CFD Online Discussion Forums

CFD Online Discussion Forums (
-   OpenFOAM Post-Processing (
-   -   Something about log file (

giovanni September 13, 2007 06:37

Hi all, I have some questio
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!


msrinath80 September 13, 2007 13:11

Transcript from previous discu
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?


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.


giovanni September 13, 2007 14:01

Thank you Srinath! Giovan
Thank you Srinath!


mattijs September 13, 2007 15:22

The foamLog script filters the
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.

giovanni September 14, 2007 02:50

Thanks a lot Mattijs for your
Thanks a lot Mattijs for your perfect clarification!
I'll see foamLog.db to know better foamLog's behaviour.



tsencic September 28, 2007 08:53

I want to write some global re
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?

hjasak September 28, 2007 09:10

Easy: << sum(Y*mesh.V())/su

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



chris_sev March 25, 2009 10:46


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_sev March 25, 2009 15:10

Ok,I have sorted this by modifying foamLog.db

All times are GMT -4. The time now is 07:08.