

Hrv

[tehache]

with the above, I get a compilation error: "missing template arguments before '&' token".
I realize its a template, but what type should I pass ?

Thanks for any hint, I am new to this ...

Thomas

[hjasak]

refCast<fixedgradientfvpatchscalarfield>

is the stuff in angle brackets really all lowercase (wrong) or is the user group software playing tricks with me?

Hrv

[tehache]

fixedGradientFvPatchScalarField<scalar>& buffer=
refCast<fixedgradientfvpatchscalarfield<scalar> >(T.boundaryField()[patchI]);
scalarField& grad = buffer.gradient();


the stuff is not lowercase, but somehow converted to lowercase on posting, I just realized.

[hjasak]

Get rid of the <scalar> bit - fixedGradientFvPatchScalarField is already typedef'd to be of scalar (as the name says). Also, compare:

Yours:

fixedGradientFvPatchScalarField<scalar>& buffer=

Mine:

fixedGradientFvPatchScalarField& buffer=

which rather gives it away.

It's a bit hard like this - in the future, can we have the piece of code and the actual error message, with the line number etc.

Enjoy,

Hrv

[vitke]

Hi all

I am trying to cast

fvPatchScalarField& pp = p.boundaryField()[patchi];
fixedGradientFvPatchScalarField& ppatch = refCast<fixedGradientFvPatchScalarField>(pp);

because I want to set

ppatch.gradient()[i] = ...

but I'm getting this error:

‘fixedGradientFvPatchScalarField’ was not declared in this scope

Is this solution outdated?

[prabhu]

I am currently facing problems when calculating heat transfer values at boundary which is used for flux boundary condition.

I am fixing the heat transfer co-efficient in cells based on the value of temperature. When doing this the values are fixed in the cells but the values at the boundary are zero.
I made some changes as

label patchI = mesh.boundaryMesh().findPatchID("leftmovingwall");
zeroGradientFvPatchScalarField& bufferh = refCast<zeroGradientFvPatchScalarField>(hT.boundar yField()[patchI]);
forAll (bufferh, faceI)
{
if (T.boundaryField()[patchI][faceI] < Tmin_hT.value())
{
bufferh[faceI] = hT_Tmin.value();
}
else if (T.boundaryField()[patchI][faceI] >= Tmin_hT.value())
{
bufferh[faceI] = hT_Tmax.value();
}
}

The compilation of code did not produce any error but when i start the simulation i get the following error :


Attempt to cast type calculated to type zeroGradient#0 Foam::error:rintStack(Foam::Ostream&) in "/apps/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/apps/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 main in "/home/prabhu/OpenFOAM/prabhu-1.5/applications/bin/linux64GccDPOpt/lasersolid"
#3 __libc_start_main in "/lib64/libc.so.6"
#4 Foam::regIOobject::readIfModified() in "/home/prabhu/OpenFOAM/prabhu-1.5/applications/bin/linux64GccDPOpt/lasersolid"
From function refCast<To>(From&)
in file /apps/OpenFOAM/OpenFOAM-1.5/src/OpenFOAM/lnInclude/typeInfo.H at line 106.
FOAM aborting
Abort

Could any1 tell me how can this problem be solved?