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

[OpenFOAM] Merged results on zero thickness surfaces

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

Like Tree1Likes
  • 1 Post By Flowkersma

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 12, 2020, 04:39
Default Merged results on zero thickness surfaces
  #1
New Member
 
Ben Gherardi
Join Date: Jun 2016
Posts: 17
Rep Power: 9
BenGher is on a distinguished road
Hello to all,


I am puzzled by an issue found while post-processing OpenFOAM cases, more specifically when trying to see contours of any values on zero thickness surfaces.



The 2 sides of the surface seem to be merged in one in paraview, and therefore the results look like a checkerboard.



Even with the motorBike tutorial, simply doing:
  • Run motorBike tutorial
  • "touch open.foam"
  • open "open.foam" in paraview
I get the results on the pictures attached (pressure).


Did any one of you encountered the same issue in the past? I have been looking for answers on this website and internet for a bit now, but it doesn't seem common.


Thanks.


Ben
Attached Images
File Type: jpg bike_surface.jpg (80.5 KB, 10 views)
File Type: jpg mudguard_surface_zoom.jpg (67.3 KB, 6 views)
File Type: png mudguard_wireframe_zoom.png (153.6 KB, 7 views)
BenGher is offline   Reply With Quote

Old   August 12, 2020, 11:20
Default
  #2
Senior Member
 
Mikko
Join Date: Jul 2014
Location: The Hague, The Netherlands
Posts: 243
Rep Power: 12
Flowkersma is on a distinguished road
Hi Ben,

You have two overlapping surfaces and that is why this is happening. You could try to move each surface a tiny bit in the normal direction. This would effectively give a small "thickness" to the surface and you would get rid of this problem.

Best, Mikko
Flowkersma is offline   Reply With Quote

Old   August 13, 2020, 04:08
Default
  #3
New Member
 
Ben Gherardi
Join Date: Jun 2016
Posts: 17
Rep Power: 9
BenGher is on a distinguished road
Hi Mikko,


The problem is that I don't have 2 surfaces, it is indeed only one surface ( like a baffle ) but with results on the 2 sides.


As you say, on surfaces enclosing volumes there is no problem, however on any occasion where there is a zero thickness surface/baffle, this error appears.


Also, I am mentioning the motorBike's tutorial because I was surprised to find this post-processing issue with it, in the sense that is seems to be a core problem and not a problem linked to a bad setup I did on a random case.


Best,


Ben
__________________
Enjoy the flow
BenGher is offline   Reply With Quote

Old   August 13, 2020, 04:43
Default
  #4
Senior Member
 
Mikko
Join Date: Jul 2014
Location: The Hague, The Netherlands
Posts: 243
Rep Power: 12
Flowkersma is on a distinguished road
Each boundary face can have only one solution so there are two overlapping surfaces. If you move the surfaces a tiny bit in the normal direction, it will help. There is no issue with the case, it is an issue in the way you are post-processing the case. Find attached an example figure of the windshield.

Best, Mikko
Attached Images
File Type: png windshield.png (33.5 KB, 13 views)
Flowkersma is offline   Reply With Quote

Old   August 13, 2020, 06:36
Default
  #5
New Member
 
Ben Gherardi
Join Date: Jun 2016
Posts: 17
Rep Power: 9
BenGher is on a distinguished road
Thanks! However how do you decompose the single mesh region into 2 surfaces?



Best,


Ben
__________________
Enjoy the flow
BenGher is offline   Reply With Quote

Old   August 13, 2020, 06:54
Default
  #6
New Member
 
Ben Gherardi
Join Date: Jun 2016
Posts: 17
Rep Power: 9
BenGher is on a distinguished road
Turns out I found a seemingly even quicker way, clicking everywhere trying to separate the mesh into surfaces.



In the options of the imported .foam case, there is a "Backface Styling" block, and modifying the default "Follow Frontface" to "Cut Frontface" seems to do the trick.



However, I am still interested on how you implement your solution by offsetting one surface of a mesh region only. Cannot find how to extract it so far.


Best,


Ben
Attached Images
File Type: jpg Comparison_follow_cut_.jpg (85.7 KB, 10 views)
__________________
Enjoy the flow
BenGher is offline   Reply With Quote

Old   August 13, 2020, 07:47
Default
  #7
Senior Member
 
Mikko
Join Date: Jul 2014
Location: The Hague, The Netherlands
Posts: 243
Rep Power: 12
Flowkersma is on a distinguished road
The way you resolved the problem is better. In my case I just calculated the surface normals (calculate surface normals filter) and then moved the surfaces in that direction (warp by vector filter).
BenGher likes this.
Flowkersma is offline   Reply With Quote

Old   August 13, 2020, 11:31
Default
  #8
New Member
 
Ben Gherardi
Join Date: Jun 2016
Posts: 17
Rep Power: 9
BenGher is on a distinguished road
Thanks for the method, because mine seems to work with openfoam cases, but not fully when trying to post-process on paraview files exported from fluent ( ensight gold export ).
__________________
Enjoy the flow
BenGher is offline   Reply With Quote

Reply

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
Strange temperature results with chtMultiRegionSimpleFoam in OF4 Wolfgang57 OpenFOAM Running, Solving & CFD 4 February 7, 2024 08:39
Extracting results on multiple surfaces sunilpatil FLUENT 0 October 21, 2018 12:15
Save Results automatically by APDL Command ansyxyz ANSYS 1 June 5, 2018 09:16
How can I get the boundary thickness out of CFD results? PeterShi Main CFD Forum 2 September 6, 2017 03:17
Creating a tool to interpolate results Luis Batista OpenFOAM Running, Solving & CFD 2 April 11, 2013 09:15


All times are GMT -4. The time now is 20:29.