# Particle-class uses wallImpactDistance on non-wall patches

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

 August 19, 2010, 07:54 Particle-class uses wallImpactDistance on non-wall patches #1 Assistant Moderator   Bernhard Gschaider Join Date: Mar 2009 Posts: 4,008 Rep Power: 43 Sponsored Links 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 randolph likes this.

 August 20, 2010, 05:17 #2 New Member   Andrew Heather Join Date: Mar 2009 Posts: 16 Rep Power: 10 Thanks for the report - I've pushed the fix from our internal line Andy

March 21, 2011, 05:38
#3
Senior Member

xinguang cui
Join Date: Mar 2009
Posts: 116
Rep Power: 10
Thanks for this kind of information. In fact, I has also met this problem. If it is possible. Would you please give some hint on how to solve the problem. I will be really grateful for it.

Quote:
 Originally Posted by heather Thanks for the report - I've pushed the fix from our internal line Andy

 March 25, 2011, 06:37 #4 Super Moderator   Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 9,978 Blog Entries: 39 Rep Power: 108 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 __________________ OpenFOAM: FAQ | Getting started Forum: How to get help, to post code/output and forum guide What am I doing/planning: blog/wiki Read this before sending me PM

March 25, 2011, 08:30
#5
Senior Member

xinguang cui
Join Date: Mar 2009
Posts: 116
Rep Power: 10
Dear Wyldkat:

Thanks so much for the information

Quote:
 Originally Posted by heather Thanks for the report - I've pushed the fix from our internal line Andy
Quote:
 Originally Posted by wyldckat 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

June 5, 2011, 12:20
Hi Bernhard,
#6
Member

edison
Join Date: May 2009
Location: Australia
Posts: 35
Rep Power: 10
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:
 Originally Posted by gschaider 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: Attachment 4452 (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: Attachment 4453 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): Attachment 4451 (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

June 7, 2011, 07:07
#7
Assistant Moderator

Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,008
Rep Power: 43
Quote:
 Originally Posted by Edison_Ge 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?
No. But I havn't worked with 1.7.1 and lagrangian in the last time. Have you tried 1.7.x?

 January 18, 2013, 04:47 Tutorial for uncoupledKinematicParcelFoam #8 New Member   Mattia Join Date: Oct 2012 Location: Milan Posts: 28 Rep Power: 6 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, 08:20
#9
Assistant Moderator

Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,008
Rep Power: 43
Quote:
 Originally Posted by gara1988 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.
Can't give you the geometry. Sorry. Also that was with a quite old version of OF so it won't be much help.

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, 08:22 #10 New Member   Mattia Join Date: Oct 2012 Location: Milan Posts: 28 Rep Power: 6 What version of OpenFoam do you intend? I have to work on 1.7. Thanks. Best regards. Mattia

January 18, 2013, 18:18
#11
Assistant Moderator

Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,008
Rep Power: 43
Quote:
 Originally Posted by gara1988 What version of OpenFoam do you intend? I have to work on 1.7.
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, 10:31 #12 New Member   Mattia Join Date: Oct 2012 Location: Milan Posts: 28 Rep Power: 6 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, 19:49
#13
Assistant Moderator

Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,008
Rep Power: 43
Quote:
 Originally Posted by gara1988 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.
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

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Nick Georgiadis Main CFD Forum 10 January 17, 2017 11:03 msrinath80 OpenFOAM Running, Solving & CFD 18 March 3, 2015 06:36 tutlhino OpenFOAM Pre-Processing 0 July 2, 2007 05:04 stephane baralon Main CFD Forum 11 September 2, 1999 04:05 Abhijit Tilak Main CFD Forum 6 February 5, 1999 02:16

All times are GMT -4. The time now is 22:17.