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

No times selected after successful parallel run

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 13, 2012, 15:34
Default No times selected after successful parallel run
  #1
New Member
 
Edwin Lee
Join Date: Jan 2012
Posts: 3
Rep Power: 5
Myoldmopar is on a distinguished road
Greetings,

I have spent some time familiarizing myself with OpenFoam after spending a good amount of time with Fluent. I was able to decompose a domain for 32 processors and successfully load up all 8 "processors" on my local machine, plus 8 on each of 3 more machines connected via ethernet.

Everything looked great, no errors during simulation. After it completed, I tried to reconstructPar, only to be given this:

--> FOAM FATAL ERROR:
No times selected

From function reconstructPar
in file reconstructPar.C at line 139.

FOAM exiting

I have searched around, but most of the problems are actually getting the parallel runs working, and I couldn't find a solution to this.

Any insights?

Thanks!
Myoldmopar is offline   Reply With Quote

Old   January 14, 2012, 05:10
Default
  #2
Senior Member
 
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 790
Rep Power: 12
Bernhard is on a distinguished road
Hi Edwin,

You have to specify which time-steps you want to reconstruct. You can either use -latestTime or specify -time as defined here: http://www.openfoamwiki.net/index.ph...ection_Options
Bernhard is offline   Reply With Quote

Old   January 16, 2012, 12:26
Default
  #3
New Member
 
Edwin Lee
Join Date: Jan 2012
Posts: 3
Rep Power: 5
Myoldmopar is on a distinguished road
Thanks for that!

So I think there is still a problem. As I mentioned, I am on one computer, lets say "A", and I have three slave machines "B-D." The simulations are run on all 8 cores of each of the four machines.

When I look at the output data from the runs, I notice each machine only has a fourth of the final output data, which is essentially what I expect:
If I log into "B", and look through the directories, I notice that processor0 folder has all the time step data output folders. processor1 only has 0 and constant subdirectories, same with processor2 and 3 folders. Then processor4 folder has all the data in it again. This is mimicked across all four machines. Each one, including the master "A," only has its own data.
What I expected was that each machine would transfer its output back to the master machine. However, I believe I am approaching that a bit wrong. When I manually merge the folders back onto the master, and do a reconstructPar, it reconstructs it pretty well, except for a different problem which I'll post about separately.

So, do I need to setup an NFS share? I hadn't done it simply because I thought everything could be communicated well enough over ssh. I am not against setting one up, just didn't want to waste any time.

Thanks so much!
Myoldmopar is offline   Reply With Quote

Old   January 25, 2012, 09:45
Default
  #4
Member
 
Vitor Vasconcelos
Join Date: Jan 2012
Posts: 33
Rep Power: 5
vitors is on a distinguished road
Quote:
Originally Posted by Myoldmopar View Post
Thanks for that!

So I think there is still a problem. As I mentioned, I am on one computer, lets say "A", and I have three slave machines "B-D." The simulations are run on all 8 cores of each of the four machines.

When I look at the output data from the runs, I notice each machine only has a fourth of the final output data, which is essentially what I expect:
If I log into "B", and look through the directories, I notice that processor0 folder has all the time step data output folders. processor1 only has 0 and constant subdirectories, same with processor2 and 3 folders. Then processor4 folder has all the data in it again. This is mimicked across all four machines. Each one, including the master "A," only has its own data.
What I expected was that each machine would transfer its output back to the master machine. However, I believe I am approaching that a bit wrong. When I manually merge the folders back onto the master, and do a reconstructPar, it reconstructs it pretty well, except for a different problem which I'll post about separately.

So, do I need to setup an NFS share? I hadn't done it simply because I thought everything could be communicated well enough over ssh. I am not against setting one up, just didn't want to waste any time.

Thanks so much!
I'm experiencing exactly the same problem... Waiting for replies.

Vitor
vitors is offline   Reply With Quote

Old   January 25, 2012, 11:31
Default
  #5
Senior Member
 
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 237
Rep Power: 9
olivierG is on a distinguished road
hello,

The simples way is to setup a nfs (or sshfs) file system.

But you can go without. You should setup in your decomposeParDict:
distributed yes;
roots
4 <- nbr of node)
(
/path/for/machine1/case
/path/for/machine2/case
...
)
In this case, the data is local to the machine, so less I/O through the network.

NB: in fact, if you use Paraview for post processing, you can load all the data from each node without recontructing, and post process all .

regards,
olivier
olivierG is offline   Reply With Quote

Reply

Tags
no times selected, parallel computation, reconstructpar

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
Script to Run Parallel Jobs in Rocks Cluster asaha OpenFOAM Running, Solving & CFD 12 July 4, 2012 22:51
Parallel run in fluent for multiphase flow apurv FLUENT 2 August 3, 2011 19:44
Change parameter and run cases parallel lingdeer ANSYS 0 July 29, 2011 10:27
Unable to run OF in parallel on a multiple-node cluster quartzian OpenFOAM 3 November 24, 2009 14:37
How to run parallel in ICEM_CFD? Kiddo Main CFD Forum 2 January 24, 2005 09:53


All times are GMT -4. The time now is 07:54.