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

Something about log file

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 13, 2007, 06:37
Default Hi all, I have some questio
  #1
New Member
 
Giovanni Boldrini
Join Date: Mar 2009
Location: Bologna, Italy
Posts: 10
Rep Power: 8
giovanni is on a distinguished road
Hi all,

I have some questions about the files generated by foamLog. In a rhoTurbFoam case I generated "logs" directory, there I can find some unknown files. So,

1) What's the difference between a name_0 file to a name_1 file?

2) Why there are 3 rho files? (rho_0, rho_1, rho_2)

3) What's the difference between contCumulative, contGlobal and contLocal?


Thanks a lot!

Giovanni
giovanni is offline   Reply With Quote

Old   September 13, 2007, 13:11
Default Transcript from previous discu
  #2
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12
msrinath80 is on a distinguished road
Transcript from previous discussions:

By Eugene de Villiers on Thursday, May 26, 2005 - 03:06 am: Edit Post

U_0 and the other *_0 fields are the old time values (i.e. timestep previous to U). They are necessary to restart calculations that use second order accurate schemes in time like Crank-Nicholson.

-----------------------------------------

By Anja Stretz on Wednesday, January 18, 2006 - 07:36 am: Edit Post

For example:
time step continuity errors :
sum local = 1.05535e-08, global = 1.65393e-14, cumulative = -9.944e-11

What exactly do you mean by converging the pressure more tightly?

Anja

By Hrvoje Jasak on Wednesday, January 18, 2006 - 07:41 am: Edit Post

This does not worry me at all: it says your global continuity error is 1e-14, which is the double precision round-off error, the sum local tells me that in the line above your pressure solver has converged to about 1e-8; in other words, all is well.

Nothing to worry about here.

Hrv
msrinath80 is offline   Reply With Quote

Old   September 13, 2007, 14:01
Default Thank you Srinath! Giovan
  #3
New Member
 
Giovanni Boldrini
Join Date: Mar 2009
Location: Bologna, Italy
Posts: 10
Rep Power: 8
giovanni is on a distinguished road
Thank you Srinath!


Giovanni
giovanni is offline   Reply With Quote

Old   September 13, 2007, 15:22
Default The foamLog script filters the
  #4
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
The foamLog script filters the provided log file. It just scans for certain patterns and the first occurrence for that becomes '_0', the second '_1' etc. so if your solver solves multiple times for e.g. p in one timestep they are kept separate.

The patterns it uses are defined in the foamLog.db file in the same directory as the foamLog script. If it is missing some feel free to extend it for other solvers/linear solvers and send me a copy.
mattijs is offline   Reply With Quote

Old   September 14, 2007, 02:50
Default Thanks a lot Mattijs for your
  #5
New Member
 
Giovanni Boldrini
Join Date: Mar 2009
Location: Bologna, Italy
Posts: 10
Rep Power: 8
giovanni is on a distinguished road
Thanks a lot Mattijs for your perfect clarification!
I'll see foamLog.db to know better foamLog's behaviour.

Regards

Giovanni
giovanni is offline   Reply With Quote

Old   September 28, 2007, 08:53
Default I want to write some global re
  #6
Member
 
Tomislav Sencic
Join Date: Mar 2009
Posts: 42
Rep Power: 8
tsencic is on a distinguished road
I want to write some global results in the logSummary file. For example for O2 concentration I write in the code:

<< sum(Y[1]*mesh.V())/sum(mesh.V()) << tab

and I obtain as output

(sum((O2*V))|sum(V)) [0 0 0 0 0 0 0] 0.233233
for each timestep.

How could I get just the value, just 0.233233?
tsencic is offline   Reply With Quote

Old   September 28, 2007, 09:10
Default Easy: << sum(Y*mesh.V())/su
  #7
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Easy:

<< sum(Y[1]*mesh.V())/sum(mesh.V()).value() << tab

Enjoy,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   March 25, 2009, 10:46
Default
  #8
New Member
 
Chris
Join Date: Mar 2009
Location: Europe
Posts: 19
Rep Power: 8
chris_sev is on a distinguished road
Hi,

Sorry for digging but I have some question regarding to foamLog.

I have written new variable to logSummary. Once the job is finished and I type foamLog, log directory is created but my new variable is not present there.

Should I modify somehow foamLog code to make it possible?

I am using OF 1.5

thanks for reply!

chris
chris_sev is offline   Reply With Quote

Old   March 25, 2009, 15:10
Default
  #9
New Member
 
Chris
Join Date: Mar 2009
Location: Europe
Posts: 19
Rep Power: 8
chris_sev is on a distinguished road
Ok,I have sorted this by modifying foamLog.db
chris_sev is offline   Reply With Quote

Reply

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
PLOT3D ASCII solution file to MATLAB data file Sandeep Rana Main CFD Forum 4 June 11, 2010 09:48
ParaView exiting while trying to save image file or movie file 21kalee OpenFOAM Paraview & paraFoam 3 January 23, 2008 17:01
Changing gambit file without change of case file?? Asghari FLUENT 2 August 28, 2006 13:48
Covert gambit file to polyflow file John FLUENT 5 August 6, 2004 08:31
Converting a surface file to a volume file Amir FLUENT 2 December 30, 2002 05:53


All times are GMT -4. The time now is 04:13.