|
[Sponsors] |
[OpenFOAM] Merged results on zero thickness surfaces |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
August 12, 2020, 04:39 |
Merged results on zero thickness surfaces
|
#1 |
New Member
Ben Gherardi
Join Date: Jun 2016
Posts: 17
Rep Power: 9 |
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:
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 |
|
August 12, 2020, 11:20 |
|
#2 |
Senior Member
Mikko
Join Date: Jul 2014
Location: The Hague, The Netherlands
Posts: 243
Rep Power: 12 |
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 |
|
August 13, 2020, 04:08 |
|
#3 |
New Member
Ben Gherardi
Join Date: Jun 2016
Posts: 17
Rep Power: 9 |
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 |
|
August 13, 2020, 04:43 |
|
#4 |
Senior Member
Mikko
Join Date: Jul 2014
Location: The Hague, The Netherlands
Posts: 243
Rep Power: 12 |
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 |
|
August 13, 2020, 06:36 |
|
#5 |
New Member
Ben Gherardi
Join Date: Jun 2016
Posts: 17
Rep Power: 9 |
Thanks! However how do you decompose the single mesh region into 2 surfaces?
Best, Ben
__________________
Enjoy the flow |
|
August 13, 2020, 06:54 |
|
#6 |
New Member
Ben Gherardi
Join Date: Jun 2016
Posts: 17
Rep Power: 9 |
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
__________________
Enjoy the flow |
|
August 13, 2020, 07:47 |
|
#7 |
Senior Member
Mikko
Join Date: Jul 2014
Location: The Hague, The Netherlands
Posts: 243
Rep Power: 12 |
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).
|
|
August 13, 2020, 11:31 |
|
#8 |
New Member
Ben Gherardi
Join Date: Jun 2016
Posts: 17
Rep Power: 9 |
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 |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
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 |