[skabilan]

Hi All,

How do I initialize a problem where T is a field, not a single value at the boundary in case of scalarTranportfoam?

Thanks
Senthil

[smehdi609]

Hi Senthil,
I usually get a reference to the scalar field and initialize it. In this way you have to change the application and recompile it.
You can also use funkySetFields utility. You can find information about it in forum and wiki. I have never used it.
Cheers,
Mahdi

[skabilan]

Hi Mahdi,

Thanks for your valuable input. I need some more help with the reference to scalar field. How can I go about doing that? Is there an example that you can share with me?

Thanks in advance
Senthil

[ngj]

Hi Senthil

If the distribution can be given in some algebraic way as a function of location, then I suggest that you go for the funkySetField application.

See the following thread for information/inspiration :

http://www.cfd-online.com/OpenFOAM_D...es/1/6821.html

There is also a wiki, but I have problems connecting to it, but I believe the link is in the above thread.

Have fun,

Niels

[smehdi609]

Hi Senthil,
It's pretty simple. Let's say you have a scalar field T and you want to initialize it with a parabolic function of y; you may write:

volScalarField yPos = mesh.C().component(vector::Y);
forAll(T, counter)
{
T[counter] = yPos[counter]*(1.0 - yPos[counter]);
}

This is just for the internal field. If you also want to initialize the boudaries as well, let's say you have a boundary patch named inlet, you may write:

label inletPatchID = mesh.boundaryMesh().findPatchID("inlet");
fvPatchScalarField& inletT = T.boundaryField()[inletPatchID];
const vectorField& faceCentresInlet = mesh.Cf().boundaryField()[inletPatchID];
forAll(inletT, pointI)
{
inletT[pointI] = faceCentresInlet[pointI].y()*(1.0 - faceCentresInlet[pointI].y());
}
This is the way I do it, because I usually write my own applications and rarely have complex initial conditions. If you want to do it very often, I think it's better to use funkySetField application.
Cheers,
Mahdi

[skabilan]

Hi All,

To make it a bit more clearer, I have attached a acrobat file which explains what I would like to do with the scalarTransportFoam. \attach

Thanks all in advance for your never ending help!

Cheers,
Senthil

[skabilan]

My bad!

Thanks
Senthil

[skabilan]

Sorry for a lot of messages. The file size was big

I have a complex temperature field (Figure 1). For the sake of argument, let us say it is defined by experiment and therefore is not expressible as a simple function of X, Y or Z

In my application, I need to solve for the time-dependent movement of the temperature thought the geometry, as a function of self-diffusion and convection. Previously, I have solved (not in OF) the diffusion equation of this field (Figure 2).

I also have from a previous run of OF, the separate solution of the incompressible Navier-
Stokes equation. My problem is to use the pre-defined velocity field and now
diffuse AND convect the temperature field. ScalarTransportFOAM has the right physics.
My question is how do I initialize the problem. It almost seems like a 'restart'. Note the
problem is decoupled in the sense that the velocity will influence (convect) the
temperature field, but the temperature field has NO influence on the velocities.

Hello Senthil,

>let us say it is defined by experiment and therefore is not expressible as a simple function of X, Y or Z

You'll probably have to find an interpolation of your measured (or simulated) data as a function of X,Y,Z. Just having a "complex temperature field" without any mesh and without other structure gets you nowhere.

>It almost seems like a 'restart'

It *is* a restart. Write your temperature field as initial conditions into the file yourcase/0/T and run.

Nadine