CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Paraview & paraFoam

Surface path (oilflow) in paraview

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

Like Tree2Likes
  • 2 Post By lovecraft22

Reply
 
LinkBack Thread Tools Display Modes
Old   March 17, 2012, 09:34
Default Surface path (oilflow) in paraview
  #1
Senior Member
 
lore
Join Date: Mar 2010
Location: Italy
Posts: 425
Rep Power: 8
lovecraft22 is on a distinguished road
Send a message via Skype™ to lovecraft22
Any way to have an oilflow in paraview?

Something quite like this:



Thanks!
__________________
I use PowerFLOW!
lovecraft22 is offline   Reply With Quote

Old   March 19, 2012, 09:18
Default
  #2
Senior Member
 
sail's Avatar
 
Vieri Abolaffio
Join Date: Jul 2010
Location: Always on the move.
Posts: 308
Rep Power: 6
sail is on a distinguished road
Ciao Lore.

have a look at this link. you should be able to adapt the methodology to your surface.

http://paraview.org/Wiki/ParaView/Custom_Filters
__________________
http://www.leadingedge.it/
Naval architecture and CFD consultancy
sail is offline   Reply With Quote

Old   March 19, 2012, 14:28
Default
  #3
Senior Member
 
lore
Join Date: Mar 2010
Location: Italy
Posts: 425
Rep Power: 8
lovecraft22 is on a distinguished road
Send a message via Skype™ to lovecraft22
Thank you Vieri;
my only concern is that what you linked is related to a section of the field i.e. a region where the velocity is not zero… In my case the surface of the body has the non slip condition, so velocity=0… Do you think I could manage to have the oilflow anyway? I tried with no luck but maybe I did something wrong…
__________________
I use PowerFLOW!
lovecraft22 is offline   Reply With Quote

Old   March 29, 2012, 16:41
Default
  #4
Senior Member
 
lore
Join Date: Mar 2010
Location: Italy
Posts: 425
Rep Power: 8
lovecraft22 is on a distinguished road
Send a message via Skype™ to lovecraft22
I eventually find a way thank to the paraview mailing list.

First of all you need to evaluate the velocity gradient at the walls of the surface shear stress by running wallGradU or wallShearStress in openFoam. Then, in paraview:
tools-->manage plugins-->surface LIC-->load selected, choose surface LIC as visualization type, then among the display options of your geometry choose what you evaluated above as the vector.
Attached Images
File Type: jpg aaaa.jpg (70.9 KB, 234 views)
Ralph M and Ivanet like this.
__________________
I use PowerFLOW!
lovecraft22 is offline   Reply With Quote

Old   July 13, 2012, 15:04
Default
  #5
Senior Member
 
Ralph Moolenaar
Join Date: Aug 2010
Location: 's-Hertogenbosch, the Netherlands
Posts: 120
Rep Power: 5
Ralph M is on a distinguished road
Hello Lore,

Thanks for your post and explanation. It's very clear for me but somehow the oilflow doesn't show up. Maybe it has to do with the paraview version that I have (v3.12) but upgrading to v13.4 doesn't work for me either.

I guess that you processed your data with foamToVTK -latestTime, opened ParaFoam and loaded the patch.vtk for which you're interested?

Thanks for the answer!

Ralph
__________________
CFD for marine applications? Go to http://www.marinecfd.com/ and join the OF Ship Hydromechanics Group: http://www.cfd-online.com/Forums/gro...mechanics.html
Ralph M is offline   Reply With Quote

Old   July 13, 2012, 16:01
Default
  #6
Senior Member
 
lore
Join Date: Mar 2010
Location: Italy
Posts: 425
Rep Power: 8
lovecraft22 is on a distinguished road
Send a message via Skype™ to lovecraft22
I think it should work either with VTK or with the built in reader. Have you selected everything as depicted in the picture I uploaded (as indicated by the yellow arrows)?
lovecraft22 is offline   Reply With Quote

Old   July 13, 2012, 16:16
Default
  #7
Senior Member
 
Ralph Moolenaar
Join Date: Aug 2010
Location: 's-Hertogenbosch, the Netherlands
Posts: 120
Rep Power: 5
Ralph M is on a distinguished road
Yep. There's only one problem. After opening paraFoam from the case by calling " paraFoam", loading data only for the surface under consideration (for which wallGradU was performed) and loading LIC from the plugins... the LIC option isn't available as visualization type.

So my question is: which patches do you load? Could you maybe send me your case of the cylinder (because my case is currently several GBs...). Thanks! ralph at marinecfd (dot) com
__________________
CFD for marine applications? Go to http://www.marinecfd.com/ and join the OF Ship Hydromechanics Group: http://www.cfd-online.com/Forums/gro...mechanics.html
Ralph M is offline   Reply With Quote

Old   July 13, 2012, 16:30
Default
  #8
Senior Member
 
lore
Join Date: Mar 2010
Location: Italy
Posts: 425
Rep Power: 8
lovecraft22 is on a distinguished road
Send a message via Skype™ to lovecraft22
I just tried and I can confirm it works both with VTK and with paraFoam. With the latter sometimes you don't get anything in the vectors drop down menu, that's a bug of paraview, simply select something else in you pipeline tree (even the firs entry, the one called builtin in my picture above) then select your patch back again and you should be able to see it working.

Also, usually I don't use paraFoam directly but I create a .foam file and then open that one in paraview.

I'll send you my case via email to you right away!
lovecraft22 is offline   Reply With Quote

Old   July 16, 2012, 14:54
Default
  #9
Senior Member
 
Ralph Moolenaar
Join Date: Aug 2010
Location: 's-Hertogenbosch, the Netherlands
Posts: 120
Rep Power: 5
Ralph M is on a distinguished road
Somehow the trick doesn't work on my Linux machine. Also an installation of Paraview on a windows machine doesn't yield the desired effect. There's no error but nothings shows up, even after some support by Lovecraft22. Anyone some clues how to solve this?

I've got Ubuntu 10.04 on the computer where I tried ParaView 3.12 (no special graphics card, 4 processors, 8GB memory), on my windows machine (less capable in every way compared to the Linux machine) I tried version 3.14.
__________________
CFD for marine applications? Go to http://www.marinecfd.com/ and join the OF Ship Hydromechanics Group: http://www.cfd-online.com/Forums/gro...mechanics.html
Ralph M is offline   Reply With Quote

Old   August 17, 2012, 05:48
Default
  #10
New Member
 
Thibault
Join Date: Aug 2010
Posts: 1
Rep Power: 0
fougere is on a distinguished road
Hi,

As Sail was saying the method explained here works:
http://paraview.org/Wiki/ParaView/Custom_Filters

To make it work, you only need to select wallShearStress or WallGradU for the SurfaceVectors filter instead of U which is null on the surface.

After that you can apply the MaskPoints filter and use the StreamTracerWithCustomSource filter on the SurfaceVectors.

Using this method I obtain more satisfying results than with the LIC method.

Regards,
Thibault
fougere is offline   Reply With Quote

Old   January 13, 2014, 11:43
Default
  #11
Member
 
Ye Zhang
Join Date: Dec 2009
Location: Delft,Netherland
Posts: 75
Rep Power: 6
kiddmax is on a distinguished road
HI Ralph

Did you find the solution? I have the exactly the same question with you!

Thanks!

Best regards,
Ye
kiddmax is offline   Reply With Quote

Old   January 18, 2014, 10:02
Default
  #12
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 6,983
Blog Entries: 32
Rep Power: 68
wyldckat is a jewel in the roughwyldckat is a jewel in the roughwyldckat is a jewel in the rough
Greetings to all!

@Ye: Are you referring to this question?
Quote:
Originally Posted by Ralph M View Post
So my question is: which patches do you load?
Can you show which patches you've selected? Or in other words: did you select only the surface patches or did you choose the internal mesh only?

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Create surface from points in Paraview Voyage_gui ParaView 0 December 12, 2011 11:10
[ICEM] Generating surface from spline (error) TKE ANSYS Meshing & Geometry 0 October 27, 2011 06:21
OF 1.6 | Ubuntu 9.10 (64bit) | GLIBCXX_3.4.11 not found piprus OpenFOAM Installation 22 February 25, 2010 13:43
solid edge problem....can you help? cindy Main CFD Forum 3 April 5, 2004 13:43
free convection heat transfer from a heated horizontal surface through a liquid to a thin cooled fin Kaushik FLUENT 1 May 8, 2000 06:47


All times are GMT -4. The time now is 13:37.