Welcome to skidl Discussions!

[xesscorp]

Welcome!

SKiDL is a module that allows you to compactly describe the interconnection of electronic circuits and components using Python. The “normal” way of designing electronics is graphically using a schematic editor. SKiDL replaces this with a text-based programming paradigm. Naturally, this can seem a bit odd to electronics designers, but not to programmers. On the other hand, programmers might find electronic design somewhat mysterious. This forum serves as a place for everyone to ask questions about designing electronics with SKiDL and future directions/enhancements for the language:

• Ask questions you’re wondering about.
• Share ideas.
• Engage with other community members.

To get started, open a separate thread/discussion with an introduction to yourself and tell us about what you want to do with this community.

[2themaxx]

A few notes for input on using SKiDL:

1. the library extensions are case sensitive. I'm not sure if you're using a Windows dev machine, but you might want to document this. I was trying to access an example part from one of the ngspice examples and was tearing my hair out trying to figure out why it wouldn't read. It turns out the ngspice was using ".LIB" instead of ".lib" for the extensions on the parts
2. SKiDL 1.0.0 is apparently incompatible with PySpice 1.4.3 for the SpiceLibrary. There is no option "recurse=true" in the constructor of spice.py (under skidl/tools, line 116-119), when using the same code (only difference was skidl was 0.0.30 upgraded to 1.0.0). you might want to update and put a requirements.txt in the beginning or use some virtual environments to make sure you capture default. Maybe these should be under issues, but I thought I would post here since they are 2 separate issues.

[xesscorp]

Thanks for using the forum!

the library extensions are case sensitive. I'm not sure if you're using a Windows dev machine, but you might want to document this. I was trying to access an example part from one of the ngspice examples and was tearing my hair out trying to figure out why it wouldn't read. It turns out the ngspice was using ".LIB" instead of ".lib" for the extensions on the parts

Which ngspice example triggered this problem? I'd like to take a look at it.

SKiDL 1.0.0 is apparently incompatible with PySpice 1.4.3...

I replied to this issue here.

[xesscorp]

I'm working on this. I'll let you know when I have any answers.

[2themaxx]

NGspice needs behavior set to Pspice

This seems to be an inconsistency with the way Ngspice interprets it's control parameters. The syntax errors are due to the pspice syntax. It also appears that set ngbehavior=psa only works from a .spiceinit, setting ngbehavior outside of a .spiceinit file (i.e. inside a spice file) doesn't appear to work, but setting it manually and then using "source" from the ngspice command line does. Using the output of print(circ) from above I got this to work (but only if ngbehavior was set before reading the file, the line pre_set ngbehavior=psa doesn't appear to do anything, commenting it out doesn't appear to affect it, I get the syntax error eitehr way).

I'm not sure how to add the raw_spice from the if ngspice won't interpret the command. This may not really be a SKiDL problem anymore.

The following spice deck will run from the examples directory, but not in another directory without the .spiceinit...

.title
.control
pre_set ngbehavior=psa
.endc
.include TLC555.lib
.TRAN 10u 100MS
.OPTIONS RELTOL=.0001
.SAVE  v(N_3) v(N_5) v(N_2)


V2 N_1 0 5V
VRESET N_4 0 DC 0V PULSE(0V 5V 1us 1us 1us 30ms 50ms)
RA N_1 N_2 1kOhm
RB N_2 N_3 5kOhm
C N_3 0 0.5uF
Ccont N_6 0 0.5uF
RL N_1 N_5 1kOhm
X1 N_3 N_6 N_3 N_4 N_5 N_2 N_1 0 tlc555


.control
      run
      plot v(N_3) v(N_5) v(N_2)
.endc
.END

[xesscorp]

I went through pretty much the same things you did:

1. Just running your original code through Python generates two types of errors: 1) ngspice errors parsing the TLC555.LIB file (Bad element...); 2) Bunches of ngspice errors as it tries to run whatever PySpice gave it and then it hangs.
2. Once I place the .spiceinit file into the same directory, running your original code through Python generates two types of errors: 1) the same ngspice errors parsing the TLC555.LIB file (Bad element...); 2) PySpice error when trying to run ngspice (NgSpiceCommandError).
3. ngspice runs to completion (but still finds error in the TLC555.LIB file) and generates some output waveforms when given a file containing the SPICE netlist generated by SKiDL and adding the necessary preamble/postamble:

.title 
.include /media/devb/Main/TEMP/ngspice-33/examples/p-to-n-examples/TLC555.LIB
.tran 10us 100ms
.save v(N_4) v(N_3) v(N_5)
V2 N_1 0 5V
VRESET N_4 0 DC 0V PULSE(0V 5V 1us 1us 1us 30ms 50ms)
RA N_1 N_2 1kOhm
RB N_2 N_3 5kOhm
C N_3 0 0.5uF
Ccont N_6 0 0.5uF
RL N_1 N_5 1kOhm
X1 N_3 N_6 N_3 N_4 N_5 N_2 N_1 0 tlc555
.control
run
plot v(N_3) v(N_5)
.endc
.end

4. ngspice runs to completion (still with errors in the TLC555.LIB file) when given the 555-timer-2.cir file and generates the same output waveforms as the SKiDL-generated netlist. These waveforms for the TLC555 don't seem correct since there aren't any pulses being generated. This is probably a result of the errors found in the library file. The ua555 model does seem to be doing more interesting things.

Based on these results, I would say:

1. The .spiceinit file is definitely needed.
2. There are errors in the TLC555.LIB that prevent ngspice from executing that model correctly regardless of what SKiDL does.
3. SKiDL generates the correct SPICE netlist.
4. PySpice has some problem communicating with ngspice whether .spiceinit is present or not. Possibly this is caused by the errors in TLC555.LIB since PySpice works OK with ngspice in other examples.

In order to make more progress, I tried to correct the errors in TLC555.LIB file. I removed the LAMBDA parameter in the NMOS and PMOS models. ngspice doesn't report any errors in the TLC555.LIB file after that, but the waveforms are still incorrect (or, at least, no different). When I use SKiDL and PySpice, the "bad element" errors are still there and no output gets generated. Those errors seem to be related to the model parameter of S elements (switch primitives). SKiDL doesn't have any part in generating those since they're already included in TLC555.LIB, so it must be a problem with PySpice processing that element in that library. Correcting that problem might let SKiDL successfully complete the simulation although the waveforms would probably still be incorrect. But that's likely a problem with the 555 model.

[2themaxx]

use simulator.ngspice.exec_command to set ngbehavior=psa in pyspice

There's an error in PySpice 1.5 (near as I can tell). The solution to get the simulation running is to execute the line:
sim.ngspice.exec_command('set ngbehavior=psa')
between the lines:

sim = circ.simulator()               # Get a simulator for the Circuit object.
waveforms = sim.transient(step_time=0.01@u_ms, end_time=100@u_ms)  # Run a transient simulation from 0 to 100 msec.

which puts it into psa mode. I understand there's an issue with the lambda parameter, but that is an ngspice compatability mode problem, but it generates comparable waveforms on my machine when executing directly from ngspice.

I was using ngspice-31 (Ubuntu 20.04), and PySpice 1.5 uses ngspice-32, so the output is different (32 uses true gmin stepping rather than the dynamic gmin stepping 31 does), but I get an error when I run the circuit (it starts the run, but urps on the transient solution).

#output (from working PSA compatability mode)

Note: Starting true gmin stepping
Trying gmin =   1.0000E-03 Note: One successful gmin step
Trying gmin =   1.0000E-04 Note: One successful gmin step
Trying gmin =   1.0000E-05 Note: One successful gmin step
Trying gmin =   1.0000E-06 Note: One successful gmin step
Trying gmin =   1.0000E-07 Warning: Further gmin increment
Trying gmin =   5.6234E-07 Note: One successful gmin step
Trying gmin =   2.3714E-07 Note: One successful gmin step
Trying gmin =   6.4938E-08 Note: One successful gmin step
Trying gmin =   9.3057E-09 Note: One successful gmin step
Trying gmin =   9.3057E-10 Note: One successful gmin step
Trying gmin =   9.3057E-11 Note: One successful gmin step
Trying gmin =   9.3057E-12 Note: One successful gmin step
Trying gmin =   1.0000E-12 Note: One successful gmin step
Note: True gmin stepping completed
Note: Starting true gmin stepping
Trying gmin =   1.0000E-03 Note: One successful gmin step
Trying gmin =   1.0000E-04 Note: One successful gmin step
Trying gmin =   1.0000E-05 Note: One successful gmin step
Trying gmin =   1.0000E-06 Note: One successful gmin step
Trying gmin =   1.0000E-07 Warning: Further gmin increment
Trying gmin =   5.6234E-07 Note: One successful gmin step
Trying gmin =   2.3714E-07 Note: One successful gmin step
Trying gmin =   6.4938E-08 Note: One successful gmin step
Trying gmin =   9.3057E-09 Note: One successful gmin step
Trying gmin =   9.3057E-10 Note: One successful gmin step
Trying gmin =   9.3057E-11 Note: One successful gmin step
Trying gmin =   9.3057E-12 Note: One successful gmin step
Trying gmin =   1.0000E-12 Note: One successful gmin step
Note: True gmin stepping completed
---------------------------------------------------------------------------
NgSpiceCommandError                       Traceback (most recent call last)
<ipython-input-29-e4a495050150> in <module>
      1 #sim = circ.simulator()               # Get a simulator for the Circuit object.
----> 2 waveforms = sim.transient(step_time=0.01@u_ms, end_time=100@u_ms)  # Run a transient simulation from 0 to 100 msec.
      3 # Get the simulation data.
      4 time = waveforms.time                  # Time values for each point on the waveforms.
      5 # TLC 555 pin names below

~/miniconda3/envs/circuitsimpipupd/lib/python3.8/site-packages/PySpice/Spice/Simulation.py in transient(self, *args, **kwargs)
   1212 
   1213     def transient(self, *args, **kwargs):
-> 1214         return self._run('transient', *args, **kwargs)
   1215 
   1216     ##############################################

~/miniconda3/envs/circuitsimpipupd/lib/python3.8/site-packages/PySpice/Spice/NgSpice/Simulation.py in _run(self, analysis_method, *args, **kwargs)
    117         # Fixme: Error: circuit not parsed.
    118         self._ngspice_shared.load_circuit(str(self))
--> 119         self._ngspice_shared.run()
    120         self._logger.debug(str(self._ngspice_shared.plot_names))
    121         self.reset_analysis()

~/miniconda3/envs/circuitsimpipupd/lib/python3.8/site-packages/PySpice/Spice/NgSpice/Shared.py in run(self, background)
   1190 
   1191         command = 'bg_run' if background else 'run'
-> 1192         self.exec_command(command)
   1193 
   1194         if background:

~/miniconda3/envs/circuitsimpipupd/lib/python3.8/site-packages/PySpice/Spice/NgSpice/Shared.py in exec_command(self, command, join_lines)
    849 
    850         if self._error_in_stdout or self._error_in_stderr:
--> 851             raise NgSpiceCommandError("Command '{}' failed".format(command))
    852 
    853         if join_lines:

NgSpiceCommandError: Command 'run' failed

[2themaxx]

I've reported the bug to the PySpice as an Issue. Thanks for the help! hopefully this will get fixed or a workaround will be posted, but it's not as big a deal since I now understand how to turn on PSpice compatibility mode.

[jackyhc01]

Hello

I want to use the generate_netlist() function, but I got the error message as following content.

===============================================================
File "C:\14-circuit-project\01-test\pretest01.py", line 96, in
generate_netlist(file=output)

File "C:\ProgramData\Anaconda3\lib\site-packages\skidl\Circuit.py", line 417, in generate_netlist
gen_func = getattr(self, "gen_netlist{}".format(tool))

AttributeError: 'Circuit' object has no attribute '_gen_netlist_skidl'

Could you please help to provide some suggestion or information?

I really need your help. Thanks.

Best-Regards
Jack

[xesscorp]

Thanks for using SKiDL! Please provide some information about what you did that led up to this error. I can tell that you're using Windows and Anaconda. What version of SKiDL? What is the code that you tried to execute that caused this error?

Also, let's continue this conversation in a separate thread. This thread was supposed to be an introductory/welcome message to the SKiDL discussion forum. I'm going to lock this one so no more replies can get added on.