CoupledInductor does not add prefix to inductor names

[mpea413]

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

Windows 7,
'3.6.4 |Anaconda, Inc.| (default, Jan 16 2018, 10:22:32) [MSC v.1900 64 bit (AMD64)]'
'1.3.2'
ngspice

Description of the bug

Running a simple coupled inductor circuit, with an ac analysis

# Imports
import numpy as np
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.Unit import *

# Parameters
frequency = 1e3
period = 1 / frequency
omega = 2 * np.pi * frequency

I_P1 = 100
L_P1 = 1e-6
L_S1 = 10e-6
K_P1S1 = 0.1

circuit = Circuit("2CoupledInductors")

#Primary Side
circuit.I("I2", circuit.gnd, "N1", "AC " + str(I_P1) + "")
circuit.L("L_P1", circuit.gnd, "N1", str(L_P1))

# Secondary Side
circuit.L("L_S1", circuit.gnd,  "N2", str(L_S1) )
circuit.K("K_P1S1", "L_P1", "L_S1", K_P1S1)

# Do the simulation
simulator = circuit.simulator(temperature=25, nominal_temperature=25)
analysis = simulator.ac(variation="lin", number_of_points=1, start_frequency=frequency, stop_frequency=frequency)

# Print the results
print("--- Results ---")
for node in analysis.nodes.values():
  print('Node {}: {:5.2f} V'.format(str(node), float(abs(node))))

Raises a NameError('Invalid plot name') from _run in PySpice/Spice/NgSpice/Simulation.py. I think this is because the simulator failed to run (could update the exception with that fact).
I then printed the netlist by adding

print(str(self))

to that same _run method in PySpice/Spice/NgSpice/Simulation.py

The netlist that was produced is

.title 2CoupledInductors
II2 0 N1 AC 100
LL_P1 0 N1 1e-06
LL_S1 0 N2 1e-05
KK_P1S1 L_P1 L_S1 0.1
.options TEMP = 25°C
.options TNOM = 25°C
.ic 
.ac lin 1 1000.0Hz 1000.0Hz
.end

Which highlights that the error is because the inductors are defined with an extra L prefix in their definitions, but this prefix is not added to the inductors in the CoupledInductor command.

The code runs as expected when this change is made

# Imports
import numpy as np
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.Unit import *

# Parameters
frequency = 1e3
period = 1 / frequency
omega = 2 * np.pi * frequency

I_P1 = 100
L_P1 = 1e-6
L_S1 = 10e-6
K_P1S1 = 0.1

circuit = Circuit("2CoupledInductors")

#Primary Side
circuit.I("I2", circuit.gnd, "N1", "AC " + str(I_P1) + "")
circuit.L("L_P1", circuit.gnd, "N1", str(L_P1))

# Secondary Side
circuit.L("L_S1", circuit.gnd,  "N2", str(L_S1) )
circuit.K("K_P1S1", "LL_P1", "LL_S1", K_P1S1) # NB, it adds an L to the name of the inductor ... 

# Do the simulation
simulator = circuit.simulator(temperature=25, nominal_temperature=25)
analysis = simulator.ac(variation="lin", number_of_points=1, start_frequency=frequency, stop_frequency=frequency)

# Print the results
print("--- Results ---")
for node in analysis.nodes.values():
  print('Node {}: {:5.2f} V'.format(str(node), float(abs(node))))

prints the expected results

--- Results ---
Node n2:  0.20 V
Node n1:  0.63 V

Suggestions

It seems like perhaps the CoupledInductor method should automatically add the L prefix to the passed inductor names, to match with the Inductor method behavior.