.. include:: /project-links.txt
.. include:: /abbreviation.txt



.. getthecode:: external-source.py
    :language: python3
    :hidden:
    :notebook:


===================================
 Simulation using External Sources
===================================

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


.. code-block:: py3

    
    
    # Fixme: Travis CI macOS
    #
    # Error on line 2 :
    #   vinput input 0 dc 0 external
    #   parameter value out of range or the wrong type
    #
    # Traceback (most recent call last):
    #     analysis = simulation.transient(step_time=period/200, end_time=period*2)
    #   File "/usr/local/lib/python3.7/site-packages/PySpice/Spice/NgSpice/Shared.py", line 1145, in load_circuit
    #     raise NgSpiceCircuitError('')
    
    
    import math
    
    import matplotlib.pyplot as plt
    
    
    import PySpice.Logging.Logging as Logging
    logger = Logging.setup_logging()
    
    
    from PySpice import Circuit, Simulator, plot
    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 = Simulator.factory(simulator='ngspice-shared', ngspice_shared=ngspice_shared)
    simulation = simulator.simulation(circuit, temperature=25, nominal_temperature=25)
    
    period = float(frequency.period)
    analysis = simulation.transient(step_time=period/200, end_time=period*2)
    
    
    figure1, ax = plt.subplots(figsize=(20, 10))
    ax.set_title('Voltage Divider')
    ax.set_xlabel('Time [s]')
    ax.set_ylabel('Voltage [V]')
    ax.grid()
    ax.plot(analysis.input)
    ax.plot(analysis.output)
    ax.legend(('input', 'output'), loc=(.05,.1))
    ax.set_ylim(float(-amplitude*1.1), float(amplitude*1.1))
    
    plt.tight_layout()
    plt.show()
    


.. image:: voltage-divider.png
    :align: center