CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ParaView

Mapping in ParaView

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 18, 2013, 10:12
Default Mapping in ParaView
  #1
New Member
 
Stephane
Join Date: Oct 2013
Posts: 4
Rep Power: 3
Steph44 is on a distinguished road
Dear all
I would like to tranfer pressure distribution from CFD meshing to FE meshing.
I used Resample command but I don't have the expected distribution?

Do you know a specific methodology to do that?

Thanks
Steph44 is offline   Reply With Quote

Old   October 19, 2013, 04:31
Default
  #2
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,507
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings Stephane,

If you can provide a simple example of the mesh with CFD data and the mesh without any data, I can give it a try.

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   October 21, 2013, 03:03
Default
  #3
New Member
 
Stephane
Join Date: Oct 2013
Posts: 4
Rep Power: 3
Steph44 is on a distinguished road
Thank you for your answer Bruno!
Please send me your email adress in a private message to provide you a example.
Stéphane
Steph44 is offline   Reply With Quote

Old   October 26, 2013, 10:39
Default
  #4
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,507
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings Stéphane,

Since I ended up not giving you my email address and you didn't give me a link to a Dropbox file or similar, and because of a question asked in this post: Paraview slice type - cylinder? post #24, here's what I've done to create a similar situation:
  1. Used OpenFOAM to ran its tutorial "incompressible/icoFoam/cavity". It provides data for both points and cells.
  2. I created a dummy tessellated mesh by using the following steps:
    1. The tutorial has the dimensions of 0.1 x 0.1 x 0.01, so I used the "Source" named "Box" and created a box with the same dimensions and position.
    2. Then used the "Triangulate" filter.
    3. And to the previous one I used the "Subdivide" filter, so that I would have a good surface mesh.
    4. Then used "File -> Save Data" and saved to STL.
    5. I then removed the items used for generating the STL and loaded the STL back into ParaView.
  3. Now with both the volume data and the dummy surface mesh loaded into ParaView, I chose the item for the tutorial "cavity.OpenFOAM" and applied the filter "Resample with DataSet". This filter asks for an input and a source, which I configured as follows (shown in the attached pictures):
    • Input: "cavity.OpenFOAM"
    • Source: "sampling_surface.stl"
  4. The result gave me the surface from "sampling_surface.stl", with interpolated data from "cavity.OpenFOAM". The only problem is that it only provided the point data and did not provide the cell data
The reason why I had asked for an example case was so that I didn't have to create one myself

Best regards,
Bruno
Attached Images
File Type: png Screenshot from 2013-10-26 15:35:59.png (29.9 KB, 36 views)
File Type: png Screenshot from 2013-10-26 15:36:02.png (31.2 KB, 24 views)
wyldckat is offline   Reply With Quote

Old   October 26, 2013, 15:36
Default
  #5
New Member
 
Stephane
Join Date: Oct 2013
Posts: 4
Rep Power: 3
Steph44 is on a distinguished road
Dear Bruno,

Thank you for your answer and test. My problem is the same, data are not at cell and I have the following problem:
see picture
image2.jpg

I don't understand why I have a red line on the back face of the half cylinder. Pressure should be constant.
I use commande Point Data to Cell data after resample command.

If you have an idea?

BR,

Stéphane
Steph44 is offline   Reply With Quote

Old   October 26, 2013, 16:01
Default
  #6
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,507
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Stéphane,

I think the problem is that a coarser mesh for the re-sampling isn't properly handled by ParaView, as shown in the attached image: on the left is the original case and on the right is a coarser surface mesh.

I'll try to find some way of controlling how the interpolation is conducted, but it will have to be done with a "Programmable Filter".

Best regards,
Bruno
Attached Images
File Type: jpg example_coarser_mesh.jpg (27.4 KB, 26 views)
wyldckat is offline   Reply With Quote

Old   October 26, 2013, 17:11
Default
  #7
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,507
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Stéphane,

If I did my research correctly, it looks like the interpolation is not configurable, even through code.
This is because the VTK filter "vtkProbeFilter" is not configurable: http://www.vtk.org/doc/release/5.8/html/a01586.html

So, the way I see it, you should use surface meshes with similar resolution, in order to minimize the differences that occurs during interpolation.

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
Installing OpenFOAM and ParaView in VirtualBox(Ubuntu on Win8) chrisb2244 OpenFOAM Installation 2 August 21, 2013 13:24
Newbie: Install ParaView 3.81 on OF-1.6-ext/OpenSuse 11.2? lentschi OpenFOAM Installation 1 March 9, 2011 03:32
Paraview not found fusij OpenFOAM Installation 2 January 1, 2011 21:44
paraFoam reader for OpenFOAM 1.6 smart OpenFOAM Installation 13 November 16, 2009 22:41
Import gmsh msh to Foam adorean Open Source Meshers: Gmsh, Netgen, CGNS, ... 24 April 27, 2005 08:19


All times are GMT -4. The time now is 14:59.