Introduction to PySpice (Python) for Simulating MOSFETs and MOSFET Amplifier Circuits

Описание

This video shows to how to simulate MOSFETs and MOSFET amplifier circuits in PySpice (Python) and LTSPICE.

It has the following chapters:
(00:00) [1] Introduction
(00:17) [2] Why MOSFETs are important
(01:21) [3] MOSFET models in PySpice
(02:58) [4] MOSFET Level 1 model in PySpice
(04:13) [5] How to add MOSFET models in LTSPICE
(06:12) [6] How to define MOSFET channel length and width
(08:00) [7] MOSFET amplifier circuit in PySpice

The Python code is posted below and also in the video comments section.

# Pyspice (Python) code to simulate MOSFET Amplifier Circuit
#####################################################

# STANDARD DECLARATIONS
# ------------------------

import matplotlib.pyplot as plt
from matplotlib.widgets import Cursor
import numpy as np
from engineering_notation import EngNumber

import PySpice.Logging.Logging as Logging
logger = Logging.setup_logging()

from PySpice.Doc.ExampleTools import find_libraries
from PySpice.Probe.Plot import plot
from PySpice.Spice.Library import SpiceLibrary
from PySpice.Spice.Netlist import Circuit
from PySpice.Unit import *


# CIRCUIT NETLIST
# ------------------------

circuit = Circuit('Common-Source MOSFET Amplifier')

# Define amplitude and frequency of input sinusoid
amp=100@u_mV
freq=1@u_kHz
# Define transient simulation step time and stop time
steptime=1@u_us
finaltime = 5@u_ms

# Define MOSFET models
# https://ltwiki.org/LTspiceHelp/LTspiceHelp/M_MOSFET.htm
# https://ltwiki.org/index.php?title=Standard.mos

# simplified model
circuit.model('2N7000', 'NMOS', Kp=0.13, Vto=2.475)

# simplified model with channel length and width
#circuit.model('2N7000', 'NMOS', L=100E-6, W=200E-6, Kp=0.13, Vto=2.475)

source = circuit.SinusoidalVoltageSource(2, 'input', circuit.gnd, amplitude=amp, frequency = freq)

circuit.R('s', 'input','inmos', 100@u_kΩ)
circuit.C(1,'inmos', 'gate', 1@u_uF)
circuit.R('1', 'Vdd', 'gate', 200@u_kΩ)
circuit.R('2', 'gate', circuit.gnd, 100@u_kΩ)
circuit.R('D', 'Vdd', 'drain', 3@u_kΩ)
circuit.R('So', 'source', circuit.gnd,1.5@u_kΩ)
circuit.V(1, 'Vdd', circuit.gnd, 18@u_V)
circuit.MOSFET(1, 'drain', 'gate', 'source','source', model='2N7000')
circuit.C(2,'drain', 'output', 10@u_uF)
circuit.C(3,'source', circuit.gnd, 22@u_uF)
circuit.R('L', 'output',circuit.gnd, 10@u_kΩ)

simulator = circuit.simulator(temperature=25, nominal_temperature=25)
analysis = simulator.transient(step_time=steptime, end_time=finaltime)

# THEORETICAL RESULTS
# ------------------------

print('------------------')
print('Theoretical Values')
print('------------------')

K = 0.13
VT =2.475@u_V

# DC bias analysis
VTH = (circuit.V1.dc_value)*(circuit.R2.resistance/(circuit.R1.resistance+ circuit.R2.resistance))
RTH = (circuit.R1.resistance*circuit.R2.resistance)/(circuit.R1.resistance+ circuit.R2.resistance)

a = K * float(circuit.RSo.resistance)
b = 1- 2*K*float(circuit.RSo.resistance)*np.abs(VT)
c = K*float(circuit.RSo.resistance)*VT*VT- np.abs(float(VTH))
V_GS = ((-b + np.sqrt(b*b-4*a*c))/(2*a))*1@u_V

I_D = (VTH-V_GS)/circuit.RSo.resistance

# small signal AC analysis
gm = 2*K*float((V_GS-VT))

R_in = RTH
R_o = circuit.RD.resistance
A_v = float(-gm*R_o*(R_in/(R_in + circuit.Rs.resistance))*(circuit.RL.resistance/(circuit.RL.resistance+ R_o)))

# Find the theoretical output waveform; use the time output of the simulation
time=np.array(analysis.time)
v_out = A_v*(amp)*(np.sin(2*np.pi*freq*time))

# Display the DC and AC parameter values
print('VTH={} V'.format(EngNumber(float(VTH))))
print('RTH={} Ω'.format(EngNumber(float(RTH))))
print('a={}'.format(EngNumber(a)))
print('b={}'.format(EngNumber(b)))
print('c={}'.format(EngNumber(c)))
print('VGS={} V'.format(EngNumber(float(V_GS))))
print('ID={} A'.format(EngNumber(float(I_D))))
print('gm={}'.format(EngNumber(gm)))

print('Rin={} Ω'.format(EngNumber(float(R_in))))
print('Ro={} Ω'.format(EngNumber(float(R_o))))
print('Av={}'.format(EngNumber(float(A_v))))
# # # # # # # # # # # # # # # # # # # # # # # # # # # # # # # # # # #

# # # # # # # # # # # # # # # # # # # # # # # # # # # # # # # # # # #

# SIMULATION RESULTS
# ------------------------

# Plot the voltages
figure, axe = plt.subplots(figsize=(11, 6))

plt.title('MOSFET Amplifier Voltages')
plt.xlabel('Time [s]')
plt.ylabel('Voltage [V]')
plt.grid()
plot(analysis['input'], axis=axe)
plot(analysis['output'], axis=axe)
plt.plot(time, v_out)
plt.legend(('sim:input', 'sim:output', 'theory'), loc=(.05,.1))
cursor = Cursor(axe, useblit=True, color='red', linewidth=1)

plt.show()