# 10.5.1. Using the pyopus symbol library¶

For drawing schematics that will be used for generating netlists you can use arbitrary KiCad schematic components. But the most straightforward way is to use the pyopus symbol library of schematic components. Predefined rules exist for netlisting these components. For other KiCad schematic components you will have to write your own netlisting rules. In some cases even the default netlisting rule will be good enough.

# 10.5.2. Getting started with your first schematic¶

First, note that in KiCad 6 schematic files have the .kicad_sch extension. This tutorial was written for KiCad 5. So if you are using KiCad 6, whenever you encounter .sch in this tutorial, note that the correct extension should be .kicad_sch.

One KiCad schematic can be subdivied in several .sch files, but in the end this hierarchy will be flattened to produce one netlist file which is either a top-level netlist or defines one subcircuit.

To introduce the PyOPUS netlister for KiCad we are going to draw two schematics. The first one (miller.sch) defines a Miller operational transconductance amplifier (OTA) as a subcircuit. The second one (topdc.sch) uses this subcircuit and simulates its DC and AC behavior.

In the folder where the schematic files will be stored start eeschema by typing

eeschema


Before you proceed, save the file by choosing File/Save Current Sheet As… Specify miller.sch as the file name. If you want to open the schematic later you must type

eeschema pwd/miller.sch


The pwd prefix must be added because eeschema requires a full path to be specified. If you open the schematic file by doubleclicking it in the file manager (e.g. Dolphin) a full path to the file will be passed to eeschema automatically. Under Windows use the File Explorer for opening schematic files to avoid typing the full path when invoking eeschema. This behavior seems to be gone in KiCad 6, where you can again specify only the schematic file without the fuill path.

The Miller OTA schematic is constructed using the following components from the pyopus symbol library

• NMOS and PMOS for the MOS transistors

• RES and CAP for the resistor and capacitor

• ISRC for the independent current source

• OUTPUT_FILE for defining the output netlist file name

• SUBCKT for defining the subciruit name and pin order

Miller OpAmp schematic.

Note that at netlisting KiCad will insist that all your component names end with a number. So don’t waste your time trying to force Ma as the MOS transistor name. Name it Ma1 instead.

MOS transistors have 3 numbers associated with every symbol. The bold one is the channel width (W). Right above/below it (depending on symbol’s rotation) is the channel length (L). Somewhat further away is the multiplier factor (M). The model name is specified as the Model filed.

By default the netlister will recognize components GND, GNDA, GNDD, GNDPWR, and GNDREF as ground nodes. You can change this in the netlister configuration. See the documentation of pyopus.netlister on how to do this. The customized configuration must be stored in a netlister.json file in the folder where the intermediate XML netlists will be generated by KiCad.

The pins of the subcircuit must be named with global labels. If you place a SUBCKT component from pyopus library the whole schematic will be treated as a subcircuit definition. The name of the subcircuit and the net names of its pins are defined as Fields of the SUBCKT component.

To define subcircuit parameters use the SUBCKT_PARAM components (one for every parameter). Arbitrary parameters can be defined using the PARAM component (one per parameter). Every PARAM component translated to one .param statement inside the subcircuit definition (or in the top-level netlist of the schematic defines a top-level netlist).

Before generating the netlist save the schematic by choosing File/Save from the mneu. Select Tools/Generate Netlist File in the eeschema menu. A window will pup up. Select the Spice Opus tab and click on the Generate button. A file dialog will pup up asking you for the netlist file name, After entering it and clicking the Save button the intermediate XML netlist will be generated and the PyOPUS KiCad netlister plugin will be invoked. This plugin reads the XML file and the netlister configuration files (.json files) that customize its behavior. After that it outputs the nelist. If you place an OUTPUT_FILE component in your schematic this component will define the name of the netlist file regardless of what you specify in the file dialog (the file name will only be used for the intermediate netlist). After the netlist file is generated a window will pop up showing the contents of the netlist file miller.inc.

*********
* SPICE OPUS netlister for KiCad
* (c)2017 EDA Lab FE Uni-Lj
*
* Netlister : KiCad -> Spice Opus
* Config    : default used
* Date      : Wed 13 Oct 2021 01:56:05 PM CEST
* Tool      : Eeschema 5.1.9+dfsg1-1
* Sheet 1   : / -- miller.sch
*********

.subckt miller inp inn out vdd vss

* Sheet: /
m2 (net003 net002 vss vss) nmosmod w=79.46u l=1.91u m=1
m1 (net002 net002 vss vss) nmosmod w=20.80u l=0.32u m=1
m3 (out net002 vss vss) nmosmod w=60.23u l=0.32u m=1
m6 (net005 net005 vdd vdd) pmosmod w=90.43u l=3.92u m=1
m7 (net004 net005 vdd vdd) pmosmod w=90.43u l=3.92u m=1
m8 (out net004 vdd vdd) pmosmod w=83.01u l=0.20u m=2
i1 (vdd net002)  dc=100u
r1 (out net001) r=67.6k
c1 (net001 net004) c=13.5p
m4 (net005 inn net003 vss) nmosmod w=67.29u l=3.97u m=1
m5 (net004 inp net003 vss) nmosmod w=67.29u l=3.97u m=1

.ends



You can close it by pressing Enter or Esc or clicking on the Close button.

To define the top-level netlist start another instance of eeschema by typing

eeschema


Note that eeschema will complain it is already running. Simply ignore the message and click Yes to continue. Save the empty schematic as topdc.sch. The top level schematic uses the following pyopus symbol library components

• VSRC for the independent voltage sources

• VCVS for the voltage-controlled voltage source

• RES and CAP for resistors and capacitors

• OPAMP for the opamp

• OUTPUT_FILE for specifying the output netlist file name

• INCLUDE for including an external file (miller.inc)

• LIB for including section tm of the library file (cmos180n.lib)

Testbench circuit schematic.

All nodes that will be accessed by the Spice Opus commands are named explicitly with global labels. The Value filed of the OPAMP is set to the name of the subcircuit that defines the Miller OTA (included from file miller.inc). By default all components that do not have a netlisting rule defined are netlisted as subcircuits. The Value field specifies the subcircuit name. The nodes of the subcircuit instance are dumped in the increasing pin number order of the component.

Any text block will be added to the netlist above/below netlisted components if it starts with the line

Text<number> position=top|bottom


If there are multiple text blocks they are dumped in in the increasing number order. Note that the schematic file must be saved before netlisting so that the netlister can extract the text blocks from the schematic file. We use this text block feature to add a .control block to the netlist with the commands thet will run a DC and an AC analysis and plot the results.

Save the finished schematic by choosing File/Save from the menu. After netlisting the topdc.sch file the following netlist will be written to the topdc.cir file (due to the OUTPUT_FILE component).

*********
* SPICE OPUS netlister for KiCad
* (c)2017 EDA Lab FE Uni-Lj
*
* Netlister : KiCad -> Spice Opus
* Config    : default used
* XML input : topdc.xml
* Output    : topdc.cir
* Date      : Tue Apr 19 08:54:27 2022
* Tool      : Eeschema 6.0.4+dfsg-1~bpo11+1
* Sheet 1   : / -- topdc.kicad_sch
*********

.include miller.inc
.lib 'cmos180n.lib' tm

* Sheet: /
cl1 (net001 0) c=1p
e1 (out 0 net001 0) gain=1
r1 (inn in) r=1meg
r2 (out inn) r=1meg
rl1 (net001 0) r=100meg
vcom1 (inp 0)  dc=0
vdd1 (vdd 0)  dc=0.9
vin1 (in 0)  dc=0 ac=1
vss1 (vss 0)  dc=-0.9
x1 (inp inn net001 vdd vss) miller

* Verbatim block Text1 from sheet /
.control
destroy all
delete all

dc vin1 -0.9 0.9 lin 500
plot v(out) vs v(inp,inn) xl -5m 2m

set units=degrees
ac dec 100 1 1g
plot db(v(out)/v(inp,inn)) unwrap(phase(v(out)/v(inp,inn)))
.endc

.end


You can run the simulation by typing

spiceopus topdc.cir


Demo files for this section can be found here.