[Zappstar]

Hello

I use Code-Saturn. My log file, generated by Code-Saturn named "listing" does not seem to work with the script above. Does anyone know the reason for that? what differs?

Regards

[pingat]

hey,

of course it doesn't work with you file. the script searches for special parts in your log file.

could you show some parts of your log file?

[AlexaB]

Hi all!!

I'm running a simulation with nonNewtonianIcoFoam. My PISO loop is defined like this:

PISO
{
nCorrectors 4;
nNonOrthogonalCorrectors 0;
}

My problem is that I cannot plot pressure residuals. I tried to adapt the code to my residuals but it doesn't work.

Can you help me on how to adapt the code, in a way I can plot my pressure residuals?

Time = 0.0358

Courant Number mean: 0.305335 max: 2.99566
smoothSolver: Solving for Ux, Initial residual = 4.04223e-06, Final residual = 4.04223e-06, No Iterations 0
smoothSolver: Solving for Uy, Initial residual = 9.82472e-06, Final residual = 9.82472e-06, No Iterations 0
GAMG: Solving for p, Initial residual = 5.01451e-06, Final residual = 3.82254e-07, No Iterations 7
time step continuity errors : sum local = 4.72856e-10, global = 2.16719e-11, cumulative = 1.06737e-05
GAMG: Solving for p, Initial residual = 3.43557e-06, Final residual = 3.16488e-07, No Iterations 7
time step continuity errors : sum local = 3.91497e-10, global = -9.67931e-12, cumulative = 1.06736e-05
GAMG: Solving for p, Initial residual = 1.56104e-06, Final residual = 1.00064e-07, No Iterations 11
time step continuity errors : sum local = 1.23779e-10, global = -1.61043e-12, cumulative = 1.06736e-05
GAMG: Solving for p, Initial residual = 5.78378e-07, Final residual = 3.118e-08, No Iterations 10
time step continuity errors : sum local = 3.857e-11, global = -1.46006e-12, cumulative = 1.06736e-05
ExecutionTime = 434.79 s ClockTime = 436 s

What value of the previous pressure residuals is the most correct to plot?

Thank you very much for your attention!

[pingat]

hey,

have you read the whole thread? whats your error message?

i think you cut out the wrong parts. as the script cuts out the 9. word position in each line and your residuals are standing at 8. position.

[AlexaB]

Hi pingat, thank you for your answer!!

Yes, I read the thread... I can get my Ux and Uy residuals, but not the pressure...

My error message is:

"Residuals", line 232: warning: Skipping data file with no valid points
sh: 1: Syntax error: Unterminated quoted string

plot "< cat itert | grep 'Solving for Ux' | cut -d' ' -f9" title 'Ux' with lines,"< cat itert | grep 'Solving for Uy' | cut -d' ' -f9" title 'Uy' with lines,"< cat itert | grep 'Solving for p' | cut -d' ' -f9 | sed -n 'p;N;N;N' | 'tr -d ','" title 'p' with lines

If I change -f9 to -f8, as you suggested, it doesn't appear nothing...

[sina_mech]

I'm using "nNonOrthogonalCorrectors = 2", so I get more than 1 pressure log each time step. How can I plot only the last pressure solution residual? Because the pressure iterations go faster. (please see the attached)

[gschaider]

Originally Posted by sina_mech

I'm using "nNonOrthogonalCorrectors = 2", so I get more than 1 pressure log each time step. How can I plot only the last pressure solution residual? Because the pressure iterations go faster. (please see the attached)

Well. I guess another command in the pipeline won't make much difference. Try one of the recipes here http://stackoverflow.com/questions/9...in-a-text-file

[Zappstar]

Hi! I cant sort this out.. =( can someone give me an example of how to setup the textfile to work with my log file?

set logscale y
set title "Residuals"
set ylabel 'Residual'
set xlabel 'Iteration'
plot "< cat log | grep 'Solving for Ux' | cut -d' ' -f9 | tr -d ','" title 'Ux' with lines,\
"< cat log | grep 'Solving for Uy' | cut -d' ' -f9 | tr -d ','" title 'Uy' with lines,\
"< cat log | grep 'Solving for Uz' | cut -d' ' -f9 | tr -d ','" title 'Uz' with lines,\
"< cat log | grep 'Solving for omega' | cut -d' ' -f9 | tr -d ','" title 'omega' with lines,\
"< cat log | grep 'Solving for k' | cut -d' ' -f9 | tr -d ','" title 'k' with lines,\
"< cat log | grep 'Solving for p' | cut -d' ' -f9 | tr -d ','" title 'p' with lines
pause 1
reread

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.3.x |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.3.x-42314c41c511
Exec : simpleFoam -parallel
Date : Nov 19 2014
Time : 13:16:02
Host : "peter-Sigma"
PID : 31421
Case : /home/peter/OpenFOAM/peter-2.3.x/run/Skyware
nProcs : 6
Slaves :
5
(
"peter-Sigma.31422"
"peter-Sigma.31423"
"peter-Sigma.31424"
"peter-Sigma.31425"
"peter-Sigma.31426"
)

Pstream initialized with:
floatTransfer : 0
nProcsSimpleSum : 0
commsType : nonBlocking
polling iterations : 0
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0.54

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting RAS turbulence model kOmegaSST
kOmegaSSTCoeffs
{
alphaK1 0.85;
alphaK2 1;
alphaOmega1 0.5;
alphaOmega2 0.856;
gamma1 0.555556;
gamma2 0.44;
beta1 0.075;
beta2 0.0828;
betaStar 0.09;
a1 0.31;
b1 1;
c1 10;
F3 false;
}

No finite volume options present


SIMPLE: convergence criteria
field p tolerance 1e-07
field U tolerance 1e-08
field "(k|epsilon|omega)" tolerance 0.0001


Starting time loop

forceCoeffs forceCoeffs1:
Not including porosity effects

Time = 0.541

smoothSolver: Solving for Ux, Initial residual = 0.000804916, Final residual = 5.49369e-07, No Iterations 11
smoothSolver: Solving for Uy, Initial residual = 2.29261e-05, Final residual = 8.56105e-07, No Iterations 5
smoothSolver: Solving for Uz, Initial residual = 0.000867147, Final residual = 5.90003e-07, No Iterations 11
GAMG: Solving for p, Initial residual = 0.00203898, Final residual = 6.64107e-07, No Iterations 9
GAMG: Solving for p, Initial residual = 0.000470797, Final residual = 8.8148e-07, No Iterations 4
GAMG: Solving for p, Initial residual = 5.863e-05, Final residual = 9.59074e-07, No Iterations 2
time step continuity errors : sum local = 3.54146e-10, global = -9.50863e-12, cumulative = -9.50863e-12
smoothSolver: Solving for omega, Initial residual = 5.37503e-05, Final residual = 9.52376e-07, No Iterations 6
smoothSolver: Solving for k, Initial residual = 0.000221609, Final residual = 5.34179e-07, No Iterations 9
ExecutionTime = 14.92 s ClockTime = 15 s

forceCoeffs forceCoeffs1 output:
Cm = -0.267356
Cd = 0.37438
Cl = 0.00166993
Cl(f) = -0.266521
Cl(r) = 0.268191

Time = 0.542

smoothSolver: Solving for Ux, Initial residual = 0.000801499, Final residual = 5.4714e-07, No Iterations 11
smoothSolver: Solving for Uy, Initial residual = 2.27642e-05, Final residual = 8.50023e-07, No Iterations 5
smoothSolver: Solving for Uz, Initial residual = 0.000862468, Final residual = 5.87098e-07, No Iterations 11

[odin]

Hello Zappstar
the command you use reads:
'cat log | grep 'Solving for Ux' | cut -d' ' -f9 | tr -d ','" title 'Ux' with lines,\...'

cat log - gives your complete log-file

grep 'Solving for Ux' - is searching for lines that include 'Solving for Ux'

cut -d' ' -f9 - cuts out the 9th field in each line using the delimiter ' '


that should be the string 'Final' in your example:
1 ___________2 _____3 _4 __5 ___6 _____7 8 ___________9 __10 ____11 12 ________13 14 ______15
smoothSolver: Solving for Ux, Initial residual = 0.000801499, Final residual = 5.4714e-07, No Iterations 11


try -f8 or -f12 instead of the option -f9


btw: tr -d ',' - deletes the comma ('0.000804916,' --> '0.000804916')

you can try this step by step by typing the commands into a terminal like:
cat log - (see what happens...)
cat log | grep 'Solving for Uz' - (see what happens...)
and so on...

good luck

[odin]

Hello sina_mech
You can use the command 'sed'. Depending on how many NonOrthogonalCorrectors you use sed -n '0~2p' and for 'the other one': sed -n '1~2p'
"< cat log.pisoFoam | grep 'Solving for p' | cut -d' ' -f9 | tr -d ',' | sed -n '0~4p'" title '0-p'
look for: 'delete pattern space. start next cycle.' in the manual

[Kozan]

Hi!

I would like to say Thank you... this script, tutorial and whole thread are very useful.
I've modified the script for my purpose. The residuals are ploted in three separated windows, which is a bit more clear (I thing).

The Courant number and deltaT are ploted in the fourth window.

set multiplot layout 2, 2 rowsfirst
set logscale y
set ylabel "Residuals"
set xlabel "Iteration"
plot "< cat log | grep 'Solving for Ux' | cut -d' ' -f9 | tr -d ','" title 'Ux' with lines,\
"< cat log | grep 'Solving for Uy' | cut -d' ' -f9 | tr -d ','" title 'Uy' with lines,\
"< cat log | grep 'Solving for Uz' | cut -d' ' -f9 | tr -d ','" title 'Uz' with lines
plot "< cat log | grep 'Solving for epsilon' | cut -d' ' -f9 | tr -d ','" title 'epsilon' with lines,\
"< cat log | grep 'Solving for k' | cut -d' ' -f9 | tr -d ','" title 'k' with lines
plot"< cat log | grep 'Solving for p' | cut -d' ' -f9 | sed -n 'p;N;N;N' | tr -d ','" title 'p' with lines,\
"< cat log | grep 'Solving for alphawater' | cut -d' ' -f9 | tr -d ','" title 'alphawater' with lines
plot"< cat log | grep 'deltaT' | cut -d' ' -f3 " title 'delta T' with lines,\
"< cat log | grep 'Courant Number' | cut -d' ' -f6 " title 'maxCo' with lines
unset multiplot
pause 1
reread

[JCD]

Hello and thanks for the script.
Does anyone have another for solids and/or FSI?

I have seen some forums directing towards pyFoam as a "plug in" for the processing of results. Is this the better solution?

Thanks

Jerry

[zandi]

Originally Posted by andersking

Another way to do this is to use pyFoam, http://openfoamwiki.net/index.php/Contrib_PyFoam, in particular

turbFoam > log &
pyFoamPlotWatcher.py log

this also plots a number of other things as well (and also provides a number of other useful utilities).

Cheers,
Andrew

Dear andersking

turbFoam > log &
pyFoamPlotWatcher.py log

doesn't work for me
could you help me please?

the ERROR is

>>> turbFoam > log &
  File "<stdin>", line 1
    turbFoam > log &
                   ^
SyntaxError: invalid syntax
>>> pyFoamPlotWatcher.py log
  File "<stdin>", line 1
    pyFoamPlotWatcher.py log
                           ^
SyntaxError: invalid syntax

[wyldckat]

Hi zandi,

The 3 "larger than" characters (>>>) mean that you're working inside the Python shell. Those commands you have tried to use are meant to be used from the bash/sh shell, not Python.

Therefore, you will need to run these commands:

quit()

turbFoam > log &
pyFoamPlotWatcher.py log

Which will look something like this on your screen:

>>> quit()

ofuser@machine:~$ turbFoam > log &
ofuser@machine:~$ pyFoamPlotWatcher.py log

Best regards,
Bruno

[saeedi]

Hi All,

I am very new to OpenFoam and have some very simple questions for you.

I usually use public domain computers to do my simulations (I submit the job and it stays in queue). In that case, the log file is not shown until the simulation is complete. Now I have the following questions for you:

1-How to record the residuals and CFL number in different columns separately in a file. In the log file, there are a lot of texts as well and practically I can not extract the CFL for example at each time step to plot them.

2-Is that possible that we can take a look at the log file before the simulation is over?

3-Also, since the simulations are 3D and needs very large space to store many snapshots, if I want to have 2D planes within the domain (for example I want to store the data at each 200 time steps just inside the plane z=0) or even a portion of that plane, can I do that?

Thanks in advance for your guidance

[zandi]

Originally Posted by saeedi

I usually use public domain computers to do my simulations (I submit the job and it stays in queue). In that case, the log file is not shown until the simulation is complete. Now I have the following questions for you:

1-How to record the residuals and CFL number in different columns separately in a file. In the log file, there are a lot of texts as well and practically I can not extract the CFL for example at each time step to plot them.

2-Is that possible that we can take a look at the log file before the simulation is over?

Hi I use CentOS cluster and with some commands I can get the log file and can take a look during the run.

the file for commands is like this

# script for paralle execution
#!/bin/bash
#PBS -S /bin/bash
#PBS -N OpenFoam
#PBS -l nodes=1:ppn=8
#PBS -q batch
#PBS -o $HOME/OF230/OF_Sample/$PBS_JOBID.OF.out
#PBS -e $HOME/OF230/OF_Sample/$PBS_JOBID.OF.err
#PBS -l walltime=12:00:00
NP=8
######## Running #######
export TOPDIR=$HOME/OF230/OF_Sample
export OFPATH=reactingFoam  {solver}
　
cd $TOPDIR
time mpirun -np $NP $OFPATH -parallel > $TOPDIR/$PBS_JOBID.out.log {log file}

then with foamLog and gnuplot I can plot the residuals but just for solvers interFoam and multiphaseInterFoam and not for twoPhaseEulerFoam. and sometimes also even I can't use it for interFoam.

[zandi]

Originally Posted by wyldckat

Hi zandi,

The 3 "larger than" characters (>>>) mean that you're working inside the Python shell. Those commands you have tried to use are meant to be used from the bash/sh shell, not Python.

Therefore, you will need to run these commands:

quit()

turbFoam > log &
pyFoamPlotWatcher.py log

Which will look something like this on your screen:

>>> quit()

ofuser@machine:~$ turbFoam > log &
ofuser@machine:~$ pyFoamPlotWatcher.py log

Best regards,
Bruno

Dear Bruno,
I still have the same problem maybe I didn't do your advice right and di not understand it. could please tell me more about it or guide me to a useful tutorial please

[saeedi]

Thanks for your reply.

Any comments regarding my third question?

Thanks

[wyldckat]

Quick answers:

Originally Posted by zandi

Dear Bruno,
I still have the same problem maybe I didn't do your advice right and di not understand it. could please tell me more about it or guide me to a useful tutorial please

• Tutorial on how to use Python: https://www.python.org/about/gettingstarted/
• Tutorial on how to use the shell: http://linuxcommand.org/lc3_learning_the_shell.php
• Tutorials on how to use PyFoam: http://openfoamwiki.net/index.php/Co...Other_material

Originally Posted by saeedi

Any comments regarding my third question?

Please ask that 3rd in a separate thread, because this thread says right on the title "Tutorial of how to plot residuals !", in other words, it's for asking questions about plotting residuals.

[BlnPhoenix]

Hello,

i have difficulties plotting my simpleFoam residuals. My log files looks like

Starting time loop

Time = 1

DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.0657653, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.0290663, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.0416476, No Iterations 1
DICPCG: Solving for p, Initial residual = 1, Final residual = 0.00888325, No Iterations 313
time step continuity errors : sum local = 0.000143341, global = -5.07606e-008, cumulative = -5.07606e-008
ExecutionTime = 6.233 s  ClockTime = 6 s

Time = 2

DILUPBiCG:  Solving for Ux, Initial residual = 0.362055, Final residual = 0.0114528, No Iterations 2
DILUPBiCG:  Solving for Uy, Initial residual = 0.529153, Final residual = 0.0453389, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 0.33249, Final residual = 0.0105906, No Iterations 2
DICPCG:  Solving for p, Initial residual = 0.939307, Final residual = 0.0085134, No Iterations 398
time step continuity errors : sum local = 0.000600287, global = -4.63279e-008, cumulative = -9.70885e-008
ExecutionTime = 10.351 s  ClockTime = 10 s

and i use the residuals script:

set logscale y
set title "Residuals"
set ylabel 'Residual'
set xlabel 'Iteration'
plot "< cat Log | grep 'Solving for Ux' | cut -d' ' -f12 | tr -d ','" title 'Ux' with lines,\
"< cat Log | grep 'Solving for Uy' | cut -d' ' -f12 | tr -d ','" title 'Uy' with lines,\
"< cat Log | grep 'Solving for Uz' | cut -d' ' -f12 | tr -d ','" title 'Uz' with lines,\
"< cat Log | grep 'Solving for p' | cut -d' ' -f12 | sed -n 'p;N;N' | tr -d ','" title 'p' with lines
pause 1
reread

The error message i get from gnuplot is:

  the command "cat" is written wrong or could not be found.

and

line 8: x range is invalid

i tried to change the -f12 values to different but i was not lucky.

I'm running OpenFoam and gnuplot under Windows with cygwin64. The command to execute gnuplot is:

gnuplot> load E:/Residuals.txt

Can somebody please help me. Thanks a lot!