[l_r_mcglashan]

Sorry for the late reply, I've been really busy!
I'm not sure why you're getting the behaviour that you observe. Possibly U has gone out of scope or something? The write() function just writes the current U field to the 0/U file.
I'd probably need to see it for myself, feel free to post your files in a tarball and I can take a quick look.

[santiagomarquezd]

Thanks Laurence for your attention even with all your work. Well, this is the code:

// Velocity field initialization

// Angular velocity
scalar omega=2000;

// Maximum velocity en parabolic profile
scalar Vmax=2.0;

// Tube radius
scalar tubeR=0.05;

// Cell centroid coordinates
const volVectorField& centres = mesh.C();

// Coordinate system origin
point origin(0, 0, 0);

// Axis of rotation
vector axis(0, 0, 1);

// Force arm calculation
vectorField palanca;

palanca = centres.internalField() - ((centres.internalField()-origin) & axis)*axis;


// Parabolic velocity field calculation
scalarField zComp=Vmax*(1-sqr(mag(palanca)/tubeR));

// Option with rotation and the parabolic
// Rotation
U.internalField()=omega*(axis^palanca);
// Parabolic in z direction
U.internalField().replace(vector::Z,zComp);

// Write to /0/U
U.write();

The sequence of includes is that follows:

#   include "createTime.H"
#   include "createMesh.H"
#   include "createFields.H"

#   include "USetUp.H"

(mine is the last one, added in scalarTransportFoam.C)

As you can see, after rewriting in memory the U vector field I call the .write() method to write the field to the hard disk. The problem is that if you run the code once, the initializated U field doesn't remain in memory, i.e. the advection equation is solved with another field, maybe zero, I don't
know. But, in the other hand, if you run the code some steps, then stop it and run it again with the /0/U recently written things go well.

That's all. Regards.

[l_r_mcglashan]

This worried me slightly, so I took a look, and I think I've figured it out.

The scalar transport equation takes phi as the coefficient in fvm::div, not U. So you have overwritten U, but now you have to recreate the flux.

So just put

#include "createPhi.H"

below

#include "USetUp.H"

Hope that's the problem.

[santiagomarquezd]

Laurence, I've been working in another things last months but I've returned to this problem. Your suggestion was right, FOAM was assembling the flux with the original U not with the one calculated by my code. I had to put the

#include "createPhi.H"

below

#include "USetUp.H"

Nevertheless it is necessary to comment the original invocation of createPhi.H file in createFields.H because the

#ifndef createPhi_H

clause within createPhi.H. As you know, this line impedes that definition can be repeated.

Regards.

[wzx1989221]

Dear Santiago,

I am struggling with getting a parabolic internal field for pipe flow in openfoam and I've found your post very useful.
Could you please give me some hints on the line "U.internalField()=omega*(axis^palanca);" ?
Another silly question, where shall I put the code, in 0/U or somewhere else? Do I need to derive my own solver for it?
I really appreciate your reply. Thank you very much.

Best regards,
Tony

[wyldckat]

Greetings to all!

FYI for future readers: Tony's question has been in essence answered here: http://www.cfd-online.com/Forums/ope...tml#post468380


@Tony: Regarding your question about Santiago's implementation: from what I can figure out from the first few posts, it seems that he created a variant of the solver scalarTransportFoam and added a new header file that includes the code discussed in this thread.

It takes a while to explain it in more detail, so I suggest that you have a look at the following tutorials, in order to get a bit more perspective into the details:

• http://openfoamwiki.net/index.php/Ho...ure_to_icoFoam
• http://openfoamwiki.net/index.php/ScalarTransportFoam

In fact, you'll see that those two tutorials are similar to each other, since the first one implements the explanation given in the second one.


Best regards,
Bruno

[wzx1989221]

Hi, Bruno

Thank you very much for the information. I will have a look at that and get back to you if I have further questions.

Best regards,
Tony