CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ParaView (http://www.cfd-online.com/Forums/paraview/)
-   -   Mapping in ParaView (http://www.cfd-online.com/Forums/paraview/125090-mapping-paraview.html)

Steph44 October 18, 2013 10:12

Mapping in ParaView
 
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

wyldckat October 19, 2013 04:31

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

Steph44 October 21, 2013 03:03

Thank you for your answer Bruno!
Please send me your email adress in a private message to provide you a example.
Stéphane

wyldckat October 26, 2013 10:39

2 Attachment(s)
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: http://www.cfd-online.com/Forums/ope...tml#post458475 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 :rolleyes:

Best regards,
Bruno

Steph44 October 26, 2013 15:36

1 Attachment(s)
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
Attachment 26392

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

wyldckat October 26, 2013 16:01

1 Attachment(s)
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

wyldckat October 26, 2013 17:11

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


All times are GMT -4. The time now is 23:21.