CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

How to speed up reconstructPar ?

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

Like Tree2Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   July 12, 2010, 05:47
Question How to speed up reconstructPar ?
  #1
New Member
 
Join Date: Jun 2010
Posts: 23
Rep Power: 7
NorbertB is on a distinguished road
Hi Foamers !

I run a LES case with 32 processors, no problem (at present ^^), it took only 5hours, but the reconstruction is incredibly slow : around 80hours !

I only use 1 processor for the reconstruction (it seems logical for me), and anyway there is no -parallel option for reconstructPar.

Does anyone know how to increase the speed of that reconstruction ?
It is quite annoying to be able to run a super fast LES whereas you need 20 more times to reconstruct the case ^^

Thanks
NorbertB is offline   Reply With Quote

Old   July 12, 2010, 06:29
Default
  #2
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,511
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings NorbertB,

How long did it take to run decomposePar? And is there any particular reason why you need to reconstruct the case?

Is it just because you need to post-process? If so, then try using ParaView 3.8 and open the case with a file "case.foam" instead of "case.OpenFOAM"! And if it works well, and you want to use paraFoam to start using 3.8.0, then follow these instructions (2nd part of the post): OpenFOAM 1.7 ParaView 3.8 installation problems

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   July 12, 2010, 06:44
Default
  #3
New Member
 
Join Date: Jun 2010
Posts: 23
Rep Power: 7
NorbertB is on a distinguished road
Hi Bruno,

Indeed I need to post-process and thus to reconstruct the case.
It took about 20min to run decomposePar, that is quite reasonable.

If I try to use ParaView before reconstructing the fields, it will show me only one processor result or the full field result ?
I am confused : you say I don't need to reconstruct the case to post-process it ?

Best regards,

Norbert
NorbertB is offline   Reply With Quote

Old   July 12, 2010, 07:02
Default
  #4
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,511
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
20min to 80 hours... wait, did you reconstruct all of the time snapshots? Because in theory, it should take something like "20min * ratio of total number of fields by number of initial fields * the number of time snapshots" to reconstruct!
You can try running:
Code:
reconstructPar -latestTime
This way you'll only reconstruct the latest time snapshot!

Ah and here you go, attached is the proof that you can process a decomposed case with ParaView 3.8.0 As long as you open with case.foam and not case.OpenFOAM, it will work
It's the motorBike tutorial case, which I ran with 2 processors, all in Windows!

Best regards,
Bruno
Attached Images
File Type: jpg motobike_decomposed.jpg (49.5 KB, 164 views)
wyldckat is offline   Reply With Quote

Old   July 12, 2010, 07:48
Default
  #5
New Member
 
Join Date: Jun 2010
Posts: 23
Rep Power: 7
NorbertB is on a distinguished road
Ahaha, indeed I reconstructed all snapshots but ideally I would like to see the transition state and not only the final state
But I think I don't have the choice

Thank you for your time and your final proof ! I don't have root access on my computer so at present I can't use 3.8 version (using 3.6 version), but it seems very useful.

Thanks again !
NorbertB is offline   Reply With Quote

Old   July 12, 2010, 07:50
Default
  #6
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,511
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Root access? Just download the pre-built versions from www.paraview.org and unpack in your home/user folder and use it That's why I gave you the link to the other post!
wyldckat is offline   Reply With Quote

Old   October 21, 2010, 10:29
Default
  #7
Member
 
Vishal Jambhekar
Join Date: Mar 2009
Location: University Stuttgart, Stuttgart Germany
Posts: 90
Blog Entries: 1
Rep Power: 8
vishal is on a distinguished road
Hi ,

I am using OF-1.7.1 and i made the change in parafoam file as u mentioned before but i am still not getting .foam file in case dir. however it used to be generate in .OpenFOAM for openfoam 1.6.0

can you please tell me how to generate .foam file
__________________
Cheers,

Vishal Jambhekar...
"Simulate the way ahead......!!!"
vishal is offline   Reply With Quote

Old   October 21, 2010, 13:49
Default
  #8
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,511
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings Vishal,

There is more than one ".OpenFOAM" in the paraFoam script You'll have to change them all!

edit: Then use:
Code:
paraFoam -touch
to generate the ".foam" file, but only if you intend to open it from another ParaView, instead of using paraFoam to open it directly in ParaView.

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   October 22, 2010, 02:44
Default
  #9
Member
 
Join Date: Nov 2009
Location: Germany
Posts: 96
Rep Power: 7
val46 is on a distinguished road
Aaahhh... and I always thought for post-proc you have to reconstruct the case.
Thanks, Bruno!

I just saw you posted a picture of the motorbike tutorial. I know its not the topic of this thread but I would like to ask if you run this case with OF 1.7.x
Because I have convergence problems when I run this tutorial as it is.

Regards,
Toni
val46 is offline   Reply With Quote

Old   October 22, 2010, 08:35
Default
  #10
Member
 
Vishal Jambhekar
Join Date: Mar 2009
Location: University Stuttgart, Stuttgart Germany
Posts: 90
Blog Entries: 1
Rep Power: 8
vishal is on a distinguished road
Hi,

Thanks Bruon.....!!! actually i converted them all :P and its working for me. But ur comment is always usefull. so now there in no more need to change format to VTK.

just use touch and its ready for paraview. yes i am using compiled version of paraview i got with OF- 1.7.1.

no parafoam for me....

does anyone know how to install qmake for CENTOS........???
__________________
Cheers,

Vishal Jambhekar...
"Simulate the way ahead......!!!"
vishal is offline   Reply With Quote

Old   October 22, 2010, 08:59
Default
  #11
Member
 
Join Date: Nov 2009
Location: Germany
Posts: 96
Rep Power: 7
val46 is on a distinguished road
hm... when I use
Code:
paraFoam - touch
I get a .OpenFOAM file.

How do I get a .foam file?
val46 is offline   Reply With Quote

Old   October 22, 2010, 11:11
Default
  #12
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,511
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi val46,

Quote:
Originally Posted by http://www.cfd-online.com/Forums/blogs/wyldckat/317-using-official-pre-built-paraview-3-8-0-version-openfoam.html
open the file "$WM_PROJECT_DIR/bin/paraFoam" in your favorite simple text editor and replace every entry ".OpenFOAM" with ".foam". Now save and close the file.
edit: wow, I didn't see that there were so many posts... OK:
  • Toni: the motorBike case converged for me with OpenFOAM 1.6.x. I haven't tried running the 1.7.x yet, so I don't know if it will converge or not
  • Vishal: OpenFOAM-1.7.0 for CentOS/RHEL/SL 5.x 64bit released - You can snatch the Third Party applications already built for CentOS from that tutorial/script

Best regards,
Bruno

Last edited by wyldckat; October 22, 2010 at 11:17. Reason: didn't see the other posts, so now updating to reply...
wyldckat is offline   Reply With Quote

Old   October 25, 2010, 05:12
Default
  #13
Member
 
Vishal Jambhekar
Join Date: Mar 2009
Location: University Stuttgart, Stuttgart Germany
Posts: 90
Blog Entries: 1
Rep Power: 8
vishal is on a distinguished road
Thanks Bruno....it was helpful....!!!
__________________
Cheers,

Vishal Jambhekar...
"Simulate the way ahead......!!!"
vishal is offline   Reply With Quote

Old   October 26, 2010, 11:16
Default
  #14
Senior Member
 
Arne Stahlmann
Join Date: Nov 2009
Location: Hanover, Germany
Posts: 209
Rep Power: 8
Arnoldinho is on a distinguished road
Hi all,

I found your post and find it very useful, as I have also always reconstructed the case for post processing before.

Following the simple instructions, I changed every .OpenFOAM entry to .foam in the paraFoam file. Nevertheless, when I type 'paraFoam' in the case folder (with folders 0, constant, system, processor0 - 15), ParaView displays only the initial state, i.e. the '0' folder. A 'paraFoam -touch' creates an empty case.foam file.

I use OpenFOAM 1.7.1 and ParaView 3.8.0 (from the openfoam website).
Arnoldinho is offline   Reply With Quote

Old   October 26, 2010, 14:07
Default
  #15
Member
 
Vishal Jambhekar
Join Date: Mar 2009
Location: University Stuttgart, Stuttgart Germany
Posts: 90
Blog Entries: 1
Rep Power: 8
vishal is on a distinguished road
Hi,

Exactly you have to create .foam file open it in paraview and the you can post process it as you want. I am using same version as you and its working fine.
__________________
Cheers,

Vishal Jambhekar...
"Simulate the way ahead......!!!"
vishal is offline   Reply With Quote

Old   October 26, 2010, 16:29
Default
  #16
Senior Member
 
Arne Stahlmann
Join Date: Nov 2009
Location: Hanover, Germany
Posts: 209
Rep Power: 8
Arnoldinho is on a distinguished road
Ok, but again: An empty .foam file is created. When opening the case in Paraview (either per paraFoam or directly within a new instance of ParaView), only the first time step is diplayed, and not the ones that are stored in the processor-subfolders .
Arnoldinho is offline   Reply With Quote

Old   October 26, 2010, 18:17
Default
  #17
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,511
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings Arne,
Quote:
Originally Posted by Arnoldinho View Post
Ok, but again: An empty .foam file is created. When opening the case in Paraview (either per paraFoam or directly within a new instance of ParaView), only the first time step is diplayed, and not the ones that are stored in the processor-subfolders .
Since a picture is worth a thousand or so words, here is one attached.
Notice the area where the mouse pointer is and the red line it points to? There you can change from "reconstructed" to "decomposed". Then don't forget to press the "Apply" button!

Best regards,
Bruno
Attached Images
File Type: jpg ParaView.foam.jpg (47.5 KB, 78 views)
iamed18 and Kopy like this.
wyldckat is offline   Reply With Quote

Old   October 27, 2010, 01:55
Default
  #18
Senior Member
 
Arne Stahlmann
Join Date: Nov 2009
Location: Hanover, Germany
Posts: 209
Rep Power: 8
Arnoldinho is on a distinguished road
Thanks Bruno,

that looks nice. It works! I always looked for the error at the side of OpenFoam, not within Paraview itself. Maybe I should have a closer look at the manual...

Regards, Arne
Arnoldinho is offline   Reply With Quote

Old   October 27, 2010, 10:27
Default
  #19
Member
 
Join Date: Nov 2009
Location: Germany
Posts: 96
Rep Power: 7
val46 is on a distinguished road
Hi Bruno,

again off-topic:
I tried the motorbike tutorial with 1.6.x and got no nice convergence (see attached picture).
Have you started it out of the box?

Regards,
Toni
Attached Images
File Type: jpeg screenshot_convergence.jpeg (52.0 KB, 43 views)
val46 is offline   Reply With Quote

Old   October 27, 2010, 20:03
Default
  #20
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,511
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Toni,

I've never worried too much about the motorBike case fully converging. I just didn't want it to diverge, which happened with the 1.6 version.

Attached is the log.simpleFoam for a run with 1.7.1, both case and applications. I didn't have my cheat-sheet with me for plotting the residuals, so the log will have to do

So, by what I can see:
  1. The default number of iterations should still be 500, although I haven't check the latest git version to confirm.
  2. These logged residuals seem to be similar to the ones from your plot.
  3. The case could use some 100 or 200 more iterations, for it to fully converge, but I believe that these results should already be good. But I'm not a CFD specialist, so it's only a hunch
  4. I think this case serves only as a tutorial... I don't think that it's a 100% perfected case yet, since the STL has some holes in its surface... which allows for air to go through some strange places into the hollowed bike... at least last time I inspected it, about 10 months ago
Best regards,
Bruno
Attached Files
File Type: gz log.simpleFoam.tar.gz (44.1 KB, 2 views)
wyldckat is offline   Reply With Quote

Reply

Tags
les, reconstructpar, slow, speed up

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Train Speed yeo FLUENT 5 February 14, 2012 09:38
Can OpenFOAM generate flow at the speed of light? Michel_sharp OpenFOAM 6 October 24, 2009 04:09
Problem with reconstructPar fabianpk OpenFOAM 5 August 14, 2007 09:17
low speed compressible flow lily CFX 2 November 16, 2005 06:15
rotation speed in the domain jiaye gan CFX 3 April 5, 2004 08:50


All times are GMT -4. The time now is 09:01.