Using Python with ngspice

We can automate this process by using ngspice in batch mode, i.e. running the simulator from the command line, and reading the output file using Python, and do the processing automatically. To run ngspice at the command line, you can use ngspice <circuit file>.

One very good environment for Python3 is Spyder. You can download this for multiple platforms, and the easiest way to install Spyder is as part of the Anaconda distribution, also available for various operating systems.

Running ngspice from Python

Below is a simple Python script for running ngspice, reading its output. It uses the ngspice_link module, that contains convenient classes and functions for running ngspice from within Python.

 1 import matplotlib.pyplot as plt
 2 from si_prefix import si_format
 3 
 4 # import our custom ngspice module
 5 import ngspice_link as ngl
 6 
 7 # setup the simulation configuration
 8 cfg = {
 9         'ngspice' : '/Applications/ngspice/bin/ngspice', 
10         'cir_dir' : '/Users/louis/Documents/UPEEEI/Classes/EE 220/2020_1/Activities/',
11         'cir_file' : 'circuit1.sp',
12         }
13 
14 # create the ngspice object
15 sim1 = ngl.ngspice(cfg)
16 
17 # run ngspice with the configuration above
18 sim1.run_ngspice()
19 
20 # read the simulation output produced by the 'wrdata' command
21 vbe, [ic] = sim1.read_dc_analysis('circuit1.dat', [1])
22 
23 # define the plot parameters
24 plt_cfg = {
25         'grid_linestyle' : 'dotted',
26         'title' : r'2N2222a NPN BJT Transfer Characteristics',
27         'xlabel' : r'$V_{BE}$ [mV]',
28         'ylabel' : r'$I_C$ [mA]',
29         'legend_loc' : 'lower left',
30         'add_legend' : False,
31         'legend_title' : None
32         }
33 
34 fig = plt.figure()
35 ax = fig.add_subplot(1, 1, 1)
36 
37 # plot the collector current vs the base-emitter voltage
38 ax.plot(ngl.scale_vec(vbe, 1e-3), ngl.scale_vec(ic, 1e-3), '-')
39 
40 # annotate the 1mA point (arbitrary)
41 ngl.add_hline_text(ax, 1, 550, \
42         r'{:.1f} mA'.format(1))
43 
44 # find the vbe corresponding to 1mA
45 idx, icx = ngl.find_in_data(ic, 1e-3) 
46 
47 # annotate the vbe that corresponds to 1mA
48 ngl.add_vline_text(ax, vbe[idx]/1e-3, 3, r'$V_{BE}=$' + \
49         si_format(vbe[idx], precision=2) + 'V')
50     
51 # label the plot
52 ngl.label_plot(plt_cfg, fig, ax)
53 
54 # save the plot as an image
55 plt.savefig('BJT_2n2222a_transfer.png', dpi=600)

Let's go through the Python code one block at a time.

Importing Python libraries

One advantage of the Python language is its large collection of libraries, covering a vast number of topics. You can even build your own library, which is what we have done, to easily run ngspice from within Python.

1 import matplotlib.pyplot as plt
2 from si_prefix import si_format
3 
4 # import our custom ngspice module
5 import ngspice_link as ngl

Here, we imported the followibng libraries:

• The matplotlib.pyplot library that contains plotting functions.
• From the si_prefix library, we import, si_formatfunction. This function converts floating point numbers to numbers with proper SI prefixes, such as milli, centi, kilo, etc.
• Our own, user-defined library, the ngspice_link library. This library contains functions to setup the simulator, run the simulation, and extract data from the simulation output files.

Creating the ngspice Object

We can the create an ngspice object, as defined in the ngspice_link library.

 7 # setup the simulation configuration
 8 cfg = {
 9         'ngspice' : '/Applications/ngspice/bin/ngspice', 
10         'cir_dir' : '/Users/louis/Documents/UPEEEI/Classes/EE 220/2020_1/Activities/',
11         'cir_file' : 'circuit1.sp',
12         }
13 
14 # create the ngspice object
15 sim1 = ngl.ngspice(cfg)