Hi: I am running icoFoam
I am running icoFoam. However, wanted to compute the turbulent variable 'nuSGS' without using the turbulence model. I tried to compute the following way:
surfaceScalarField nusgs = sqrt(mesh().V()/thickness)*symm(grad(U));
computing the thickness variable as given in LESdeltas, but was not able to work it out.
some errors include:
error: no match for call to (Foam :: fvMesh) ()
error: grad was not declared in this scope..
Can someone elaborate on how to obtain this quantity?
further, in the incompressible code, Can i Add this computed field to constant "nu" to make it an effective nueff = nu+nusgs.
Why mesh().V() instead of mesh
Why mesh().V() instead of mesh.V()? I would also say Foam::sqrt and the rest looks OK.
Hello Hrv: I tried to imple
I tried to implement your suggestions. on Compiling, I received following errors:
error: no match for 'operator*' in 'Foam::operator*(const Foam::scalar&, const Foam::tmp<foam::field<type> >&) [with Ty
pe = double](((const Foam::tmp<foam::field<double> >&)((const Foam::tmp<foam::field<double> >*)(& Foam::sqrt(const Foam::UList<double>
&)())))) * Foam::symm(const Foam::GeometricField<foam::tensor<double>, PatchField, GeoMesh>&) [with PatchField = Foam::fvPatchField, G
eoMesh = Foam::volMesh]()'
I am not able to access mesh volume for some reason. Please let me know your thoughts on this.
Split it up and try bits of th
Split it up and try bits of the expression - not obvious like his...
I tried to compute mesh.V(), m
I tried to compute mesh.V(), mesh().V(),I keep getting the same error Foam::fvMesh problem.
Is there any other way to access the cell structure?
Actually, now that I look at t
Actually, now that I look at this, it is so full of rubbish that I should not have bothered to answer in the first place. Let's just go slowly through it.
1) so, U is a volVectorField, right. Thank makes fvc::grad(U) a volTensor field. You forgot the fvc:: bit in the grad; I will discuss the type of result further
2) symm(fvc::grad(U)) is still a volTensorField (well, a symmetric tensor, but we've still haven't got that one). Fine.
3) mesh.V(), according to fvMesh.H returns a scalar field:
//- Return cell volumes
const scalarField& V() const;
Note that V() gives you cell volumes, so it does not have any boundary conditions.
4) I sincerely hope that thickness is also a scalarField. If so, Foam::sqrt(mesh.V()/thickness) will give you a scalar field. Not clear if you've tried that.
5) So, now we've got:
which would be a scalarField times a volTensorField. How do you imagine I will deal with the boundary conditions: the gradient is defined on the boundary, but the scale is not. In other words, this is a completely wrong operation - the best I can do for you is to multiply the internal field of the gradient with the scalar field and let you deal with the boundary conditions yourself. Thus:
Info<< "Reading field U\n" << endl;
scalarField thickness(mesh.V().size(), 3.73);
volTensorField a = fvc::grad(U);
scalarField t = Foam::sqrt(mesh.V()/thickness);
volTensorField b = fvc::grad(U);
b.internalField() *= t;
6) and finally, the best one of all:
surfaceScalarField nusgs = all this lot! How did you imagine that a surfaceScalarField (one scalar for all faces) can be initiated from a product of a scalar field and a tensor field? scalar = tensor??? Hmm. What happened to interpolation: how do I get face value from celll values?
I think some serious thought is required before continuing :-)
Enjoy (and sorry about the tone),
|All times are GMT -4. The time now is 06:19.|