[wyldckat]

Greetings BlnPhoenix,

Originally Posted by BlnPhoenix

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

[...]
I'm running OpenFoam and gnuplot under Windows with cygwin64.

I've Googled just now for:

cygwin install cat

and found this answer: http://www.linuxquestions.org/questi...4/#post3934155

Are these commands not working or are these not installed on your system?
Do you get any error message?

If it is not installed, restarted the setup.exe for cygwin and select the base system. This should include all basic tools.

More details are available at the linked page.

Best regards,
Bruno

[liu-t11]

Originally Posted by 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

thanks for this thread! it finally help me to get my problem solved!

[Tadeu_T_Rodrigues]

Hello everyone!

I have been trying to use to provided script, however I got the following problems:

1 - warning: Skipping data file with no valid points.

2 - x range is invalid.

I tried everything from the previous post (including set different cut positions), set x range and etc, without success.

Has anyone solved this problem?

I appreciate any help!

[liu-t11]

What if I want to end the plot cycle when the computation is finished. It seems that I should add an if condition before reread command, but how can I express the condition that it read "END" in log file?

Any reply is welcomed!

[vineet_bhola]

I know it is a very old post. But does someone know how to edit the Residual script for multi-Region Domain?
I am using two fluids and a solid ...and all the residuals are getting mixed up.
Thanks
Vineet

[vineet_bhola]

Let me explain my Situation a Little better. Here is my log file. What I want is it first searches only for abgas Region and get me all Residuals for abgas. But what I am getting is Ux for both abgas and wasser Region.
has anyone worked on a similar issue before? I tried man pages for grep, cut and tr. My assumption is if somehow I can ask grep to rather add the next line too for Ux, that might help. But I am not till now successful.
Vineet

 Time = 1


Solving for fluid region abgas
DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.02348612, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.01860567, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.008489814, No Iterations 1
DILUPBiCG: Solving for h, Initial residual = 1, Final residual = 0.01319835, No Iterations 1
Min/max T:800.0236 1247.3
GAMG: Solving for p_rgh, Initial residual = 0.9999939, Final residual = 0.006830426, No Iterations 11
time step continuity errors : sum local = 7.336919, global = -0.1074577, cumulative = -0.1074577
Min/max rho:0.7 0.7
DILUPBiCG: Solving for epsilon, Initial residual = 0.1393761, Final residual = 0.002278375, No Iterations 2
DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 0.02064519, No Iterations 2

Solving for fluid region wasser
DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.02964463, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.02533394, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.03579749, No Iterations 1
DILUPBiCG: Solving for h, Initial residual = 1, Final residual = 0.02474972, No Iterations 1
Min/max T:363.15 799.7066
GAMG: Solving for p_rgh, Initial residual = 0.9872267, Final residual = 0.007051082, No Iterations 3
time step continuity errors : sum local = 8885.723, global = -5147.09, cumulative = -5147.197
Min/max rho:1030.98 1030.98
DILUPBiCG: Solving for epsilon, Initial residual = 0.9995245, Final residual = 0.02359116, No Iterations 2
DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 0.001944546, No Iterations 1

Solving for solid region kopf
DICPCG: Solving for T, Initial residual = 1, Final residual = 0.0363293, No Iterations 2
Min/max T:767.9964 801.6727
ExecutionTime = 28.16 s ClockTime = 29 s

[ansubru]

Hi Vineet!!

Have you tried any of these methods?? They would work in my opinion as the output string is rather uniform in instance..

http://stackoverflow.com/questions/9...in-a-text-file

Let me know if that helped

regards

ansubru

[Mortada]

Thanks a lot it was very beneficial

[mohsen.boojari]

Hi,
I tried to use the text file but I got this error :

mohen@mohen-Lenovo-G580:~/Desktop/new-snappy$ gnuplot Residuals -
Cannot open load file 'Residuals'
"Residuals", line 0: util.c: No such file or directory

what's wrong whit this??

[thomas.]

Hi,

do you have any experiences with foamMonitor? Why do you prefer the alternatives discussed here instead of the foamMonitor one?

Thanks in advance!

[mohsen.boojari]

Hi,
unfortunately I have not worked with foamMonitor yet .

[thomas.]

ok, thanks anyway

[thomas.]

Hello all,

I am trying to adjust the script to my case. I am exporting a patchAverage of the velocity field with a function object. While trying to plot the three separate U components I am getting an error for the Ux.

The file where the data is looks like this:

#           Time         outlet
              1              (0.076778439 -2.6155751e-06 1.5359649e-05)

My gnuplot script looks like this:

set autoscale 
set key bottom right
set xlabel "Simulation time [s]"
set ylabel "Primary average velocities [m/s]"
set title "Plot of average velocity components over simulation time"
set grid

plot    "./postProcessing/patchAverage_U/0/U" using ($1):($2) with lines title "Ux"

pause 1
reread

And the error looks like this:

"U_prim.txt", line 8: warning: Skipping data file with no valid points

plot    "./postProcessing/patchAverage_U/0/U" using ($1):($2) with lines title "Ux"
                                                                                                                     ^
"U_prim.txt", line 8: x range is invalid

I think it has something to do with the "(" before the actual number, since the column "2" starts with it. If so, is there a way to "jump over" the "("?

Thanks in advance!

[rahulksoni]

Originally Posted by wolle1982

Hi all,

since apearantly noone has an idea of how to plot the residuals of a calculation on-the-fly, I will give a small manual on that:

Tutorial on "How to plot the residuals (and forces) graphically on screen on-the-fly"

Step 1:
Start the calculation and make it write out a log-file. for example

turbFoam >log

"log" is the name of the log-file to be output. It is written into the main-case-folder.

Step 2:
If desired you can open a new console-window of the main-case-folder and follow the text-output by the command

tail -f log

"log" is the name of the log-file to be read in. To stop reading the file constantly just use Crtl+C

Step 3:
To plot the residuals graphically on the screen you can use gnuplot that is delivered with linux already.
Within the main-case-folder you have to put a text file with a name e.g. "Residuals" (also see attachments).
The file should contain the following gnuplot properties:

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

The pause-command sets the seconds till reload. Deletion makes it faster in some cases.

Execute the command

gnuplot Residuals -

in the main-case-folder.

Step 4:
Another good indicator for the calculations convergence is the forces-plot. Therefore you have to set the function in the controlDict that calculates the forces and forceCoeffs. See thread http://www.cfd-online.com/Forums/ope...es-of15-3.html or attachments.

Be sure to have the properties for gnuplot in the main-case-folder (see attachments).

You have the adapt the folder-name where the forceCoeffs.dat is inside before.

While the calculation runs you also can use the gnuplot command

gnuplot forceCoeffs -

in the main-case-folder. When the forces seem to not change any more, the pressure allocation must be constantly what makes the convergent case proofed.

Step5:
Plotting the real forces is also easy. Proceed identically like in "Step 4" but be sure to set

magUInf 1.0; //free stream velocity magnitude
lRef 1.0; //reference length
Aref 1.632653; //reference area

in the controlDict.

Using the attached text-files, remove the ".txt" first.

Hope that helps somebody.

Greetings,
Wolfgang

How can I plot the same thing with x-axis as time and not iteration, as it will even simply the observations (at least I believe this).

[rahulksoni]

Originally Posted by rahulksoni

How can I plot the same thing with x-axis as time and not iteration, as it will even simply the observations (at least I believe this).

Please check http://www.cfd-online.com/Forums/ope...residuals.html

[rahulksoni]

How can I plot the same thing with x-axis as time and not iteration, as it will even simply the observations (at least I believe this).

[rahulksoni]

Ok solved the problem by getting idea from http://www.cfdsupport.com/OpenFOAM-T...rt/node80.html

You need to do following to achieve the goal.

1. In the case folder type following command to generate various log files that will be created in a new directory /logs/
   

   watch -n 60 foamLog -l log

2. foamLog creates log files in /logs/ directory. watch command here re-executes foamLog command at every 60 seconds to refresh the files as simulation is keep on running.
3. Create a file with the name ‘residuals’ in case directory and paste following code in it
   

   set multiplot layout 2, 2 title "Residuals" font ",14"
   set tmargin 5
   set title "Residuals"
   set ylabel 'Final Residual'
   set xlabel 'time'
   set grid
   
   set title "Proc 0" #font ",12"
   plot './Ux_0' with lines,\
    './Uy_0' with lines,\
    './Uz_0' with lines,\
    './p_rgh_0' with lines
   
   set title "Proc 1" #font ",12"
   plot './Ux_1' with lines,\
    './Uy_1' with lines,\
    './Uz_1' with lines,\
    './p_rgh_1' with lines
   
   set title "Proc 2" #font ",12"
   plot './Ux_2' with lines,\
    './Uy_2' with lines,\
    './Uz_2' with lines,\
    './p_rgh_2' with lines
   
   set title "Proc 3" #font ",12"
   plot './Ux_3' with lines,\
    './Uy_3' with lines,\
    './Uz_3' with lines,\
    './p_rgh_3' with lines
   
   MAX=GPVAL_DATA_Y_MAX  #extract max residual value from log files
   MIN=GPVAL_DATA_Y_MIN  #extract max residual value from log files
   set yrange [MIN:MAX+(MAX-MIN)*0.05]   #set y range to MIN and MAX+5% of MAX
   
   pause 60
   reread

4. Make this file executable by following steps at http://askubuntu.com/questions/48471...ile-executable
5. The above approach is meant for a simulation running in parallel for 4 processors. Residuals for other variables can also be added as per desire (You can check all available variables in the directory /logs/).
6. Go to logs folder
   

    
   cd logs

7. Now, run the gnuplot to start plotting the residuals
   

   gnuplot ../residuals

8. Since, our foamLog command was run along with watch, it will keep running the foamLog at specified frequency of time. And, pause command is mentioned in residuals file so it will keep refreshing the gnuplot command. Therefore, plot will keep on updating.

[rahulksoni]

Originally Posted by wolle1982

Hi all,

since apearantly noone has an idea of how to plot the residuals of a calculation on-the-fly, I will give a small manual on that:

Tutorial on "How to plot the residuals (and forces) graphically on screen on-the-fly"

Step 1:
Start the calculation and make it write out a log-file. for example

turbFoam >log

"log" is the name of the log-file to be output. It is written into the main-case-folder.

Step 2:
If desired you can open a new console-window of the main-case-folder and follow the text-output by the command

tail -f log

"log" is the name of the log-file to be read in. To stop reading the file constantly just use Crtl+C

Step 3:
To plot the residuals graphically on the screen you can use gnuplot that is delivered with linux already.
Within the main-case-folder you have to put a text file with a name e.g. "Residuals" (also see attachments).
The file should contain the following gnuplot properties:

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

The pause-command sets the seconds till reload. Deletion makes it faster in some cases.

Execute the command

gnuplot Residuals -

in the main-case-folder.

Step 4:
Another good indicator for the calculations convergence is the forces-plot. Therefore you have to set the function in the controlDict that calculates the forces and forceCoeffs. See thread http://www.cfd-online.com/Forums/ope...es-of15-3.html or attachments.

Be sure to have the properties for gnuplot in the main-case-folder (see attachments).

You have the adapt the folder-name where the forceCoeffs.dat is inside before.

While the calculation runs you also can use the gnuplot command

gnuplot forceCoeffs -

in the main-case-folder. When the forces seem to not change any more, the pressure allocation must be constantly what makes the convergent case proofed.

Step5:
Plotting the real forces is also easy. Proceed identically like in "Step 4" but be sure to set

magUInf 1.0; //free stream velocity magnitude
lRef 1.0; //reference length
Aref 1.632653; //reference area

in the controlDict.

Using the attached text-files, remove the ".txt" first.

Hope that helps somebody.

Greetings,
Wolfgang

How can I plot the same thing with x-axis as time and not iteration, as it will even simply the observations (at least I believe this).

Ok solved the problem by getting idea from http://www.cfdsupport.com/OpenFOAM-T...rt/node80.html

You need to do following to achieve the goal.

1. Before proceeding one should ensure that the OpenFoam solver is generating a log file. It can be done by appending tee log command at the end of any solver execution to write a log file name ‘log’ in the case directory. An example is presented for multiphaseInterFoam
   

   multiphaseInterFoam | tee log

2. In the case folder type following command to generate various log files that will be created in a new directory /logs/
   

   watch -n 60 foamLog log

3. foamLog creates log files in /logs/ directory. watch command here re-executes foamLog command at every 60 seconds to refresh the files as simulation is keep on running.
4. Create a file with the name ‘residuals’ in case directory and paste following code in it
   

   set multiplot layout 2, 2 title "Residuals" font ",14"
   set tmargin 5
   set title "Residuals"
   set ylabel 'Final Residual'
   set xlabel 'time'
   set grid
   
   set title "Proc 0" #font ",12"
   plot './Ux_0' with lines,\
    './Uy_0' with lines,\
    './Uz_0' with lines,\
    './p_rgh_0' with lines
   
   set title "Proc 1" #font ",12"
   plot './Ux_1' with lines,\
    './Uy_1' with lines,\
    './Uz_1' with lines,\
    './p_rgh_1' with lines
   
   set title "Proc 2" #font ",12"
   plot './Ux_2' with lines,\
    './Uy_2' with lines,\
    './Uz_2' with lines,\
    './p_rgh_2' with lines
   
   set title "Proc 3" #font ",12"
   plot './Ux_3' with lines,\
    './Uy_3' with lines,\
    './Uz_3' with lines,\
    './p_rgh_3' with lines
   
   pause 60  #wait for 60 seconds between each update
   reread

5. Make this file executable by following steps at http://askubuntu.com/questions/48471...ile-executable
6. The above approach is meant for a simulation running in parallel for 4 processors. Residuals for other variables can also be added as per desire (You can check all available variables in the directory /logs/).
7. Go to logs folder
   

    
   cd logs

8. Now, run the gnuplot to start plotting the residuals
   

   gnuplot ../residuals

9. Since, our foamLog command was run along with watch, it will keep running the foamLog at specified frequency of time. And, pause command is mentioned in residuals file so it will keep refreshing the gnuplot command. Therefore, plot will keep on updating.

[fredicenci]

Hello Everyone,
Could someone help me out? The plots for the residuals worked =). However, for the forces I've got this error:

--> FOAM FATAL ERROR:
Could not find rho

From function void Foam::functionObjects::forces::initialise()
in file forces/forces.C at line 196.

FOAM exiting

I am a beginner in openFoam and I would really appreciate the help. Thank you guys!!

[fredicenci]

Originally Posted by fredicenci

Hello Everyone,
Could someone help me out? The plots for the residuals worked =). However, for the forces I've got this error:

--> FOAM FATAL ERROR:
Could not find rho

From function void Foam::functionObjects::forces::initialise()
in file forces/forces.C at line 196.

FOAM exiting

I am a beginner in openFoam and I would really appreciate the help. Thank you guys!!

Solved. Just change rhoName for rho!