Export simulation data in Raspberry PI 4

[Daniel_Lencses]

Hello everyone!
I’m working on a Raspberry pi 4 and it has a different ARM Cortex-A72 architecture, it is compatible with software which works on armhf architecture.
So, i read the ngspice documentation and i have read this topic:

Simulation-Data Export

This forum is a user-to-user support forum and not the right place to address feature enhancements to the KiCad developers. Your request has been addressed some time ago at the bug/feature tracker https://gitlab.com/kicad/code/kicad/-/issues/2566. There also has been discussed an intermediate solution: By adding a .control section to the Eeschema circuit diagram, replacing the previous single line in a text box .ac dec 10 1 1Meg you may use the output commands offered by stand-alone ngspice.…

I have tried to implement the code which holger suggested to the OP.
On my system it would be look like this or something similar, maybe i made mistake, because sadly i’m not a linux or raspberry pi or Kicad expert.

So my “code” looks like this:

.tran 1m 800m
.control
*wait until simulation is finished
set controlswait
*cd into a file that has write access
cd /home/pi/Downloads/behav_counter_ste/Logdata
*set output format for cvs
set wr_vecnames
set wr_singlescale
option numdgt=7
*data to csv file
wrdata skey.csv “/staircase”
.endc

But when i ran the simulation then i dont get any data into the /home/pi/Downloads/behav_counter_ste/Logdata file and the simulation gives back the error message:
Current directory: /home/pi
Error: no such vector “/staircase”

In the Kicad it looks like this:

I feel like i’m missing something and i make stupid mistakes.
Could you please tell me or suggest me anything what can i do to export data from simulation in to a file in linux based system?

Thank you for listening!

Best regards,
Daniel

[holger]

@Daniel_Lencses

cd /home/pi/Downloads/behav_counter_ste/Logdata

One idea: The above command will not generate the directory, but just switch into an existing directory. So try to manually make the directory before running the simulation.

[Daniel_Lencses]

Unfortunately, i made a directory by hand so the Logdata is an existing directory, so the problem sadly is not with that, but thank you for mentioning that.
Best regards,
Daniel

[Ste]

Sounds like the 3rd to last post in that thread you linked might be the cause?

Simulation-Data Export

P.S.: I noticed, that the path for “cd …” is only interpreted in lower-case letter independent from, what I wrote in the control-section. So “cd ~/Projekte” was transformed into “cd ~/projekte” and consequently not found. Do you know, how I can apply upper-case letters, too? thx, sepp2gl

[holger]

@Daniel_Lencses

Error: no such vector “/staircase”

This tells you that the vector (as a result of the simulation) is not available.

The command ‘display’ before ‘wrdata’ will tell you what vectors you have.

[holger]

@Simulation-Data Export Simulation (Ngspice)

“cd …” is only interpreted in lower-case letter

This bug will be fixed in ngspice-33. So for now your path should be named

/home/pi/downloads/behav_counter_ste/logdata

You may also try skipping command cd and give the full path to wrdata, which already now should aknowledge upper and lower case letters.

[Daniel_Lencses]

Thank you all help!
It seems this code worked for me on Raspberry PI 4 in raspbian OS (if anyone in the future try to make something similar):

.tran 500m 7.5
.control
*wait until simulation is finished
set controlswait
*set output format for cvs
set wr_vecnames
set wr_singlescale
option numdgt=7
*data to csv file
wrdata /home/pi/behavcounter/logdata.csv V(OPAMPOUT)
.endc

in Kicad it looks like this:

Run the simulation:

The output csv file:

Maybe this is an offtopic question, but is it able to run simulation via Python script?
I was thinking, Kicad using ngspice, and the simulation generate the simulated signals,values from the sch file.
Is it a possible way, to run the simulation from Python script, generate the simulated values and export them to a csv file like in Kicad?

Best regards,
Daniel