[peterhess]

Hello Everybody!

Thank for the great feedback.

I tried the code and it works!

I changed the code slightly like this:

set logscale y
set title "Tmax heater"
set ylabel 'Tmax'
set xlabel 'Iteration'
plot "< cat log.chtMultiRegionSimpleFoam | grep 'Min/max' | cut -d' ' -f3 | tr -d ','" title 'Tmax'
pause 1
reread

It works actually but I have a problem.

In my log.chtMultiRegionSimpleFoam file, one iteration looks like this:

Solving for fluid region bottomAir
DILUPBiCG: Solving for Ux, Initial residual = 2.470196e-05, Final residual = 2.969919e-07, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 1.437032e-05, Final residual = 1.604827e-07, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 1.741628e-05, Final residual = 4.959543e-07, No Iterations 1
DILUPBiCG: Solving for h, Initial residual = 0.009048544, Final residual = 5.287758e-05, No Iterations 2
Min/max T:303.7611 304.39
GAMG: Solving for p_rgh, Initial residual = 4.127734e-05, Final residual = 1.326083e-06, No Iterations 1000
time step continuity errors : sum local = 1.355654e-07, global = -4.023393e-19, cumulative = -0.0886042
Min/max rho:1.156752 1.159142

Solving for fluid region topAir
DILUPBiCG: Solving for Ux, Initial residual = 1.136693e-05, Final residual = 3.449505e-08, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 8.489421e-05, Final residual = 1.582533e-07, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 2.811805e-05, Final residual = 3.09551e-08, No Iterations 1
DILUPBiCG: Solving for h, Initial residual = 0.0001787168, Final residual = 1.17763e-06, No Iterations 1
Min/max T:300 304.1752
GAMG: Solving for p_rgh, Initial residual = 0.0001523519, Final residual = 7.043136e-07, No Iterations 2
time step continuity errors : sum local = 3.013158e-07, global = -2.91909e-07, cumulative = -0.08860449
Min/max rho:1.142718 1.158621

Solving for solid region heater
DICPCG: Solving for h, Initial residual = 0.006304606, Final residual = 0.0004823271, No Iterations 1
Min/max T:304.0113 304.3917

Solving for solid region leftSolid
DICPCG: Solving for h, Initial residual = 0.009657879, Final residual = 0.0003739408, No Iterations 1
Min/max T:303.7599 304.1081

Solving for solid region rightSolid
DICPCG: Solving for h, Initial residual = 0.01246801, Final residual = 0.0004664707, No Iterations 1
Min/max T:303.8347 304.1204
ExecutionTime = 453.44 s ClockTime = 454 s

Time = 2000


In this iteration Min/max appears 5 times!

The code above prints the Tmax 5 times...

How could I print just the Min/max for a specific region, lets say for region heater?

For any feedback I would be very thankful!

Regards

Peter

[gschaider]

Originally Posted by peterhess

Hello Everybody!

Thank for the great feedback.

I tried the code and it works!

I changed the code slightly like this:

set logscale y
set title "Tmax heater"
set ylabel 'Tmax'
set xlabel 'Iteration'
plot "< cat log.chtMultiRegionSimpleFoam | grep 'Min/max' | cut -d' ' -f3 | tr -d ','" title 'Tmax'
pause 1
reread

It works actually but I have a problem.

In my log.chtMultiRegionSimpleFoam file, one iteration looks like this:

Solving for fluid region bottomAir
DILUPBiCG: Solving for Ux, Initial residual = 2.470196e-05, Final residual = 2.969919e-07, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 1.437032e-05, Final residual = 1.604827e-07, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 1.741628e-05, Final residual = 4.959543e-07, No Iterations 1
DILUPBiCG: Solving for h, Initial residual = 0.009048544, Final residual = 5.287758e-05, No Iterations 2
Min/max T:303.7611 304.39
GAMG: Solving for p_rgh, Initial residual = 4.127734e-05, Final residual = 1.326083e-06, No Iterations 1000
time step continuity errors : sum local = 1.355654e-07, global = -4.023393e-19, cumulative = -0.0886042
Min/max rho:1.156752 1.159142

Solving for fluid region topAir
DILUPBiCG: Solving for Ux, Initial residual = 1.136693e-05, Final residual = 3.449505e-08, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 8.489421e-05, Final residual = 1.582533e-07, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 2.811805e-05, Final residual = 3.09551e-08, No Iterations 1
DILUPBiCG: Solving for h, Initial residual = 0.0001787168, Final residual = 1.17763e-06, No Iterations 1
Min/max T:300 304.1752
GAMG: Solving for p_rgh, Initial residual = 0.0001523519, Final residual = 7.043136e-07, No Iterations 2
time step continuity errors : sum local = 3.013158e-07, global = -2.91909e-07, cumulative = -0.08860449
Min/max rho:1.142718 1.158621

Solving for solid region heater
DICPCG: Solving for h, Initial residual = 0.006304606, Final residual = 0.0004823271, No Iterations 1
Min/max T:304.0113 304.3917

Solving for solid region leftSolid
DICPCG: Solving for h, Initial residual = 0.009657879, Final residual = 0.0003739408, No Iterations 1
Min/max T:303.7599 304.1081

Solving for solid region rightSolid
DICPCG: Solving for h, Initial residual = 0.01246801, Final residual = 0.0004664707, No Iterations 1
Min/max T:303.8347 304.1204
ExecutionTime = 453.44 s ClockTime = 454 s

Time = 2000


In this iteration Min/max appears 5 times!

The code above prints the Tmax 5 times...

How could I print just the Min/max for a specific region, lets say for region heater?

For any feedback I would be very thankful!

Regards

Peter

The problem is that you'd have to switch according to the "Solving for fluid region bottomAir" output. Grep is not capable of this. One possibilty would be to write an awk-script (or another scripting language. But awk was made for that kind of stateful text processing). The other would be to use pyFoam (in the current release the plotting utilities automatically recognize cht-Foam and split temperature plots accordingly)

Bernhard

[peterhess]

Hello Bernhard,

Thanks for the suggestion.

I will work on it and see whats happends.

Regards

Peter

[sersol]

It still works properly. Thank you so much.

[indy07cz]

Hi foamers,
I used some ideas written here and wrote own script to plot residuals vs time on the fly during simulation. My script is for interFoam solver but it can be changed for others.

file residuals.sh prepares input data for gnuplot every n seconds and run gnuplot
file gnupl_input is gnuplot file which defines plot design

Paste these files into case folder, edit files and run ./residuals.sh during simulation. Enjoy.

[RobertHB]

This might be a bit off-topic, but i hope someone can help me. As written multiple times the original residual script works fine. Also for me. Now, as i am running transient simulation i came up with the idea of monitoring my Courant Number using the approach taken in the residual script.
The output i want to plot is:

Courant Number mean: 0.0108355 max: 0.113549

So my script reads

plot "< cat piso.log | grep 'Courant Number' | cut -d' ' -f4 | tr -d ','" title 'Co mean' with lines,\
"< cat piso.log | grep 'max:' | cut -d' ' -f8 | tr -d ','" title 'Co max' with lines,
reread

The first line reads the mean CFL value. Check. Accordingly the Co max value should be on the 8th position (read by the 2nd line). But instead an error occurs

"CFLno", line 6: warning: Skipping data file with no valid points
failed to get the current screen resources
QXcbConnection: XCB error: 170 (Unknown), sequence: 163, resource id: 90, major code: 146 (Unknown), minor code: 20
[...]
tr: Schreibfehler
cut: Schreibfehler: Datenübergabe unterbrochen (broken pipe)

Can anybode point me to my mistake?

Regards
Robert

[indy07cz]

Have you tried run second command to separate co max number simply in bash? Try simply cat, then add grep, cut an so on. I think it is on 6th position not 8th.

[gxuxg]

Originally Posted by indy07cz

Hi foamers,
I used some ideas written here and wrote own script to plot residuals vs time on the fly during simulation. My script is for interFoam solver but it can be changed for others.

file residuals.sh prepares input data for gnuplot every n seconds and run gnuplot
file gnupl_input is gnuplot file which defines plot design

Paste these files into case folder, edit files and run ./residuals.sh during simulation. Enjoy.

I have improved the scripts with regard to residuals curves, with the easy update of line titles.
Revised scripts are updated in case it is useful.

[indy07cz]

Hey that's great! What kind of coding (UTF, ...) did you use for residual.sh? I'm not able to open it correctly in Vim or Gedit.

[gxuxg]

Originally Posted by indy07cz

Hey that's great! What kind of coding (UTF, ...) did you use for residual.sh? I'm not able to open it correctly in Vim or Gedit.

Sorry, did not notice that the file had crashed.
Here they are.

[Ben UWIHANGANYE]

Hello,

I don't know if this thread is still active, but i have a question

My problem now is the difference between ux uy and P residual plot. why pressure goes up to 2000 while ux and uy ends at 500 iterations.
Could you help me to know why?

You may see my plot of residuals on attached picture


I will be happy to get your support.


Regard!

[peterhess]

Hello!

Why: Well because you have proberly 4 times pressure corrections (nNonOrthogonalCorrectors 3; ) in your PISO in the fvSolution.

The code shown above searches every time for "Solving for Ux, Solving for Ux, Solving for p".

The code find in every itteration 1 X Solving for Ux and 1 X Solving for Uy and 4 X Solving for p.

4 X 500 = 2000 !

Solution:

Well, instead of plotting the p and ux, uy on the same graph, I suggest to plot them separately.

Make a file called

plot_U

and use the following code inside:

set title "Residuals"
set ylabel 'Residual_U'
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
pause 1
reread

Make other file called

plot_p

and use the following code inside:

set title "Residuals"
set ylabel 'Residual_p'
set xlabel 'Iteration'
plot "< cat log | grep 'Solving for p' | cut -d' ' -f9 | tr -d ','" title 'p' with lines
pause 1
reread

Start gnuplot by typing:

gnuplot plot_p | gnuplot plot_U

Like that two graphs will be started simultaneously.

Or simply reduce the nNonOrthogonalCorrectors to 0 and plot as before...

Regards

Peter

[Ben UWIHANGANYE]

I thank 4r the feedback.
That approach is much better though it is not answering my question. Why does pressure residuals goes up to 2000 velocity stop at 500 iteration? (previous post)
Is there a scientific reason?

Thank you!

[peterhess]

Hello,

I answerd the question in the first section of my post.

It has no scientific reason.

If you take a look to your log file you will see in one itteration something like this:

1: smoothSolver: Solving for Ux, Initial residual = 0.931847, Final residual = 7.06554e-06, No Iterations 21
1: smoothSolver: Solving for Uy, Initial residual = 0.899434, Final residual = 7.32104e-06, No Iterations 20
1: DICPCG: Solving for p, Initial residual = 0.965189, Final residual = 0.0378369, No Iterations 20
2: DICPCG: Solving for p, Initial residual = 0.0197448, Final residual = 0.000760858, No Iterations 4
3: DICPCG: Solving for p, Initial residual = 0.000761143, Final residual = 3.19517e-05, No Iterations 19
4: DICPCG: Solving for p, Initial residual = 3.19457e-05, Final residual = 9.21943e-07, No Iterations 10

That means, in one calculation itteration you are printing 4 times for pressure.

The total number of itterations is 500. The 2000 itterations come from 4 times pressure corrections X 500!

Do the following to see the effect:

Reducing the nNonOrthogonalCorrectors in fvSolution from 3 to 0 will result:

1: smoothSolver: Solving for Ux, Initial residual = 0.931847, Final residual = 7.06554e-06, No Iterations 21
1: smoothSolver: Solving for Uy, Initial residual = 0.899434, Final residual = 7.32104e-06, No Iterations 20
1: DICPCG: Solving for p, Initial residual = 0.965189, Final residual = 0.0378369, No Iterations 20

Like that the counter for the pressure and the velocities are identical!

Regards

Peter

[Ben UWIHANGANYE]

Originally Posted by peterhess

Hello,

I answerd the question in the first section of my post.

It has no scientific reason.

If you take a look to your log file you will see in one itteration something like this:

1: smoothSolver: Solving for Ux, Initial residual = 0.931847, Final residual = 7.06554e-06, No Iterations 21
1: smoothSolver: Solving for Uy, Initial residual = 0.899434, Final residual = 7.32104e-06, No Iterations 20
1: DICPCG: Solving for p, Initial residual = 0.965189, Final residual = 0.0378369, No Iterations 20
2: DICPCG: Solving for p, Initial residual = 0.0197448, Final residual = 0.000760858, No Iterations 4
3: DICPCG: Solving for p, Initial residual = 0.000761143, Final residual = 3.19517e-05, No Iterations 19
4: DICPCG: Solving for p, Initial residual = 3.19457e-05, Final residual = 9.21943e-07, No Iterations 10

That means, in one calculation itteration you are printing 4 times for pressure.

The total number of itterations is 500. The 2000 itterations come from 4 times pressure corrections X 500!

Do the following to see the effect:

Reducing the nNonOrthogonalCorrectors in fvSolution from 3 to 0 will result:

1: smoothSolver: Solving for Ux, Initial residual = 0.931847, Final residual = 7.06554e-06, No Iterations 21
1: smoothSolver: Solving for Uy, Initial residual = 0.899434, Final residual = 7.32104e-06, No Iterations 20
1: DICPCG: Solving for p, Initial residual = 0.965189, Final residual = 0.0378369, No Iterations 20

Like that the counter for the pressure and the velocities are identical!

Regards

Peter

I am sorry, I did not read the answer entirely.
Do you have an idea about convergence? So far I think it occurs at a certain iteration where the solution is not changing compared to the previous iteration. For my case(earlier posted) I think after 150 iterations the solution was not still changing. hence simulation converged.

Is that true?

Regard!

[peterhess]

Hello!

Well this is a complatly different topic than the thread in this discussion.

This topic has been discussed so often in the Forum.

Search for those threads and you will find much informations.

Or open a new thread

Regards

Peter

[Kieran]

Hi everyone,

I've been using this script, and I'm wondering if anyone can help me with non-orthogonal correctors. In this thread a few people have talked about using sed -n 'p;N...' to only plot the first sub-iteration for pressure, which works great, although I have changed the number of non-orthogonal correctors part way through my case, does anyone know how to account for this.

Is it possible to read the first X steps of the log and plot in one way, and then plot the remaining steps in a different way, to adjust for the change in non-orthogonal correctors?

Thanks,

Kieran

[neznayer]

Thank you for that plotting solution!
But I have a question: gnuplot window keeps popping up even after the simulation is over. I think thats because it rereads the log every n seconds no matter if simulation is over or not..
How could I tell it to stop if new data isn't added to the log anymore?

[Kannan86]

While trying to plot Residuals by following the steps above I am getting an error message like this. Please help me out.





gnuplot> load "Residuals"
"Residuals" line 10: warning: Skipping data file with no valid points
"Residuals" line 10: warning: Skipping data file with no valid points
"Residuals" line 10: warning: Skipping data file with no valid points
"Residuals" line 10: warning: Skipping data file with no valid points
"Residuals" line 10: warning: Skipping data file with no valid points
"Residuals" line 10: warning: Skipping data file with no valid points

gnuplot> 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



^
"Residuals" line 10: x range is invalid

[peterhess]

I got this error also before...

I dont know why that happens, anyway the probleme could be solved by adding:

set xrange [1:*]

at the start of the skript.

Regards

Peter