|
[Sponsors] |
September 13, 2007, 06:37 |
Hi all,
I have some questio
|
#1 |
New Member
Giovanni Boldrini
Join Date: Mar 2009
Location: Bologna, Italy
Posts: 10
Rep Power: 17 |
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 |
|
September 13, 2007, 13:11 |
Transcript from previous discu
|
#2 |
Senior Member
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 703
Rep Power: 21 |
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 |
|
September 13, 2007, 14:01 |
Thank you Srinath!
Giovan
|
#3 |
New Member
Giovanni Boldrini
Join Date: Mar 2009
Location: Bologna, Italy
Posts: 10
Rep Power: 17 |
Thank you Srinath!
Giovanni |
|
September 13, 2007, 15:22 |
The foamLog script filters the
|
#4 |
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
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. |
|
September 14, 2007, 02:50 |
Thanks a lot Mattijs for your
|
#5 |
New Member
Giovanni Boldrini
Join Date: Mar 2009
Location: Bologna, Italy
Posts: 10
Rep Power: 17 |
Thanks a lot Mattijs for your perfect clarification!
I'll see foamLog.db to know better foamLog's behaviour. Regards Giovanni |
|
September 28, 2007, 08:53 |
I want to write some global re
|
#6 |
Member
Tomislav Sencic
Join Date: Mar 2009
Posts: 42
Rep Power: 17 |
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? |
|
September 28, 2007, 09:10 |
Easy:
<< sum(Y*mesh.V())/su
|
#7 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,905
Rep Power: 33 |
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 |
|
March 25, 2009, 09:46 |
|
#8 |
New Member
Chris
Join Date: Mar 2009
Location: Europe
Posts: 19
Rep Power: 17 |
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 |
|
March 25, 2009, 14:10 |
|
#9 |
New Member
Chris
Join Date: Mar 2009
Location: Europe
Posts: 19
Rep Power: 17 |
Ok,I have sorted this by modifying foamLog.db
|
|
|
|
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 |
[OpenFOAM] ParaView exiting while trying to save image file or movie file | 21kalee | ParaView | 3 | January 23, 2008 16:01 |
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 04:53 |