CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Visualization & Post-Processing Software > ParaView

[OpenFOAM] SurfaceFields on paraFoam

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree15Likes
  • 1 Post By fjgg1549
  • 1 Post By wyldckat
  • 13 Post By wyldckat

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 29, 2012, 15:53
Default SurfaceFields on paraFoam
  #1
New Member
 
Javier Garcia
Join Date: Sep 2009
Posts: 7
Rep Power: 16
fjgg1549 is on a distinguished road
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
kmou likes this.
fjgg1549 is offline   Reply With Quote

Old   February 4, 2012, 18:05
Default surfaceFields
  #2
New Member
 
Javier Garcia
Join Date: Sep 2009
Posts: 7
Rep Power: 16
fjgg1549 is on a distinguished road
Could anyone help me please?

Javier Garcia
fjgg1549 is offline   Reply With Quote

Old   February 10, 2012, 16:18
Default
  #3
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,974
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
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
Kummi likes this.
__________________
wyldckat is offline   Reply With Quote

Old   February 10, 2012, 20:19
Default
  #4
New Member
 
Javier Garcia
Join Date: Sep 2009
Posts: 7
Rep Power: 16
fjgg1549 is on a distinguished road
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
fjgg1549 is offline   Reply With Quote

Old   February 11, 2012, 12:10
Default
  #5
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,974
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
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
roenby, yanxiang, Vietazz and 10 others like this.
__________________
wyldckat is offline   Reply With Quote

Old   February 11, 2012, 17:23
Default
  #6
New Member
 
Javier Garcia
Join Date: Sep 2009
Posts: 7
Rep Power: 16
fjgg1549 is on a distinguished road
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
fjgg1549 is offline   Reply With Quote

Old   October 3, 2016, 18:41
Default
  #7
Member
 
Pedro
Join Date: Nov 2014
Posts: 50
Rep Power: 11
pupo is on a distinguished road
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,
pupo is offline   Reply With Quote

Old   December 5, 2016, 14:33
Default
  #8
Member
 
Camille Bilger
Join Date: Jul 2013
Posts: 43
Rep Power: 12
kmou is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
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
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
Code:
 foamToVTK -surfaceFields
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
Code:
 foamToVTK -surfaceFields
is indeed doing the job ?
Thank you for your help.
kmou is offline   Reply With Quote

Old   December 6, 2016, 05:58
Default
  #9
Member
 
Camille Bilger
Join Date: Jul 2013
Posts: 43
Rep Power: 12
kmou is on a distinguished road
sorry I realised my mistake, the file to load being VTK/surfaceFields/surfaceFields_
kmou is offline   Reply With Quote

Old   March 31, 2022, 08:49
Default
  #10
Member
 
hari charan
Join Date: Sep 2021
Location: India,hyderabad
Posts: 96
Rep Power: 4
saicharan662000@gmail.com is on a distinguished road
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.

Last edited by saicharan662000@gmail.com; April 4, 2022 at 04:58.
saicharan662000@gmail.com is offline   Reply With Quote

Reply

Tags
parafoam, paraview, surfacefields, surfacescalarfields

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[OpenFOAM] Unable to launch parafoam & boonhow ParaView 5 March 23, 2022 09:09
[OpenFOAM.com] paraFoam cannot open due to Qt issues - [Solved/Information] u2berggeist OpenFOAM Installation 2 July 2, 2018 18:03
[OpenFOAM] Problem with spaces in paraFoam execution chrisb2244 ParaView 1 November 9, 2013 16:06
[OpenFOAM] How to use paraFoam on a cluster andreas ParaView 1 March 6, 2013 18:11
[OpenFOAM] OpenFoam (Ubuntu): paraFoam via Xming+PuTTY raketenmaid ParaView 4 February 5, 2013 06:20


All times are GMT -4. The time now is 05:01.