|
[Sponsors] |
Particle-class uses wallImpactDistance on non-wall patches |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
August 19, 2010, 07:54 |
Particle-class uses wallImpactDistance on non-wall patches
|
#1 |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
Versions: this is found in OF-Versions 1.5 till the present (1.7.x)
Description: When calculating the lambda (normalized time to impact on a patch) the wallImpactDistance (basically radius of the particle) is used to take a non-zero thickness into acount when a particle is being reflected on a wall. The problem is that the wallImpactDistance is used for all other types of patches. This leads especially for processor-patches to the problem that the exact time when the particle center crosses onto the other processor is not correctly predicted which for unfortunate circumstances (small timesteps are a big factor, then it happens even with very small particles) can lead to particles being transfered back and forth across a processor boundary (but also for symmetry-boundaries the particle never reaches the symmetry, but is reflected before it). The picture below is from an uncoupledKinematicParcelFoam-simulation (1.7.x, no modifications to the code) and illustrates the problem: unpatchedParticle.jpg (the strange blocking of the particles is a processor-boundary and is not seen in the serial version of this run) This patch checks whether a boundary-face is a wall and only then applies the impact distance: wallParticles.patch After applying the patch in the same simulation particles have no problem to "get to the other side" and the result looks like the serial computation (same decompostion as the original picture): patchedParticle.jpg (it can be discussed of course whether the impact distance is relevant for other "regular" patches but for the general case - outlet, inlet - I think the particle center is the better point of reference) Bernhard |
|
August 20, 2010, 05:17 |
|
#2 |
New Member
Andrew Heather
Join Date: Mar 2009
Posts: 16
Rep Power: 17 |
Thanks for the report - I've pushed the fix from our internal line
Andy |
|
March 21, 2011, 04:38 |
|
#3 |
Senior Member
xinguang cui
Join Date: Mar 2009
Posts: 116
Rep Power: 17 |
||
March 25, 2011, 05:37 |
|
#4 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128 |
Greetings flying,
I've looked up the commits made to the official git repo and believe the respective fix is this one: https://github.com/OpenCFD/OpenFOAM-...45ed21b5fdecd5 But this should only be necessary if you are using a version of OpenFOAM older than 1.7.1. Best regards, Bruno
__________________
|
|
March 25, 2011, 07:30 |
|
#5 | ||
Senior Member
xinguang cui
Join Date: Mar 2009
Posts: 116
Rep Power: 17 |
Dear Wyldkat:
Thanks so much for the information Quote:
Quote:
|
|||
June 5, 2011, 12:20 |
Hi Bernhard,
|
#6 | |
Member
edison
Join Date: May 2009
Location: Australia
Posts: 35
Rep Power: 16 |
Hi Bernhard,
I'm using OF1.7.1 which alrealy include your patch fix for the wallImpactDistance but still experiencing the same particle transform back and forth the processor boundary patch. I'm implementing a PDF method on OF. so the particle has no diameter and I would think the wallImpactDistance is not he only place OF got wrong. Do you have similar experience? Quote:
|
||
June 7, 2011, 07:07 |
|
#7 | |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
Quote:
|
||
January 18, 2013, 03:47 |
Tutorial for uncoupledKinematicParcelFoam
|
#8 |
New Member
Mattia
Join Date: Oct 2012
Location: Milan
Posts: 28
Rep Power: 13 |
Hello, I see that Bernhard computes a case with uncoupledKinematicParcelFoam. I'm trying to run a similar case. Could you Bernhard send me the folder of your case? because I haven't find tutorials. Thanks a lot.
Best regards. Mattia |
|
January 18, 2013, 07:20 |
|
#9 | |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
Quote:
Anyway: 2.1 has a tutorial in lagrangian/icoUncoupledKinematicFoam. My proposal: just run uncoupledKinematicParcelFoam on your case and add the things OF asks for (most work will be about the specification of the lagrangian particles and that strongly depends on your case anyway - if unsure check the other lagrangian-tutorials)
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request |
||
January 18, 2013, 07:22 |
|
#10 |
New Member
Mattia
Join Date: Oct 2012
Location: Milan
Posts: 28
Rep Power: 13 |
What version of OpenFoam do you intend? I have to work on 1.7.
Thanks. Best regards. Mattia |
|
January 18, 2013, 17:18 |
|
#11 |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
Not sure where I have the case and therefor unsure for which version this is. Anyway. Just run the utility in your case and give it the stuff it asks for
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request |
|
January 19, 2013, 09:31 |
|
#12 |
New Member
Mattia
Join Date: Oct 2012
Location: Milan
Posts: 28
Rep Power: 13 |
Ok. Thanks. Last question. How can I see the parcel? I impose only one parcel in the CloudPosition file and I want to see this parcel. Thanks a lot.
Best regards. Mattia |
|
January 19, 2013, 18:49 |
|
#13 |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
Could you be a bit more specific about "see"? I assume you mean "postprocess in paraview". To my knowledge none of the two paraview-readers reads the CloudPosition-file. They only read (and display) the locations of particles that were written at later timesteps (you will have to select the particle "mesh" in the Reader-Panel, extract it with the ExtractParts-filter and visualize them with the Glyphs-filter)
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
help with wall functions | Nick Georgiadis | Main CFD Forum | 10 | January 17, 2017 10:03 |
Superlinear speedup in OpenFOAM 13 | msrinath80 | OpenFOAM Running, Solving & CFD | 18 | March 3, 2015 05:36 |
Wall functions | tutlhino | OpenFOAM Pre-Processing | 0 | July 2, 2007 05:04 |
Wall function in adverse pressure gradients | stephane baralon | Main CFD Forum | 11 | September 2, 1999 04:05 |
Wall functions | Abhijit Tilak | Main CFD Forum | 6 | February 5, 1999 01:16 |