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!

Giovanni

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?

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

Thank you Srinath! Giovan
 

Thank you Srinath!


Giovanni

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.

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.

Regards

Giovanni

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?

Easy: << sum(Y*mesh.V())/su
 

Easy:

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

Enjoy,

Hrv

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

Ok,I have sorted this by modifying foamLog.db