[suman91]

Hi there,

I am currently running a flow over backward facing step (using LES) in OpenFAOM 2.4.0. I want access to the kinematic viscosity. So in a ".H" file which I include in pisoFoam.C, I write the following just to see if I have access to nu (kinematic viscosity) value:

double k_viscosity;
const scalarField& nuCells = nu().internalField();
forAll(mesh.cells(), celli)
{
    k_viscosity = nuCells[celli];;
    Info<< "nu = " << k_viscosity << endl;
}

But during compiling i get error: "error: ‘nu’ was not declared in this scope"

I also want to access the nut values calculated by the solver. Is there a function to access it ?

Thanks in advance.

[Bloerb]

There is no volScalarField called nu. nu is part of the turbulence model because most of those use calculate an effective viscosity by adding a turbulent one. This is the nut file. Check those on how to access it. The correct way should be
turbulence->nu() and turbulence->nut() for the turbulent viscosity

[suman91]

Hi,

Thank you for the reply. Will turbulence->nu() return a double value? I was trying out this command only and got an error like :

"Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> >’ to ‘double’ in initialization"

Just by printing using:
Info<<"\n nu value is"<<turbulence->nu();


I get output:

nu value is dimensions [0 2 -1 0 0 0 0];

internalField uniform 0.00035714;

How to access only the scalar value ?

[suman91]

Hi again,

Able to access nu().

The "createFields.H" file had a line:

singlePhaseTransportModel laminarTransport(U, phi);

So it is creating an object named laminartransport of type singlePhaseTransportModel

Inside singlePhaseTransportModel.H, there sits a member function

virtual tmp<volScalarField> nu() const;

So if I write:

const volScalarField k_viscosity = laminarTransport.nu();
double viscosity;
forAll(mesh.cells(), celli)
{
    viscosity = k_viscosity[celli];
    Info<< "\ncell number in list = " << celli << endl;
    Info<< "nu = " << viscosity << endl;
}

Then am getting the nu value for each cell.

[suman91]

Better approach:
Using the turbulenceModel object to access the viscosity rather than singlePhaseTransportModel.

const volScalarField k_viscosity = turbulence->nu(); double viscosity; forAll(mesh.cells(), celli) {     viscosity = k_viscosity[celli];     Info<< "\ncell number in list = " << celli << endl;     Info<< "nu = " << viscosity << endl; }

Similar process can be used to access nut():

const volScalarField nu_t = turbulence->nut();
forAll(mesh.cells(), celli)
{
    Info<< "nut = " << nu_t[celli] << endl;
}

[albet]

Hello,
I am calculating nut from two different ways, but the values are different. Could anybody explain why they give me different values please?

1.
volScalarField nu_t (turbulence -> nut());

2.
volScalarField& nut = const_cast<volScalarField&>
(mesh.lookupOblect<volScalarField>("nut"));


Regards,
Amir

[zwlwf]

Originally Posted by albet

Hello,
I am calculating nut from two different ways, but the values are different. Could anybody explain why they give me different values please?

1.
volScalarField nu_t (turbulence -> nut());

2.
volScalarField& nut = const_cast<volScalarField&>
(mesh.lookupOblect<volScalarField>("nut"));


Regards,
Amir

Hello albet,

In my opinion, the first one calls a copy constructor, which just copy the value of nut. This means the nu_t is an different object with nu, the second is a referrence to nut itself. During the simulation, the nu with be updated with time, so they may have different value.

[albet]

Originally Posted by zwlwf

Hello albet,

In my opinion, the first one calls a copy constructor, which just copy the value of nut. This means the nu_t is an different object with nu, the second is a referrence to nut itself. During the simulation, the nu with be updated with time, so they may have different value.

Many thanks for your reply.
I used these methods in every iteration of my simulation to have access to nut. Could you please let me know which one gives me the correct nut in every iteration?
Kind regards,
Amir

[zwlwf]

I think the second one is what you want.

and I think if you write the first one as :

volScalarField& nu_t  = turbulence -> nut();

these two way should have same result.

[albet]

Originally Posted by zwlwf

I think the second one is what you want.

and I think if you write the first one as :

volScalarField& nu_t  = turbulence -> nut();

these two way should have same result.

Many thanks. You are right!
based on the error I received, I think this form is correct:

const volScalarField& nu_t  = turbulence -> nut();

Kind regards,
Amir