Using circuit.simulator(simulator='ngspice-subprocess',...) breaks PySpice execution

[cyber-g]

Environment (OS, Python version, PySpice version, simulator)

Ubuntu 20.04.6 LTS
Python 3.8.10
PySpice version: '1.5'
Simulator: NGSpice

Expected Behaviour

No error message ; elements values should be printed

Actual Behaviour

PySpice stops with the following output:

me@compute:PySpice/examples/resistor$ python3 voltage-divider.py 
2023-09-08 19:08:14,060 - PySpice.Spice.Netlist.Node.__init__ - WARNING - Node name 'in' is a Python keyword
2023-09-08 19:08:14,071 - PySpice.Spice.NgSpice.Server.SpiceServer.__call__ - INFO - Start the spice subprocess
Traceback (most recent call last):
  File "voltage-divider.py", line 27, in <module>
    analysis = simulator.operating_point()
  File "git-dir/PySpice/PySpice/Spice/Simulation.py", line 1194, in operating_point
    return self._run('operating_point', *args, **kwargs)
  File "git-dir/PySpice/PySpice/Spice/NgSpice/Simulation.py", line 76, in _run
    raw_file = self._spice_server(spice_input=str(self))
  File "git-dir/PySpice/PySpice/Spice/NgSpice/Server.py", line 162, in __call__
    return RawFile(stdout, number_of_points)
  File "git-dir/PySpice/PySpice/Spice/NgSpice/RawFile.py", line 170, in __init__
    raw_data = self._read_header(stdout)
  File "git-dir/PySpice/PySpice/Spice/NgSpice/RawFile.py", line 192, in _read_header
    self.circuit_name = self._read_header_field_line(header_line_iterator, 'Circuit')
  File "git-dir/PySpice/PySpice/Spice/RawFile.py", line 243, in _read_header_field_line
    raise NameError("Expected label %s instead of %s" % (expected_label, label))
NameError: Expected label Circuit instead of No compatibility mode selected
me@compute:PySpice/examples/resistor$ 

The failure happens for any kind of circuit but is demonstrated below with one of the builtin example.

Steps to reproduce the behaviour

Open example examples/resistor/voltage-divider.py and replace line L25:

simulator = circuit.simulator(temperature=25, nominal_temperature=25)

with

simulator = circuit.simulator(simulator='ngspice-subprocess',temperature=25, nominal_temperature=25)

Then run :

python3 voltage-divider.py

[cyber-g]

I have investigated the problem. It comes from an evolution on NGSpice side that began on 2021-01-01 :
https://sourceforge.net/p/ngspice/ngspice/ci/1234c3bdf8a48e6201a3ecf03e10396657fa96e8/tree//src/frontend/inpcom.c?diff=164d3dd20c6008d842bd4ae34d63d3ae22923e68

From that moment, inpcom.c began to display a message at the very beginning of the output of the simulation mode.
The message has been latter moved to inpcompat.c.

The message can be easily shown with the following command from the terminal :

echo "bla" | ngspice -s

No compatibility mode selected!


Circuit: bla

Note: No ".plot", ".print", or ".fourier" lines; no simulations run

which mimics what is done in Server.py

If one sets an spinit file containing a compatibility setting, for example:

set ngbehavior=hsa

and configures the SPICE_SCRIPTS environment variable to use this spinit file then you get:

echo "bla" | ngspice -s

Compatibility modes selected: hs a


Circuit: bla

Doing analysis at TEMP = 27.000000 and TNOM = 27.000000

Please note that the message is not an error; it is just a note given by NGSpice.

To fix the issue, one may want to update :
_read_header

to contain something like:

self.note = self._read_header_field_line(header_line_iterator, 'Note')

(only valid for the latest versions of NGSpice (later than 2022-03-14)

I need to check if this first idea for fix is valid.

[cyber-g]

Please note, that there is no issue when using the circuit.simulator(simulator='ngspice-shared') option instead

[KolosKoblasz]

Hi @cyber-g !

I'm trying to run ngspice sims with PySpice on Ubuntu, but I'm stuck on an issue.
Could you help me to fix it?

I created the environment variable in my .bashrc:
export SPICE_SCRIPTS="/home/kolos/spinit"
echo $SPICE_SCRIPTS /home/kolos/spinit

but ngspice can't find the spinit file:

Note: can't find the initialization file spinit.

Note: No compatibility mode selected!


Circuit: bla

Doing analysis at TEMP = 27.000000 and TNOM = 27.000000

Using SPARSE 1.3 as Direct Linear Solver

[cyber-g]

Dear @KolosKoblasz

Your issue is a little bit off topic of this track issue. However, it should be easy to fix with following explanation.
The environment variable SPICE_SCRIPTS should contain the path of the directory that contains the spinit file.

This is documented here : 12.5 Standard configuration file spinit

The path may be overridden by setting the environmental variable SPICE_SCRIPTS to a path where spinit is located.

So if you have your spinit file in /home/kolos/, then you have to put in your .bashrc:

export SPICE_SCRIPTS="/home/kolos/"