SurfaceFields on paraFoam
 

Dear Foamers,

I need to plot surfaceScalarFields (like phi) in paraFoam.

I have modified interFoam solver to create some surfaceScalarFields (openFoam 2.1.0). When I run the solver the corresponding field-files are created nicely in their respective time-folders.

I have already run foamToVTK -surfaceFields and I have got the VTK subdirectory. I have also used a Glyph filter.

My problem is that I cannot see any surfaceScalarField in the "Color by" pop-up menu. so I am unable to plot them.

Could anyone help me please?

Thanks.

Javier Garcia

surfaceFields
 

Could anyone help me please?

Javier Garcia

Greetings Javier and welcome to the forum!

If you attach one of those VTK files, or a small example case, it would be a lot easier to help you!
Otherwise, all we can do is guess: the surface scalar field probably only has vectors, but no scalars. Most you can get is coloring based on length/magnitude of the vectors.

Best regards,
Bruno

Thanks wyldckat for your reply. I am using OpenFoam 2.1.0. I need to calculate the whole volume exiting a pipe, and take it into account in order to modify the pressure within a vessel. So I took interFoam as a starting point, and I have created a surfaceScalarField in createFileds.H called localVolume:

surfaceScalarField localVolume
(
IOobject
(
"localVolume",
runTime.timeName(),
mesh,
IOobject::READ_IF_PRESENT,
IOobject::AUTO_WRITE
),
phi*scalar(0)*runTime.deltaT()
);

Field localVolume is defined as (time integral of phi):

localVolume = phi * runTime.deltaT() + localVolume;

Later, I have created a groovyBC in patch inlet for p_rgh, using a variable called exitVolume in patch atmosphere:

inlet
{
type groovyBC;
value uniform 1;
valueExpression "1/pow(1+0.001*exitVolume,1.4)";
gradientExpression "0";
fractionExpression "1";
variables "exitVolume{atmosphere}=sum(localVolume);";
}

My case runs beautifully. My only problem is that I cannot see field localVolume (neither phi) in paraFoam, because it is a surfaceScalarField and it does not appear in any of the pull-down menus of fields offered in paraFoam.
How should I proceed in order to visualize my field localVolume (or phi for that matter)? Could you, please, offer a step-by-step procedure to do so?

I shall be very grateful if you could do it.

Thanks and best regards.

Javier Garcia

Hi Javier,

OK, now I understand. These fields are only points, although we can't display them directly. The solution is somewhat simple:

1. Run foamToVTK:
   Code:

   ---

   foamToVTK -surfaceFields

   ---

2. Run paraFoam.
3. Load the surface fields base file "VTK/surfaceFields/surfaceFields_..vtk", so you can see them with the respective time snapshot.
4. Then apply the "Glyphs" filter to this file and you should see the respective points in glyph form.

Best regards,
Bruno

Thank you very much Bruno. Now I can see some nice arrows of surfaceScalarField localVolume.

You have been most helpfull.

Thanks and best regards.

Javier Garcia

Old thread, but I'm having a hard time with this one.

I can load the surface gradient field i itend to watch following Wyldcat's steps.... but i can't make them appear in the surfaces. They appear all over the place though....

Any way to control the surface the glyph appears?

Best regards,

Hi Bruno, and others :)

I am trying to perform a similar task, with a surfaceVectorField (the interface normal extracted from interfaceProperties in interFoam, that I called nHat). It is being correctly outputted to the time folders, a long list of vectors, no scalars.
I have run and loaded the VTK file,
but nHat does not appear in the drop down menu after applying the Glyph filter.

How can I check that is indeed doing the job ?
Thank you for your help.

sorry I realised my mistake, the file to load being VTK/surfaceFields/surfaceFields_

Hello kmou,
Can I know how did you extract nHat from interface properties in interfoam. I want nHatfv from interface properties. Can you tell me how to extract them.
Thanks in advance.