Hi all, newbie here! I want to simulate a transistor using PySpice. Can anyone tell me the proper way of including "sky130_fd_pr__nfet_01v8_lvt" in my simple python code here? I use PySpice 1.5 / ngspice-32. Including a simple PTM model file and defining a MOSFET just works fine.

circuit.include("./ptm_90nm.model")
circuit.M('1', 'node_drain', 'node_gate',  circuit.gnd, circuit.gnd, model='nmos', width=1e-6, length=1e-6)

However, including

sky130_fd_pr__nfet_01v8_lvt.pm3.spice

and defining a subcircuit does not work.

circuit.include("../share/pdk/sky130A/libs.ref/sky130_fd_pr/spice/sky130_fd_pr__nfet_01v8_lvt.pm3.spice")
circuit.X('M1', d='node_drain', g='node_gate', s=circuit.gnd, b=circuit.gnd, model='sky130_fd_pr__nfet_01v8', w=1, l=1, subcircuit_name='nfet')
---
Error: unknown subckt: xm1 nfet b=0 d={node_drain} g={node_gate} l=1 model={sky130_fd_pr__nfet_01v8} s=0 w=1
    Simulation interrupted due to error!

Am I missing something? Please refer to the code below. It's just I-V plotting, but I'm lost. Haha

import matplotlib.pyplot as plt
import numpy as np

import PySpice
from PySpice.Spice.Netlist import Circuit, SubCircuit, SubCircuitFactory
from PySpice.Unit import u_V, u_mA

import sys, os
if sys.platform =="linux" or sys.platform =="linux2":
    PySpice.Spice.Simulation.CircuitSimulator.DEFAULT_SIMULATOR = 'ngspice-subprocess'
circuit = Circuit('IVtest')

Vdrain = circuit.V('drain', 'node_drain', circuit.gnd, 1@u_V)
Vgate = circuit.V('gate', 'node_gate', circuit.gnd, 1@u_V)

# circuit.include("./ptm_90nm.model")
# circuit.M('1', 'node_drain', 'node_gate',  circuit.gnd, circuit.gnd, model='nmos', width=1e-6, length=1e-6) # this just works fine

# circuit.lib('../share/pdk/sky130A/libs.tech/ngspice/sky130.lib.spice', 'tt')
# circuit.include("../share/pdk/sky130A/libs.tech/ngspice/corners/tt.spice")

circuit.include("../share/pdk/sky130A/libs.ref/sky130_fd_pr/spice/sky130_fd_pr__nfet_01v8_lvt.pm3.spice")
circuit.X('M1', d='node_drain', g='node_gate', s=circuit.gnd, b=circuit.gnd, model='sky130_fd_pr__nfet_01v8', w=1, l=1, subcircuit_name='nfet')
print(circuit)

simulator = circuit.simulator(temperature=27)
print(simulator)

analysis = simulator.dc(Vgate=slice(0, 2, 0.1))

figure, ax = plt.subplots(figsize=(6,3))
ax.plot(u_V(analysis.node_gate), u_mA(-analysis.Vdrain))
ax.grid()
ax.set_xlabel('Vgs [V]')
ax.set_ylabel('Id [mA]')
ax.set_yscale('log')
plt.tight_layout()
plt.show()

Including the library resulted in ~2000 lines of parsing error and >20min of running time, so I aborted it. Thanks in advance

you only need the .lib. No other includes or .libs. That is likely cause

Oh thanks! I'll just include the .lib. And generated netlist below.

.title IVtest
.include /home/acelab1/share/pdk/sky130A/libs.ref/sky130_fd_pr/spice/sky130_fd_pr__nfet_01v8_lvt.pm3.spice
Vdrain node_drain 0 1V
Vgate node_gate 0 1V
XM1 nfet b=0 d=node_drain g=node_gate l=1 model=sky130_fd_pr__nfet_01v8 s=0 w=1
.options TEMP = 27C
.options TNOM = 27C
.options NOINIT
.options filetype = binary
.end

@Wonjae Ji:

circuit.include("../share/pdk/sky130A/libs.ref/sky130_fd_pr/spice/sky130_fd_pr__nfet_01v8_lvt.pm3.spice")
circuit.X('M1', d='node_drain', g='node_gate', s=circuit.gnd, b=circuit.gnd, model='sky130_fd_pr__nfet_01v8', w=1, l=1, subcircuit_name='nfet')
---
Error: unknown subckt: xm1 nfet b=0 d={node_drain} g={node_gate} l=1 model={sky130_fd_pr__nfet_01v8} s=0 w=1
    Simulation interrupted due to error!

sky130_fd_pr__nfet_01v8_lvt

is not the same as

sky130_fd_pr__nfet_01v8

. But you are likely to have problems trying to include files if you don't start at the top with

sky130.lib.spice

. This needs a

.lib

statement, not

.include

, and I don't know how you do that with PySpice, but I assume there's a way. The output line should be

.lib /home/acelab1/share/pdk/sky130A/libs.tech/ngspice/sky130.lib.spice tt

. If you do not want the startup to take 30 minutes, then you need to copy the file ``/home/acelab1/share/pdk/sky130A/libs.tech/ngspice/spinit` to the local directory where you are running ngspice, and rename it to

.spiceinit

.

Thanks for your help, @Tim Edwards! Yes, now I did

.include

sky130 tt.

.spiceinint

tip also works fine. Thanks! But I'm still having trouble running my PySpice code. I believe now this is a PySpice matter, but I'm looking for any advice. My status: I get

NameError: Unexpected line: Scale set

. Below is the spice code generated by my PySpice code. I believe now there's no problem.

.title IVtest
.lib /home/acelab1/share/pdk/sky130A/libs.tech/ngspice/sky130.lib.spice tt
XM1 node_drain node_gate GND GND sky130_fd_pr__nfet_01v8_lvt L=1 W=1 nf=1 ad='int((nf+1)/2) * W/nf * 0.29' as='int((nf+2)/2) * W/nf * 0.29' pd='2*int((nf+1)/2) * (W/nf + 0.29)' ps='2*int((nf+2)/2) * (W/nf + 0.29)' nrd='0.29 / W' nrs='0.29 / W' sa=0 sb=0 sd=0 mult=1 m=1
Vdrain node_drain 0 1V
Vgate node_gate 0 1V
.options TEMP = 27C
.options TNOM = 27C
.options NOINIT
.options filetype = binary
.end

However, I get the error below.

NameError                                 Traceback (most recent call last)
/home/acelab1/Transistor/nfet_01v8_lvt_IV.ipynb cell 3 in <cell line: 4>()
      1 simulator = circuit.simulator(temperature=27)
      2 print(simulator)
----> 4 analysis = simulator.dc(Vgate=slice(0, 2, 0.1))

File ~/anaconda3/lib/python3.9/site-packages/PySpice/Spice/Simulation.py:1199, in CircuitSimulator.dc(self, *args, **kwargs)
   1198 def dc(self, *args, **kwargs):
-> 1199     return self._run('dc', *args, **kwargs)

File ~/anaconda3/lib/python3.9/site-packages/PySpice/Spice/NgSpice/Simulation.py:76, in NgSpiceSubprocessCircuitSimulator._run(self, analysis_method, *args, **kwargs)
     72 def _run(self, analysis_method, *args, **kwargs):
     74     super()._run(analysis_method, *args, **kwargs)
---> 76     raw_file = self._spice_server(spice_input=str(self))
     77     self.reset_analysis()
     78     raw_file.simulation = self

File ~/anaconda3/lib/python3.9/site-packages/PySpice/Spice/NgSpice/Server.py:162, in SpiceServer.__call__(self, spice_input)
    157 if number_of_points is None:
    158     raise NameError('The number of points was not found in the standard error buffer,'
    159                     ' ngspice returned:' + os.linesep +
    160                     stderr)
--> 162 return RawFile(stdout, number_of_points)
...
    221     return line
    222 else:
--> 223     raise NameError("Unexpected line: %s" % (line))

NameError: Unexpected line: Scale set

So, I think PySpice cannot handle the

Scale set

line. Anyone can point me out what to do if I wanna manage the ngspice output, i.e. disable that

Scale set

line? Maybe I'm asking odd questions... but any help will be very much appreciated!

@Wonjae Ji: Seems like PySpice is supposed to be reading an output raw file, but is also capturing the stdout (stderr?) output from ngspice. It might just be a matter of properly separating stdout and stderr output streams. But that's just a guess.

Create an issue on GitHub of PySpice so that others can find it/it can be fixed. This is something pyspice should handle I assume