# Simulation using External Sources¶

This example explains how to plug a voltage source from Python to NgSpice.

import math

import matplotlib.pyplot as plt

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

from PySpice.Probe.Plot import plot
from PySpice.Spice.Netlist import Circuit
from PySpice.Spice.NgSpice.Shared import NgSpiceShared
from PySpice.Unit import *

class MyNgSpiceShared(NgSpiceShared):

def __init__(self, amplitude, frequency, **kwargs):

super().__init__(**kwargs)

self._amplitude = amplitude
self._pulsation = float(frequency.pulsation)

def get_vsrc_data(self, voltage, time, node, ngspice_id):
self._logger.debug('ngspice_id-{} get_vsrc_data @{} node {}'.format(ngspice_id, time, node))
voltage[0] = self._amplitude * math.sin(self._pulsation * time)
return 0

def get_isrc_data(self, current, time, node, ngspice_id):
self._logger.debug('ngspice_id-{} get_isrc_data @{} node {}'.format(ngspice_id, time, node))
current[0] = 1.
return 0

circuit = Circuit('Voltage Divider')

circuit.V('input', 'input', circuit.gnd, 'dc 0 external')
circuit.R(1, 'input', 'output', 10@u_kΩ)
circuit.R(2, 'output', circuit.gnd, 1@u_kΩ)

amplitude = 10@u_V
frequency = 50@u_Hz
ngspice_shared = MyNgSpiceShared(amplitude=amplitude, frequency=frequency, send_data=False)
simulator = circuit.simulator(temperature=25, nominal_temperature=25,
simulator='shared', ngspice_shared=ngspice_shared)
period = float(frequency.period)
analysis = simulator.transient(step_time=period/200, end_time=period*2)

figure1 = plt.figure(1, (20, 10))
plt.title('Voltage Divider')
plt.xlabel('Time [s]')
plt.ylabel('Voltage [V]')
plt.grid()
plot(analysis.input)
plot(analysis.output)
plt.legend(('input', 'output'), loc=(.05,.1))
plt.ylim(float(-amplitude*1.1), float(amplitude*1.1))

plt.tight_layout()
plt.show()