layout

title

description

headline

TL;DR

Never use a lousy schematic editor again! SKiDL is a simple module that lets you describe electronic circuits using Python. The resulting Python program outputs a netlist that a PCB layout tool uses to create a finished circuit board.

Introduction

SKiDL is a module that allows you to compactly describe the interconnection of electronic circuits and components using Python. The resulting Python program performs electrical rules checking for common mistakes and outputs a netlist that serves as input to a PCB layout tool.

First, let's look at a "normal" design flow in KiCad:

Here, you start off in a schematic editor (for KiCad, that's EESCHEMA) and draw a schematic. From that, EESCHEMA generates a netlist file that lists what components are used and how their pins are interconnected. Then you'll use a PCB layout tool (like KiCad's PCBNEW) to arrange the part footprints and draw the wire traces that connect the pins as specified in the netlist. Once that is done, PCBNEW outputs a set of Gerber files that are sent to a PCB fabricator who will create a physical PCB and ship it to you. Then you'll post a picture of them on Twitter and promptly dump them in a drawer for a few years because you got bored with the project.

In the SKiDL-based design flow, you use a text editor to create a Python code file that employs the SKiDL library to describe interconnections of components. This code file is executed by a Python interpreter and a netlist file is output. From there, the design flow is identical to the schematic-based one (including dumping the PCBs in a drawer).

So, why would you want to use SKiDL? Here are some of the features SKiDL brings to electronic design:

Requires only a text editor and Python.
Has a powerful, flexible syntax (because it is Python).
Permits compact descriptions of electronic circuits (think about not tracing signals through a multi-page schematic).
Allows textual descriptions of electronic circuits (think about using diff and git for circuits).
Performs electrical rules checking (ERC) for common mistakes (e.g., unconnected device I/O pins).
Supports linear / hierarchical / mixed descriptions of electronic designs.
Fosters design reuse (think about using PyPi and Github to distribute electronic designs).
Makes possible the creation of smart circuit modules whose behavior / structure are changed parametrically (think about filters whose component values are automatically adjusted based on your desired cutoff frequency).
Can work with any ECAD tool (only two methods are needed: one for reading the part libraries and another for outputing the correct netlist format).
Takes advantage of all the benefits of the Python ecosystem (because it is Python).
Free software: MIT license.
Open source: https://github.com/xesscorp/skidl

As a very simple example, the SKiDL program below describes a circuit that takes an input voltage, divides it by three, and outputs it:

from skidl import *

# Create input & output voltages and ground reference.
vin, vout, gnd = Net('VI'), Net('VO'), Net('GND')

# Create two resistors.
r1, r2 = 2 * Part("Device", 'R', TEMPLATE, footprint='Resistor_SMD.pretty:R_0805_2012Metric')
r1.value = '1K'   # Set upper resistor value.
r2.value = '500'  # Set lower resistor value.

# Connect the nets and resistors.
vin += r1[1]      # Connect the input to the upper resistor.
gnd += r2[2]      # Connect the lower resistor to ground.
vout += r1[2], r2[1] # Output comes from the connection of the two resistors.

# Or you could do it with a single line of code:
# vin && r1 && vout && r2 && gnd

# Output the netlist to a file.
generate_netlist()

And this is the netlist output that is passed to PCBNEW to do the PCB layout:

(export (version D)                                                                                    
  (design                                                                                              
    (source "C:\xesscorp\KiCad\tools\skidl\tests\vdiv.py")                                             
    (date "09/14/2018 08:49 PM")                                                                       
    (tool "SKiDL (0.0.23)"))                                                                           
  (components                                                                                          
    (comp (ref R1)                                                                                     
      (value 1K)                                                                                       
      (footprint Resistor_SMD.pretty:R_0805_2012Metric)                                                                 
      (fields                                                                                          
        (field (name description) Resistor)                                                            
        (field (name keywords) "r res resistor"))                                                      
      (libsource (lib device) (part R))                                                                
      (sheetpath (names /top/12995167876889795071) (tstamps /top/12995167876889795071)))               
    (comp (ref R2)                                                                                     
      (value 500)                                                                                      
      (footprint Resistor_SMD.pretty:R_0805_2012Metric)                                                                 
      (fields                                                                                          
        (field (name description) Resistor)                                                            
        (field (name keywords) "r res resistor"))                                                      
      (libsource (lib device) (part R))                                                                
      (sheetpath (names /top/8869138953290924483) (tstamps /top/8869138953290924483))))                
  (nets                                                                                                
    (net (code 0) (name GND)                                                                           
      (node (ref R2) (pin 2)))                                                                         
    (net (code 1) (name VI)                                                                            
      (node (ref R1) (pin 1)))                                                                         
    (net (code 2) (name VO)                                                                            
      (node (ref R1) (pin 2))                                                                          
      (node (ref R2) (pin 1))))                                                                        
)

Installation

SKiDL is pure Python so it's easy to install:

$ pip install skidl

To give SKiDL some part libraries to work with, you'll also need to install KiCad. Then, you'll need to set an environment variable so SKiDL can find the libraries. For Windows, do this:

set KICAD_SYMBOL_DIR=C:\Program Files\KiCad\share\kicad\kicad-symbols

And for linux-type OSes, define the environment variable in your .bashrc like so:

export KICAD_SYMBOL_DIR="/Library/Application Support/kicad/kicad-symbols"

These paths are OS-dependent, so launch KiCAD and click Preferences->Configure Paths to reveal the needed paths.

Basic Usage

This is the minimum that you need to know to design electronic circuitry using SKiDL:

How to get access to SKiDL.
How to find and instantiate a component (or part).
How to connect pins of the parts to each other using nets.
How to run an ERC on the circuit.
How to generate a netlist for the circuit that serves as input to a PCB layout tool.

I'll demonstrate these steps using SKiDL in an interactive Python session, but normally the statements that are shown would be entered into a file and executed as a Python script.

Accessing SKiDL

To use skidl in a project, just place the following at the top of your file:

import skidl

But for this tutorial, I'll just import everything:

from skidl import *

Finding Parts

Command-line Searching

SKiDL provides a convenience function for searching for parts called (naturally) search. For example, if you needed an operational amplifier, then the following command would pull up some likely candidates:

>>> search('opamp')
linear.lib: LT1492
linear.lib: MCP601SN (2.7V to 6.0V Single Supply CMOS Operational Amplifier, SO-8)
linear.lib: LM321 (Low Power Single Operational Amplifier)
linear.lib: MCP601R (2.7V to 6.0V Single Supply CMOS Operational Amplifier, SOT-23-5)
linear.lib: LM555N (Dual Op amp, rail-to-rail, 8MHz, MSOP8, SOIC8)
...
linear.lib: MCP603ST (2.7V to 6.0V Single Supply CMOS Operational Amplifier, with Chip Select, TSSOP-8)
linear.lib: NE5534 (Low-Noise High-Speed Audio Operational Amplifier)
linear.lib: LT1493
linear.lib: MCP601P (2.7V to 6.0V Single Supply CMOS Operational Amplifier, DIP-8)
linear.lib: MCP601ST (2.7V to 6.0V Single Supply CMOS Operational Amplifier, TSSOP-8)

search accepts a regular expression and scans for it anywhere within the name, description and keywords of all the parts in the library path. (You can read more about how SKiDL handles libraries here.) So the following search pulls up several candidates:

>>> search('lm35')
dc-dc.lib: LM3578 (Switching Regulator (adjustable))
linear.lib: LM358 (Dual Rail-to-rail CMOS Operational Amplifier)
regul.lib: LM350T (3A 33V Adjustable Linear Regulator, TO-220)
sensors.lib: LM35-LP (Precision centigrade temperature sensor, TO-92 package)
sensors.lib: LM35-D (Precision centigrade temperature sensor, SOIC-8 package)
sensors.lib: LM35-NEB (Precision centigrade temperature sensor, TO-220 package)

If you want to restrict the search to a specific part, then use a regular expression like the following:

>>> search('^lm358$')
linear.lib: LM358 (Dual Rail-to-rail CMOS Operational Amplifier)

If you give search multiple terms, then it will only find parts that contain all those terms:

>>> search('opamp low-noise dip-8')

Amplifier_Operational.lib: NE5534 (Single Low-Noise Operational Amplifiers, DIP-8/SOIC-8)
Amplifier_Operational.lib: LT1012 (Single Low-Noise Operational Amplifiers, DIP-8/SOIC-8)
Amplifier_Operational.lib: SA5534 (Single Low-Noise Operational Amplifiers, DIP-8/SOIC-8)
Amplifier_Operational.lib: LM301 (Single Low-Noise Operational Amplifiers, DIP-8/SOIC-8)
Amplifier_Operational.lib: LM201 (Single Low-Noise Operational Amplifiers, DIP-8/SOIC-8)
Amplifier_Operational.lib: LM101 (Single Low-Noise Operational Amplifiers, DIP-8/SOIC-8)
Amplifier_Operational.lib: AD797 (Single Low-Noise Operational Amplifiers, DIP-8/SOIC-8)

You can also use the | character to find parts that contain at least one of a set of choices:

>>> search('opamp (low-noise|dip-8)')

Amplifier_Audio.lib: LM386 (Low Voltage Audio Power Amplifier, DIP-8/SOIC-8/SSOP-8)
Amplifier_Operational.lib: TLV2371P (Rail-to-Rail Input/Output Operational Amplifier, PDIP-8)
Amplifier_Operational.lib: MAX4239ASA (Ultra-Low Offset/Drift, Low-Noise, Precision Amplifiers, SOIC-8)
Amplifier_Operational.lib: LM4250 (Programmable Operational Amplifier, DIP-8/SOIC-8)
Amplifier_Operational.lib: LF256 (Single JFET-Input Operational Amplifiers, DIP-8/SOIC-8)
Amplifier_Operational.lib: MAX4239AUT (Ultra-Low Offset/Drift, Low-Noise, Precision Amplifiers, SOT-23-6)
Amplifier_Operational.lib: LM6361 (Single High Speed Operational Amplifier, DIP-8/SOIC-8)
Amplifier_Operational.lib: LF257 (Single JFET-Input Operational Amplifiers, DIP-8/SOIC-8)
Amplifier_Operational.lib: AD8603 (Zero-Drift, Precision, Low-Noise, Rail-to-Rail Output, 36-V Operational Amplifier, TSOT-23-5)
...

If you need to search for a string containing spaces, just enclose it in quotes:

>>> search('opamp "high performance"')

Amplifier_Operational.lib: OP77 (Single SoundPlus High Performance Audio Operational Amplifiers, DIP-8/SOIC-8)
Amplifier_Operational.lib: LT1363 (Single SoundPlus High Performance Audio Operational Amplifiers, DIP-8/SOIC-8)
Amplifier_Operational.lib: OP07 (Single SoundPlus High Performance Audio Operational Amplifiers, DIP-8/SOIC-8)
Amplifier_Operational.lib: OPA134 (Single SoundPlus High Performance Audio Operational Amplifiers, DIP-8/SOIC-8)

Once you have the part name and library, you can see the part's pin numbers, names and their functions using the show function:

>>> show('linear', 'lm358')

LM358: Dual Rail-to-rail CMOS Operational Amplifier
    Pin None/4/V-/POWER-IN
    Pin None/8/V+/POWER-IN
    Pin None/1/~/OUTPUT
    Pin None/2/-/INPUT
    Pin None/3/+/INPUT
    Pin None/5/+/INPUT
    Pin None/6/-/INPUT
    Pin None/7/~/OUTPUT

show looks for exact matches of the part name in a library, so the following command raises an error:

>>> show('linear', 'lm35')
ERROR: Unable to find part lm35 in library linear.

In addition to searching for parts, you can also search for footprints using the search_footprints command. It works similarly to the search command:

>>> search_footprints('QFN-48')

Package_DFN_QFN: QFN-48-1EP_5x5mm_P0.35mm_EP3.7x3.7mm ("QFN, 48 Pin (https://www.espressif.com/sites/default/files/documentation/esp32_datasheet_en.pdf#page=38), generated with kicad-footprint-generator ipc_dfn_qfn_generator.py" - "QFN DFN_QFN")
Package_DFN_QFN: QFN-48-1EP_5x5mm_P0.35mm_EP3.7x3.7mm_ThermalVias ("QFN, 48 Pin (https://www.espressif.com/sites/default/files/documentation/esp32_datasheet_en.pdf#page=38), generated with kicad-footprint-generator ipc_dfn_qfn_generator.py" - "QFN DFN_QFN")
Package_DFN_QFN: QFN-48-1EP_6x6mm_P0.4mm_EP4.2x4.2mm ("QFN, 48 Pin (https://static.dev.sifive.com/SiFive-FE310-G000-datasheet-v1p5.pdf#page=20), generated with kicad-footprint-generator ipc_dfn_qfn_generator.py" - "QFN DFN_QFN")
Package_DFN_QFN: QFN-48-1EP_6x6mm_P0.4mm_EP4.2x4.2mm_ThermalVias ("QFN, 48 Pin (https://static.dev.sifive.com/SiFive-FE310-G000-datasheet-v1p5.pdf#page=20), generated with kicad-footprint-generator ipc_dfn_qfn_generator.py" - "QFN DFN_QFN")
...

Zyc: A GUI Search Tool

If you want to avoid using command-line tools for part/footprint searches, then you might like to try the zyc utility. It lets you search for parts and footprints using a GUI. You can read more about it here.

Instantiating Parts

The part library and name are used to instantiate a part as follows:

>>> resistor = Part("Device",'R')

You can customize the resistor by setting its attributes:

>>> resistor.value = '1K' 
>>> resistor.value        
'1K'

You can also combine the setting of attributes with the creation of the part:

>>> resistor = Part("Device", 'R', value='1K')
>>> resistor.value
'1K'

You can use any valid Python name for a part attribute, but ref, value, and footprint are necessary in order to generate the final netlist for your circuit. And the attribute can hold any type of Python object, but simple strings are probably the most useful.

The ref attribute holds the reference for the part. It's set automatically when you create the part:

>>> resistor.ref
'R1'

Since this was the first resistor we created, it has the honor of being named R1. But you can easily change it:

>>> resistor.ref = 'R5'
>>> resistor.ref
'R5'

Now what happens if we create another resistor?:

>>> another_res = Part("Device",'R')   
>>> another_res.ref                        
'R1'

Since the R1 reference was now available, the new resistor got it. What if we tried renaming the first resistor back to R1:

>>> resistor.ref = 'R1'
>>> resistor.ref
'R1_1'

Since the R1 reference was already taken, SKiDL tried to give us something close to what we wanted. SKiDL won't let different parts have the same reference because that would confuse the hell out of everybody.

Connecting Pins

Parts are great and all, but not very useful if they aren't connected to anything. The connections between parts are called nets (think of them as wires) and every net has one or more part pins on it. SKiDL makes it easy to create nets and connect pins to them. To demonstrate, let's build the voltage divider circuit shown in the introduction.

First, start by creating two resistors (note that I've also added the footprint attribute that describes the physical package for the resistors):

>>> rup = Part("Device", 'R', value='1K', footprint='Resistor_SMD.pretty:R_0805_2012Metric')                            
>>> rlow = Part("Device", 'R', value='500', footprint='Resistor_SMD.pretty:R_0805_2012Metric')                          
>>> rup.ref, rlow.ref                                                
('R1', 'R2')                                                         
>>> rup.value, rlow.value                                            
('1K', '500')

To bring the voltage that will be divided into the circuit, let's create a net:

>>> v_in = Net('VIN')
>>> v_in.name
'VIN'

Now attach the net to one of the pins of the rup resistor (resistors are bidirectional which means it doesn't matter which pin, so pick pin 1):

>>> rup[1] += v_in

You can verify that the net is attached to pin 1 of the resistor like this:

>>> rup[1].net
VIN: Pin R1/1/~/PASSIVE

Next, create a ground reference net and attach it to rlow:

>>> gnd = Net('GND')
>>> rlow[1] += gnd
>>> rlow[1].net
GND: Pin R2/1/~/PASSIVE

Finally, the divided voltage has to come out of the circuit on a net. This can be done in several ways. The first way is to define the output net and then attach the unconnected pins of both resistors to it:

>>> v_out = Net('VO')
>>> v_out += rup[2], rlow[2]
>>> rup[2].net, rlow[2].net
(VO: Pin R1/2/~/PASSIVE, Pin R2/2/~/PASSIVE, VO: Pin R1/2/~/PASSIVE, Pin R2/2/~/PASSIVE)

An alternate method is to connect the resistors and then attach their junction to the output net:

>>> rup[2] += rlow[2]
>>> v_out = Net('VO')
>>> v_out += rlow[2]
>>> rup[2].net, rlow[2].net
(VO: Pin R1/2/~/PASSIVE, Pin R2/2/~/PASSIVE, VO: Pin R1/2/~/PASSIVE, Pin R2/2/~/PASSIVE)

Either way works! Sometimes pin-to-pin connections are easier when you're just wiring two devices together, while the pin-to-net connection method excels when three or more pins have a common connection.

Checking for Errors

Once the parts are wired together, you can do simple electrical rules checking like this:

>>> ERC()                           
                                    
2 warnings found during ERC.        
0 errors found during ERC.

Since this is an interactive session, the ERC warnings and errors are stored in the file skidl.erc. (Normally, your SKiDL circuit description is stored as a Python script such as my_circuit.py and the ERC() function will dump its messages to my_circuit.erc.) The ERC messages are:

WARNING: Only one pin (PASSIVE pin 1/~ of R/R1) attached to net VIN.
WARNING: Only one pin (PASSIVE pin 1/~ of R/R2) attached to net GND.

These messages are generated because the VIN and GND nets each have only a single pin on them and this usually indicates a problem. But it's OK for this simple example, so the ERC can be turned off for these two nets to prevent the spurious messages:

>>> v_in.do_erc = False
>>> gnd.do_erc = False
>>> ERC()

No ERC errors or warnings found.

Generating a Netlist

The end goal of using SKiDL is to generate a netlist that can be used with a layout tool to generate a PCB. The netlist is output as follows:

>>> generate_netlist()

Like the ERC output, the netlist shown below is stored in the file skidl.net. But if your SKiDL circuit description is in the my_circuit.py file, then the netlist will be stored in my_circuit.net.

(export (version D)
  (design
    (source "C:\xesscorp\KiCad\tools\skidl\skidl\skidl.py")
    (date "08/12/2016 10:05 PM")
    (tool "SKiDL (0.0.1)"))
  (components
    (comp (ref R1)
      (value 1K)
      (footprint Resistor_SMD.pretty:R_0805_2012Metric))
    (comp (ref R2)
      (value 500)
      (footprint Resistor_SMD.pretty:R_0805_2012Metric)))
  (nets
    (net (code 0) (name "VIN")
      (node (ref R1) (pin 1)))
    (net (code 1) (name "GND")
      (node (ref R2) (pin 1)))
    (net (code 2) (name "VO")
      (node (ref R1) (pin 2))
      (node (ref R2) (pin 2))))
)
(export (version D)
  (design
    (source "C:\TEMP\skidl tests\intro_example.py")
    (date "04/19/2017 04:09 PM")
    (tool "SKiDL (0.0.12)"))
  (components
    (comp (ref R1)
      (value 1K)
      (footprint Resistor_SMD.pretty:R_0805_2012Metric)
      (fields
        (field (name keywords) "r res resistor")
        (field (name description) Resistor))
      (libsource (lib device) (part R)))
    (comp (ref R2)
      (value 500)
      (footprint Resistor_SMD.pretty:R_0805_2012Metric)
      (fields
        (field (name keywords) "r res resistor")
        (field (name description) Resistor))
      (libsource (lib device) (part R))))
  (nets
    (net (code 0) (name GND)
      (node (ref R2) (pin 2)))
    (net (code 1) (name VI)
      (node (ref R1) (pin 1)))
    (net (code 2) (name VO)
      (node (ref R1) (pin 2))
      (node (ref R2) (pin 1))))
)

You can also generate the netlist in XML format:

>>> generate_xml()

This is useful in a KiCad environment where the XML file is used as the input to BOM-generation tools.

Going Deeper

The previous section showed the bare minimum you need to know to design circuits with SKiDL, but doing a complicated circuit that way would suck donkeys. This section will talk about some more advanced features.

Basic SKiDL Objects: Parts, Pins, Nets, Buses

SKiDL uses four types of objects to represent a circuit: Part, Pin, Net, and Bus.

The Part object represents an electronic component, which SKiDL thinks of as simple bags of Pin objects with a few other attributes attached (like the part number, name, reference, value, footprint, etc.).

The Pin object represents a terminal that brings an electronic signal into and out of the part. Each Pin object has two important attributes:

part which stores the reference to the Part object to which the pin belongs.
net which stores the the reference to the Net object that the pin is connected to, or None if the pin is unconnected.

A Net object is kind of like a Part: it's a simple bag of pins. The difference is, unlike a part, pins can be added to a net. This happens when a pin on some part is connected to the net or when the net is merged with another net.

Finally, a Bus is just a list of Net objects. A bus of a certain width can be created from a number of existing nets, newly-created nets, or both.

Creating SKiDL Objects

Here's the most common way to create a part in your circuit:

my_part = Part('some_library', 'some_part_name')

When this is processed, the current directory will be checked for a file called some_library.lib which will be opened and scanned for a part with the name some_part_name. If the file is not found or it doesn't contain the requested part, then the process will be repeated using KiCad's default library directory. (You can change SKiDL's library search by changing the list of directories stored in the skidl.lib_search_paths_kicad list.)

You're not restricted to using only the current directory or the KiCad default directory to search for parts. You can also search any file for a part by using a full file name:

my_part = Part('C:/my_libs/my_great_parts.lib', 'my_super_regulator')

You're also not restricted to getting an exact match on the part name: you can use a regular expression instead. For example, this will find a part with "358" anywhere in a part name or alias:

my_part = Part('some_library', '.*358.*')

If the regular expression matches more than one part, then you'll only get the first match and a warning that multiple parts were found.

Once you have a part, you can set its attributes like you could for any Python object. As was shown previously, the ref attribute will already be set but you can override it:

my_part.ref = 'U5'

In addition, the value and footprint attributes are required for generating a netlist. You can also add any other attribute:

my_part.manf = 'Atmel'
my_part.setattr('manf#', 'ATTINY4-TSHR')

It's also possible to set the attributes during the part creation:

my_part = Part('some_lib', 'some_part', ref='U5', footprint='Package_TO_SOT_SMD.pretty:SOT-23-6', manf='Atmel')

Creating nets is also simple:

my_net = Net()              # An unnamed net.
my_other_net = Net('Fred')  # A named net.

As with parts, SKiDL will alter the name you assign to a net if it collides with another net having the same name.

You can create a bus of a certain width like this:

my_bus = Bus('bus_name', 8)  # Create a byte-wide bus.

(All buses must be named, but SKiDL will look for and correct colliding bus names.)

You can also create a bus from existing nets, or buses, or the pins of parts:

my_part = Part('linear', 'LM358')
a_net = Net()
b_net = Net()
bus_nets = Bus('net_bus', a_net, b_net)            # A 2-bit bus.
bus_pins = Bus('pin_bus', my_part[1], my_part[3])  # A 2-bit bus.
bus_buses = Bus('bus_bus', my_bus)                 # An 8-bit bus.

Finally, you can mix-and-match any combination of widths, nets, buses or part pins:

bus_mixed = Bus('mongrel', 8, a_net, my_bus, my_part[2])  # 8+1+8+1 = 18-bit bus.

Finally, you can modify an existing bus by inserting or extending it with any combination of widths, nets, buses or pins:

bus = Bus('A', 8)   # Eight-bit bus.
bus.insert(4, Bus('I', 3))  # Insert 3-bit bus before bus line bus[4].
bus.extend(5, Pin(), Net()) # Extend bus with another 5-bit bus, a pin, and a net.

The final object you can create is a Pin. You'll probably never do this (except in interactive sessions), and it's probably a mistake if you ever do do it, but here's how to do it:

>>> p = Pin(num=1, name='my_pin', func=Pin.TRISTATE)
>>> p
Pin ???/1/my_pin/TRISTATE

Finding SKiDL Objects

Sometimes you may want to access a bus, net, or part that's already been created. In such an instance, you can use the get() class method:

n = Net.get('Fred')  # Find the existing Net object named 'Fred'.
b = Bus.get('A')     # Find the existing Bus object named 'A'.
p = Part.get('AS6C1616')  # Find all parts with this part name.

If a net or bus is found with the exact name that was given, then that SKiDL object is returned (no wild-card searches using regular expressions are allowed). If the search is unsuccessful, None is returned.

For parts, the search is performed using string matching on part names, references (e.g., R4), and aliases. In addition, regular expression matching is used to search within the part descriptions, so you could search for all parts with "ram" in their description.

There may be other times when you want to access a particular bus or net and, if it doesn't exist, then create it (this is not possible with parts). The fetch() class method is used for this:

n = Net.fetch('Fred')  # Find the existing Net object named 'Fred' or create it if not found.
b = Bus.fetch('A', 8)  # Find the existing Bus object named 'A' or create it if not found.

Note that with the Bus.fetch() method, you also have to provide the arguments to build the bus (such as its width) in case it doesn't exist.

Copying SKiDL Objects

Instead of creating a SKiDL object from scratch, sometimes it's easier to just copy an existing object. Here are some examples of creating a resistor and then making some copies of it:

>>> r1 = Part("Device", 'R', value=500)
>>> r2 = r1.copy()                         # Make a single copy of the resistor.
>>> r2_lst = r1.copy(1)                    # Make a single copy, but return it in a list.
>>> r3 = r1.copy(value='1K')               # Make a single copy, but give it a different value.
>>> r4 = r1(value='1K')                    # You can also call the object directly to make copies.
>>> r5, r6, r7 = r1(3)                     # Make 3 copies of the resistor.
>>> r8, r9, r10 = r1(value=[110,220,330])  # Make 3 copies, each with a different value.
>>> r11, r12 = 2 * r1                      # Make copies using the '*' operator.

In some cases it's clearer to create parts by copying a template part that doesn't actually get included in the netlist for the circuitry. This is done like so:

>>> r_template = Part("Device", 'R', dest=TEMPLATE)  # Create a resistor just for copying.
>>> r1 = r_template(value='1K')  # Make copy that becomes part of the actual circuitry.

Accessing Part Pins and Bus Lines

Accessing Part Pins

You can access the pins on a part or the individual nets of a bus using numbers, slices, strings, and regular expressions, either singly or in any combination.

Suppose you have a PIC10 processor in a six-pin package:

>>> pic10 = Part('microchip_pic10mcu', 'pic10f220-i/ot')
>>> pic10

PIC10F220-I/OT: PIC10F222, 512W Flash, 24B SRAM, SOT-23-6
    Pin U1/1/ICSPDAT/AN0/GP0/BIDIRECTIONAL
    Pin U1/2/VSS/POWER-IN
    Pin U1/3/ICSPCLK/AN1/GP1/BIDIRECTIONAL
    Pin U1/4/T0CKI/FOSC4/GP2/BIDIRECTIONAL
    Pin U1/5/VDD/POWER-IN
    Pin U1/6/Vpp/~MCLR~/GP3/INPUT

The most natural way to access one of its pins is to give the pin number in brackets:

>>> pic10[3]
Pin U1/3/ICSPCLK/AN1/GP1/BIDIRECTIONAL

(If you have a part in a BGA package with pins numbers like C11, then you'll have to enter the pin number as a quoted string like 'C11'.)

You can also get several pins at once in a list:

>>> pic10[3,1,6]
[Pin U1/3/ICSPCLK/AN1/GP1/BIDIRECTIONAL, Pin U1/1/ICSPDAT/AN0/GP0/BIDIRECTIONAL, Pin U1/6/Vpp/~MCLR~/GP3/INPUT]

You can even use Python slice notation:

>>> pic10[2:4]  # Get pins 2 through 4.
[Pin U1/2/VSS/POWER-IN, Pin U1/3/ICSPCLK/AN1/GP1/BIDIRECTIONAL, Pin U1/4/T0CKI/FOSC4/GP2/BIDIRECTIONAL]
>>> pic10[4:2]  # Get pins 4 through 2.
[Pin U1/4/T0CKI/FOSC4/GP2/BIDIRECTIONAL, Pin U1/3/ICSPCLK/AN1/GP1/BIDIRECTIONAL, Pin U1/2/VSS/POWER-IN]
>>> pic10[:]    # Get all the pins.
[Pin U1/1/ICSPDAT/AN0/GP0/BIDIRECTIONAL, Pin U1/2/VSS/POWER-IN, Pin U1/3/ICSPCLK/AN1/GP1/BIDIRECTIONAL, Pin U1/4/T0CKI/FOSC4/GP2/BIDIRECTIONAL, Pin U1/5/VDD/POWER-IN, Pin U1/6/Vpp/~MCLR~/GP3/INPUT]

(It's important to note that the slice notation used by SKiDL for parts is slightly different than standard Python. In Python, a slice n:m would fetch indices n, n+1, ..., m-1. With SKiDL, it actually fetches all the way up to the last number: n, n+1, ..., m-1, m. The reason for doing this is that most electronics designers are used to the bounds on a slice including both endpoints. Perhaps it is a mistake to do it this way. We'll see...)

In addition to the bracket notation, you can also get a single pin using an attribute name that begins with a 'p' followed by the pin number:

>>> pic10.p2
Pin U1/2/VSS/POWER-IN

Instead of pin numbers, sometimes it makes the design intent more clear to access pins by their names. For example, it's more obvious that a voltage supply net is being attached to the power pin of the processor when it's expressed like this:

pic10['VDD'] += supply_5V

Like pin numbers, pin names can also be used as attributes to access the pin:

>>> pic10.VDD
Pin U1/5/VDD/POWER-IN

You can use multiple names or regular expressions to get more than one pin:

>>> pic10['VDD','VSS']
[Pin U1/5/VDD/POWER-IN, Pin U1/2/VSS/POWER-IN]
>>> pic10['.*gp[1-3]']
[Pin U1/3/ICSPCLK/AN1/GP1/BIDIRECTIONAL, Pin U1/4/T0CKI/FOSC4/GP2/BIDIRECTIONAL, Pin U1/6/Vpp/~MCLR~/GP3/INPUT]

It can be tedious and error prone entering all the quote marks if you're accessing many pin names. SKiDL lets you enter a single, comma-delimited string of pin names:

>>> pic10['.*GP0, .*GP1, .*GP2']
[Pin U1/1/ICSPDAT/AN0/GP0/BIDIRECTIONAL, Pin U1/3/ICSPCLK/AN1/GP1/BIDIRECTIONAL, Pin U1/4/T0CKI/FOSC4/GP2/BIDIRECTIONAL]

Some parts have sequentially-numbered sets of pins like the address and data buses of a RAM. SKiDL lets you access these pins using a slice-like notation in a string like so:

>>> ram = Part('memory', 'sram_512ko')
>>> ram['D[0:7]']
[Pin U1/13/D0/TRISTATE, Pin U1/14/D1/TRISTATE, Pin U1/15/D2/TRISTATE, Pin U1/17/D3/TRISTATE, Pin U1/18/D4/TRISTATE, Pin U1/19/D5/TRISTATE, Pin U1/20/D6/TRISTATE, Pin U1/21/D7/TRISTATE]

Or you can access the pins in the reverse order:

>>> ram = Part('memory', 'sram_512ko')
>>> ram['D[7:0]']
[Pin U2/21/D7/TRISTATE, Pin U2/20/D6/TRISTATE, Pin U2/19/D5/TRISTATE, Pin U2/18/D4/TRISTATE, Pin U2/17/D3/TRISTATE, Pin U2/15/D2/TRISTATE, Pin U2/14/D1/TRISTATE, Pin U2/13/D0/TRISTATE]

Part objects also provide the get_pins() function which can select pins in even more ways. For example, this would get every bidirectional pin of the processor:

>>> pic10.get_pins(func=Pin.BIDIR)
[Pin U1/1/ICSPDAT/AN0/GP0/BIDIRECTIONAL, Pin U1/3/ICSPCLK/AN1/GP1/BIDIRECTIONAL, Pin U1/4/T0CKI/FOSC4/GP2/BIDIRECTIONAL]

Since you can access part pins by number or by name using strings or regular expressions, it's worth discussing how SKiDL decides which one to select. When given a pin index, SKiDL prioritizes the search for the corresponding pins like so:

If one or more pin numbers match the index, then those pins are returned and the search stops.
If one or more pin names match the index using standard string matching, then those pins are returned and the search stops.
If one or more pin aliases match the index using standard string matching, then those pins are returned and the search stops.
If one or more pin names match the index using it as a regular expression, then those pins are returned and the search stops.
If one or more pin aliases match the index using it as a regular expression, then those pins are returned and the search stops.

It should also be mentioned that when using the index as a regular expression, SKiDL surrounds it with .* so it will match anywhere within a pin name or alias. Hence, if an index of D1 did not exactly match any pin number, name or alias, then it would become .*D1.* and would match any pin with D1 in its name. You can stop this by placing start and end characters in the index like so: ^D1$ will match only D1.

Finally, since SKiDL prioritizes pin number matches over name matches, what happens when you want to use a pin whose name is the same as the pin number of another pin? For example, a memory chip in a BGA would have pin numbers A1, A2, A3, ... but might also have other pins used for addresses named A1, A2, A3, ... . SKiDL provides the p and n part attributes so you can specifically target either pin numbers or names:

ram['A1, A2, A3']    # Selects pin numbers A1, A2 and A3 if the part is a BGA.
ram.p['A1, A2, A3']  # Use the p attribute to specifically select pin numbers A1, A2 and A3.
ram.n['A1, A2, A3']  # Use the n attribute to specifically select pin names A1, A2 and A3.

If you want to access part pins algorithmically in a loop, it can be done as follows:

for p in pic10.get_pins():
  <do something with p>

The same thing could also be done using a Part object as an iterator:

for p in pic10:
  <do something with p>

Accessing Bus Lines

Accessing the individual lines of a bus works similarly to accessing part pins:

>>> a = Net('NET_A')  # Create a named net.
>>> b = Bus('BUS_B', 8, a)  # Create a nine-bit bus.
>>> b
BUS_B:
        BUS_B0:  # Note how the individual lines of the bus are named.
        BUS_B1:
        BUS_B2:
        BUS_B3:
        BUS_B4:
        BUS_B5:
        BUS_B6:
        BUS_B7:
        NET_A:   # The last net retains its original name.

>>> b[0]  # Get the first line of the bus.
BUS_B0:

>>> b[4,8]  # Get the fifth and ninth bus lines.
[BUS_B4: , NET_A: ]

>>> b[3:0]  # Get the first four bus lines in reverse order.
[BUS_B3: , BUS_B2: , BUS_B1: , BUS_B0: ]

>>> b['BUS_B.*']  # Get all the bus lines except the last one.
[BUS_B0: , BUS_B1: , BUS_B2: , BUS_B3: , BUS_B4: , BUS_B5: , BUS_B6: , BUS_B7: ]

>>> b['NET_A']  # Get the last bus line.
NET_A:

>>> for line in b:  # Access lines in bus using bus as an iterator.
...:    print(line)
...:
BUS_B0:
BUS_B1:
BUS_B2:
BUS_B3:
BUS_B4:
BUS_B5:
BUS_B6:
BUS_B7:
NET_A:

Making Connections

Pins, nets, parts and buses can all be connected together in various ways, but the primary rule of SKiDL connections is:

The += operator is the only way to make connections!

At times you'll mistakenly try to make connections using the assignment operator (=). In many cases, SKiDL warns you if you do that, but there are situations where it can't (because Python is a general-purpose programming language where assignment is a necessary operation). So remember the primary rule!

After the primary rule, the next thing to remember is that SKiDL's main purpose is creating netlists. To that end, it handles four basic, connection operations:

Pin-to-Net: A pin is connected to a net, adding it to the list of pins connected to that net. If the pin is already attached to other nets, then those nets are connected to this net as well.

Net-to-Pin: This is the same as doing a pin-to-net connection.

Pin-to-Pin: A net is created and both pins are attached to it. If one or both pins are already connected to other nets, then those nets are connected to the newly-created net as well.

Net-to-Net: Connecting one net to another merges the pins on both nets onto a single, larger net.

For each type of connection operation, there are three variants based on the number of things being connected:

One-to-One: This is the most frequent type of connection, for example, connecting one pin to another or connecting a pin to a net.

One-to-Many: This mainly occurs when multiple pins are connected to the same net, like when multiple ground pins of a chip are connected to the circuit ground net.

Many-to-Many: This usually involves bus connections to a part, such as connecting a bus to the data or address pins of a processor. For this variant, there must be the same number of things to connect in each set, e.g. you can't connect three pins to four nets.

As a first example, let's connect a net to a pin on a part:

>>> pic10 = Part('microchip_pic10mcu','pic10f220-i/ot')  # Get a part.
>>> io = Net('IO_NET')    # Create a net.
>>> pic10['.*GP0'] += io  # Connect the net to a part pin.
>>> io                    # Show the pins connected to the net.
IO_NET: Pin U1/1/ICSPDAT/AN0/GP0/BIDIRECTIONAL

You can do the same operation in reverse by connecting the part pin to the net with the same result:

>>> pic10 = Part('microchip_pic10mcu','pic10f220-i/ot')
>>> io = Net('IO_NET')
>>> io += pic10['.*GP0']  # Connect a part pin to the net.
>>> io
IO_NET: Pin U1/1/ICSPDAT/AN0/GP0/BIDIRECTIONAL

You can also connect a pin directly to another pin. In this case, an implicit net will be created between the pins that you can access using the net attribute of either part pin:

>>> pic10['.*GP1'] += pic10['.*GP2']  # Connect two pins together.
>>> pic10['.*GP1'].net     # Show the net connected to the pin.
N$1: Pin U1/3/ICSPCLK/AN1/GP1/BIDIRECTIONAL, Pin U1/4/T0CKI/FOSC4/GP2/BIDIRECTIONAL
>>> pic10['.*GP2'].net     # Show the net connected to the other pin. Same thing!
N$1: Pin U1/3/ICSPCLK/AN1/GP1/BIDIRECTIONAL, Pin U1/4/T0CKI/FOSC4/GP2/BIDIRECTIONAL

You can connect multiple pins together, all at once:

>>> pic10[1] += pic10[2,3,6]
>>> pic10[1].net
N$1: Pin U1/1/ICSPDAT/AN0/GP0/BIDIRECTIONAL, Pin U1/2/VSS/POWER-IN, Pin U1/3/ICSPCLK/AN1/GP1/BIDIRECTIONAL, Pin U1/6/Vpp/~MCLR~/GP3/INPUT

Or you can do it incrementally:

>>> pic10[1] += pic10[2]
>>> pic10[1] += pic10[3]
>>> pic10[1] += pic10[6]
>>> pic10[1].net
N$1: Pin U1/1/ICSPDAT/AN0/GP0/BIDIRECTIONAL, Pin U1/2/VSS/POWER-IN, Pin U1/3/ICSPCLK/AN1/GP1/BIDIRECTIONAL, Pin U1/6/Vpp/~MCLR~/GP3/INPUT

If you connect pins on separate nets together, then all the pins are merged onto the same net:

>>> pic10[1] += pic10[2]  # Put pins 1 & 2 on one net.
>>> pic10[1].net
N$1: Pin U1/1/ICSPDAT/AN0/GP0/BIDIRECTIONAL, Pin U1/2/VSS/POWER-IN
>>> pic10[3] += pic10[4]  # Put pins 3 & 4 on another net.
>>> pic10[3].net
N$2: Pin U1/3/ICSPCLK/AN1/GP1/BIDIRECTIONAL, Pin U1/4/T0CKI/FOSC4/GP2/BIDIRECTIONAL
>>> pic10[1] += pic10[4]  # Connect two pins from different nets.
>>> pic10[3].net          # Now all the pins are on the same net!
N$2: Pin U1/1/ICSPDAT/AN0/GP0/BIDIRECTIONAL, Pin U1/2/VSS/POWER-IN, Pin U1/3/ICSPCLK/AN1/GP1/BIDIRECTIONAL, Pin U1/4/T0CKI/FOSC4/GP2/BIDIRECTIONAL

Here's an example of connecting a three-bit bus to three pins on a part:

>>> pic10 = Part('microchip_pic10mcu','pic10f220-i/ot')
>>> pic10

PIC10F220-I/OT: PIC10F222, 512W Flash, 24B SRAM, SOT-23-6
    Pin U1/1/ICSPDAT/AN0/GP0/BIDIRECTIONAL
    Pin U1/2/VSS/POWER-IN
    Pin U1/3/ICSPCLK/AN1/GP1/BIDIRECTIONAL
    Pin U1/4/T0CKI/FOSC4/GP2/BIDIRECTIONAL
    Pin U1/5/VDD/POWER-IN
    Pin U1/6/Vpp/~MCLR~/GP3/INPUT
>>> b = Bus('GP', 3)        # Create a 3-bit bus.
>>> pic10[4,3,1] += b[2:0]  # Connect bus to part pins, one-to-one.
>>> b
GP:
        GP0: Pin U1/1/ICSPDAT/AN0/GP0/BIDIRECTIONAL
        GP1: Pin U1/3/ICSPCLK/AN1/GP1/BIDIRECTIONAL
        GP2: Pin U1/4/T0CKI/FOSC4/GP2/BIDIRECTIONAL

But SKiDL will warn you if there aren't the same number of things to connect on each side:

>>> pic10[4,3,1] += b[1:0]  # Too few bus lines for the pins!
ERROR: Connection mismatch 3 != 2!
Traceback (most recent call last):
  File "<stdin>", line 1, in <module>
  File "c:\xesscorp\kicad\tools\skidl\skidl\skidl.py", line 3330, in __iadd__
    raise Exception
Exception

Making Parallel and Serial Networks

The previous section showed some general-purpose techniques for connecting parts, but SKiDL also has some specialized syntax for wiring two-pin components in parallel or serial. For example, here is a network of four resistors connected in series between power and ground:

vcc, gnd = Net('VCC'), Net('GND')
r1, r2, r3, r4 = Part("Device", 'R', dest=TEMPLATE) * 4
ser_ntwk = vcc & r1 & r2 & r3 & r4 & gnd

It's also possible to connect the resistors in parallel between power and ground:

par_ntwk = vcc & (r1 | r2 | r3 | r4) & gnd

Or you can do something like placing pairs of resistors in series and then paralleling those combinations like this:

combo_ntwk = vcc & ((r1 & r2) | (r3 & r4)) & gnd

The examples above work with non-polarized components, but what about parts like diodes? In that case, you have to specify the pins explicitly with the first pin connected to the preceding part and the second pin to the following part:

d1 = Part("Device", 'D')
polar_ntwk = vcc & r1 & d1['A,K'] & gnd  # Diode anode connected to resistor and cathode to ground.

Explicitly listing the pins also lets you use multi-pin parts with networks. For example, here's an NPN-transistor amplifier:

q1 = Part("Device", 'Q_NPN_ECB')
ntwk_ce = vcc & r1 & q1['C,E'] & gnd  # VCC through load resistor to collector and emitter attached to ground.
ntwk_b = r2 & q1['B']  # Resistor attached to base.

That's all well and good, but how do you connect to internal points in these networks where the interesting things are happening? For instance, how do you apply an input to the transistor circuit and then connect to the output? One way is by inserting nets inside the networks:

inp, outp = Net('INPUT'), Net('OUTPUT')
ntwk_ce = vcc & r1 & outp & q1['C,E'] & gnd  # Connect net outp to the junction of the resistor and transistor collector.
ntwk_b = inp & r2 & q1['B']  # Connect net inp to the resistor driving the transistor base.

After that's done, the inp and outp nets can be connected to other points in the circuit.

Aliases

Aliases let you assign a more descriptive name to a part, pin, net, or bus without affecting the original name. This is probably most useful in assigning names to pins to describe their functions.

r = Part("Device", 'R')
r[1] += vcc  # Connect one end of resistor to VCC net.
r[2].aliases += "pullup"  # Add the alias "pullup" to the other end of the resistor.

uc['RESET'] += r['pullup']  # Connect the pullup resistor to the reset pin of a microcontroller.

To see the assigned aliases, just use the aliases attribute:

>>> r = Part("Device", 'R')
>>> r.aliases += "resistor"
>>> r.aliases += "pullup resistor"
>>> r.aliases

{'pullup resistor', 'resistor'}

Units Within Parts

Some components may contain smaller units that operate independently of the component as a whole. For example, an operational amplifier chip might contain two individual opamp units, each capable of operating on their own set of inputs and outputs.

Some library parts may already have predefined units, but you can add them to any part. For example, a four-pin resistor network might contain two resistors: one attached between pins 1 and 4, and the other bewtween pins 2 and 3. Each resistor could be assigned to a unit as follows:

>>> rn = Part("Device", 'R_Pack02')
>>> rn.make_unit('A', 1, 4)  # Make a unit called 'A' for the first resistor.

 R_Pack02 (): 2 Resistor network, parallel topology, DIP package
    Pin RN1/4/R1.2/PASSIVE
    Pin RN1/1/R1.1/PASSIVE

>>> rn.make_unit('B', 2, 3)  # Now make a unit called 'B' for the second resistor.

 R_Pack02 (): 2 Resistor network, parallel topology, DIP package
    Pin RN1/2/R2.1/PASSIVE
    Pin RN1/3/R2.2/PASSIVE

Once the units are defined, you can use them just like any part:

>>> rn.unit['A'][1,4] += Net(), Net()  # Connect resistor A to two nets.
>>> rn.unit['B'][2,3] += rn.unit['A'][1,4]  # Connect resistor B in parallel with resistor A.

Now this isn't all that useful because you still have to remember which pins are assigned to each unit, and if you wanted to swap the resistors you would have to change the unit names and the pins numbers!. In order to get around this inconvenience, you could assign aliases to each pin like this:

>>> rn[1].aliases += 'L' # Alias 'L' of pin 1 on left-side of package.
>>> rn[4].aliases += 'R' # Alias 'R' of pin 4 on right-side of package.
>>> rn[2].aliases += 'L' # Alias 'L' of pin 2 on left-side.
>>> rn[3].aliases += 'R' # Alias 'R' of pin 3 on right-side.

Now the same connections can be made using the pin aliases:

>>> rn.unit['A']['L,R'] += Net(), Net()  # Connect resistor A to two nets.
>>> rn.unit['B']['L,R'] += rn.unit['A']['L,R']  # Connect resistor B in parallel with resistor A.

In this case, if you wanted to swap the A and B resistors, you only need to change their unit labels. The pin aliases don't need to be altered.

If you find the unit[...] notation cumbersome, units can also be accessed by using their names as attributes:

>>> rn.A['L,R'] += Net(), Net()  # Connect resistor A to two nets.
>>> rn.B['L,R'] += rn.A['L,R']   # Connect resistor B in parallel with resistor A.

Part Fields

Parts typically have field that store additional information such as manufacturer identifiers. Every Part object stores this information in a dictionary called fields:

>> lm35 = Part('Sensor_Temperature', 'LM35-D')
>> lm35.fields

{'F0': 'U',
 'F1': 'LM35-D',
 'F2': 'Package_SO:SOIC-8_3.9x4.9mm_P1.27mm',
 'F3': ''}

>>> lm35.fields['F1']

'LM35-D'

Fields can also be accessed as attributes of the part:

>>> lm35.F1

'LM35-D'

New fields can be added just by adding new keys and values to the fields dictionary.

Hierarchy

SKiDL supports the encapsulation of parts, nets and buses into modules that can be replicated to reduce the design effort, and can be used in other modules to create a functional hierarchy. It does this using Python's built-in machinery for defining and calling functions so there's almost nothing new to learn.

As an example, here's the voltage divider as a module:

from skidl import *
import sys

# Define the voltage divider module. The @subcircuit decorator 
# handles some skidl housekeeping that needs to be done.
@subcircuit
def vdiv(inp, outp):
    """Divide inp voltage by 3 and place it on outp net."""
    rup = Part("Device", 'R', value='1K', footprint='Resistor_SMD.pretty:R_0805_2012Metric')
    rlo = Part("Device",'R', value='500', footprint='Resistor_SMD.pretty:R_0805_2012Metric')
    rup[1,2] += inp, outp
    rlo[1,2] += outp, gnd

gnd = Net('GND')         # GLobal ground net.
input_net = Net('IN')    # Net with the voltage to be divided.
output_net = Net('OUT')  # Net with the divided voltage.

# Instantiate the voltage divider and connect it to the input & output nets.
vdiv(input_net, output_net)

generate_netlist(sys.stdout)

For the most part, vdiv is just a standard Python function: it accepts inputs, it performs operations on them, and it could return outputs (but in this case, it doesn't need to). Other than the @subcircuit decorator that appears before the function definition, vdiv is just a Python function and it can do anything that a Python function can do.

Here's the netlist that's generated:

(export (version D)
  (design
    (source "C:\TEMP\skidl tests\hier_example.py")
    (date "04/20/2017 09:39 AM")
    (tool "SKiDL (0.0.12)"))
  (components
    (comp (ref R1)
      (value 1K)
      (footprint Resistor_SMD.pretty:R_0805_2012Metric)
      (fields
        (field (name keywords) "r res resistor")
        (field (name description) Resistor))
      (libsource (lib device) (part R)))
    (comp (ref R2)
      (value 500)
      (footprint Resistor_SMD.pretty:R_0805_2012Metric)
      (fields
        (field (name keywords) "r res resistor")
        (field (name description) Resistor))
      (libsource (lib device) (part R))))
  (nets
    (net (code 0) (name GND)
      (node (ref R2) (pin 2)))
    (net (code 1) (name IN)
      (node (ref R1) (pin 1)))
    (net (code 2) (name OUT)
      (node (ref R1) (pin 2))
      (node (ref R2) (pin 1))))
)

For an example of a multi-level hierarchy, the multi_vdiv module shown below can use the vdiv module to divide a voltage multiple times:

from skidl import *
import sys

# Define the voltage divider module.
@subcircuit
def vdiv(inp, outp):
    """Divide inp voltage by 3 and place it on outp net."""
    rup = Part("Device", 'R', value='1K', footprint='Resistor_SMD.pretty:R_0805_2012Metric')
    rlo = Part("Device",'R', value='500', footprint='Resistor_SMD.pretty:R_0805_2012Metric')
    rup[1,2] += inp, outp
    rlo[1,2] += outp, gnd

@subcircuit
def multi_vdiv(repeat, inp, outp):
    """Divide inp voltage by 3 ** repeat and place it on outp net."""
    for _ in range(repeat):
        out_net = Net()     # Create an output net for the current stage.
        vdiv(inp, out_net)  # Instantiate a divider stage.
        inp = out_net       # The output net becomes the input net for the next stage.
    outp += out_net         # Connect the output from the last stage to the module output net.

gnd = Net('GND')         # GLobal ground net.
input_net = Net('IN')    # Net with the voltage to be divided.
output_net = Net('OUT')  # Net with the divided voltage.
multi_vdiv(3, input_net, output_net)  # Run the input through 3 voltage dividers.

generate_netlist(sys.stdout)

(For the EE's out there: yes, I know cascading three simple voltage dividers will not multiplicatively scale the input voltage because of the input and output impedances of each stage! It's just the simplest example I could use to show hierarchy.)

And here's the resulting netlist:

(export (version D)
  (design
    (source "C:\TEMP\skidl tests\multi_hier_example.py")
    (date "04/20/2017 09:43 AM")
    (tool "SKiDL (0.0.12)"))
  (components
    (comp (ref R1)
      (value 1K)
      (footprint Resistor_SMD.pretty:R_0805_2012Metric)
      (fields
        (field (name keywords) "r res resistor")
        (field (name description) Resistor))
      (libsource (lib device) (part R)))
    (comp (ref R2)
      (value 500)
      (footprint Resistor_SMD.pretty:R_0805_2012Metric)
      (fields
        (field (name keywords) "r res resistor")
        (field (name description) Resistor))
      (libsource (lib device) (part R)))
    (comp (ref R3)
      (value 1K)
      (footprint Resistor_SMD.pretty:R_0805_2012Metric)
      (fields
        (field (name keywords) "r res resistor")
        (field (name description) Resistor))
      (libsource (lib device) (part R)))
    (comp (ref R4)
      (value 500)
      (footprint Resistor_SMD.pretty:R_0805_2012Metric)
      (fields
        (field (name keywords) "r res resistor")
        (field (name description) Resistor))
      (libsource (lib device) (part R)))
    (comp (ref R5)
      (value 1K)
      (footprint Resistor_SMD.pretty:R_0805_2012Metric)
      (fields
        (field (name keywords) "r res resistor")
        (field (name description) Resistor))
      (libsource (lib device) (part R)))
    (comp (ref R6)
      (value 500)
      (footprint Resistor_SMD.pretty:R_0805_2012Metric)
      (fields
        (field (name keywords) "r res resistor")
        (field (name description) Resistor))
      (libsource (lib device) (part R))))
  (nets
    (net (code 0) (name GND)
      (node (ref R2) (pin 2))
      (node (ref R4) (pin 2))
      (node (ref R6) (pin 2)))
    (net (code 1) (name IN)
      (node (ref R1) (pin 1)))
    (net (code 2) (name N$1)
      (node (ref R1) (pin 2))
      (node (ref R2) (pin 1))
      (node (ref R3) (pin 1)))
    (net (code 3) (name N$2)
      (node (ref R3) (pin 2))
      (node (ref R4) (pin 1))
      (node (ref R5) (pin 1)))
    (net (code 4) (name OUT)
      (node (ref R5) (pin 2))
      (node (ref R6) (pin 1))))
)

Interfaces

Passing nets between hierarchically-organized modules can lead to long lists of arguments. To make the code easier to write and understand, SKiDL supports interfaces which are simply containers that encapsulate a number of Bus, Net, or Pin objects. For example, here is an interface for a memory:

mem_intfc = Interface(
  rd = Net('MEM_RD#'),
  wr = Net('MEM_WR#'),
  addr = Bus('MEM_ADDR', 20),
  data = Bus('MEM_DATA', 16)
)

Then this interface can be passed to a module that implements a RAM memory and a microcontroller that uses it:

mem_module(mem_intfc)
uc_module(clk, mem_intfc, io_intfc)

Inside the mem_module, the interface signals are connected to a RAM chip:

@subcircuit
def mem_module(intfc):
  ram = Part('Memory_RAM', 'AS6C1616')
  ram['A[0:19]'] += intfc.addr
  ram['DQ[0:15]'] += intfc.data
  ram['WE#'] += intfc.wr
  ram['OE#'] += intfc.rd
  ...

Libraries

As you've already seen, SKiDL gets its parts from part libraries. By default, SKiDL finds the libraries provided by KiCad (using the KICAD_SYMBOL_DIR environment variable), so if that's all you need then you're all set.

Currently, SKiDL supports the library formats for the following ECAD tools:

KICAD: KiCad schematic part libraries.
SKIDL: Schematic parts stored as SKiDL/Python modules.

You can set the default library format you want to use in your SKiDL script like so:

set_default_tool(KICAD)  # KiCad is the default library format.
set_default_tool(SKIDL)  # Now SKiDL is the default library format.

You can select the directories where SKiDL looks for parts using the lib_search_paths dictionary:

lib_search_paths[SKIDL] = ['.', '..', 'C:\\temp']
lib_search_paths[KICAD].append('C:\\my\\kicad\\libs')

You can convert a KiCad library into the SKiDL format by exporting it:

kicad_lib = SchLib("Device", tool=KICAD)       # Open a KiCad library.
kicad_lib.export('my_skidl_lib')               # Export it into a file in SKiDL format.
skidl_lib = SchLib('my_skidl_lib', tool=SKIDL) # Create a SKiDL library object from the new file.
if len(skidl_lib) == len(kicad_lib):
    print('As expected, both libraries have the same number of parts!')
else:
    print('Something went wrong!')
diode = Part(skidl_lib, 'D')                   # Instantiate a diode from the SKiDL library.

You can make ad-hoc libraries just by creating a SchLib object and adding Part objects to it:

my_lib = SchLib(name='my_lib')                      # Create an empty library object.
my_part = Part(name='R', tool=SKIDL, dest=TEMPLATE) # Create an empty part object template.
my_part.ref_prefix = 'R'                            # Set the part reference prefix.
my_part.description = 'resistor'                    # Set the part's description field.
my_part.keywords = 'res resistor'                   # Set the part's keywords.
my_part += Pin(num=1, func=Pin.PASSIVE)             # Add a pin to the part.
my_part += Pin(num=2, func=Pin.PASSIVE)             # Add another pin to the part.
my_lib += my_part                                   # Add the part to the library.

new_resistor = Part(my_lib, 'R')                    # Instantiate the part from the library.
my_lib.export('my_lib')                             # Save the library in a file my_lib.py.

Always create a part intended for a library as a template so you don't inadvertently add it to the circuit netlist. Then set the part attributes and create and add pins to the part. Here are the most common attributes you'll want to set:

Attribute	Meaning
name	A string containing the name of the part, e.g. 'LM35' for a temperature sensor.
ref_prefix	A string containing the prefix for this part's references, e.g. 'U' for ICs.
description	A string describing the part, e.g. 'temperature sensor'.
keywords	A string containing keywords about the part, e.g. 'sensor temperature IC'.

When creating a pin, these are the attributes you'll want to set:

Attribute	Meaning
num	A string or integer containing the pin number, e.g. 5 or 'A13'.
name	A string containing the name of the pin, e.g. 'CS'.
func	An identifier for the function of the pin.

The pin function identifiers are as follows:

Identifier	Pin Function
Pin.INPUT	Input pin.
Pin.OUTPUT	Output pin.
Pin.BIDIR	Bidirectional in/out pin.
Pin.TRISTATE	Output pin that goes into a high-impedance state when disabled.
Pin.PASSIVE	Pin on a passive component (like a resistor).
Pin.UNSPEC	Pin with an unspecified function.
Pin.PWRIN	Power input pin (either voltage supply or ground).
Pin.PWROUT	Power output pin (like the output of a voltage regulator).
Pin.OPENCOLL	Open-collector pin (pulls to ground but not to positive rail).
Pin.OPENEMIT	Open-emitter pin (pulls to positive rail but not to ground).
Pin.NOCONNECT	A pin that should be left unconnected.

SKiDL will also create a library of all the parts used in your design whenever you use the generate_netlist() function. For example, if your SKiDL script is named my_design.py, then the parts instantiated in that script will be stored as a SKiDL library in the file my_design_lib.py. This can be useful if you're sending the design to someone who may not have all the libraries you do. Just send them my_design.py and my_design_lib.py and any parts not found when they run the script will be fetched from the backup parts in the library.

Doodads

SKiDL has a few features that don't fit into any other category. Here they are.

No Connects

Sometimes you will use a part, but you won't use every pin. The ERC will complain about those unconnected pins:

>>> pic10 = Part('microchip_pic10mcu','pic10f220-i/ot')
>>> ERC()
ERC WARNING: Unconnected pin: BIDIRECTIONAL pin 1/ICSPDAT/AN0/GP0 of PIC10F220-I/OT/U1.
ERC WARNING: Unconnected pin: POWER-IN pin 2/VSS of PIC10F220-I/OT/U1.
ERC WARNING: Unconnected pin: BIDIRECTIONAL pin 3/ICSPCLK/AN1/GP1 of PIC10F220-I/OT/U1.
ERC WARNING: Unconnected pin: BIDIRECTIONAL pin 4/T0CKI/FOSC4/GP2 of PIC10F220-I/OT/U1.
ERC WARNING: Unconnected pin: POWER-IN pin 5/VDD of PIC10F220-I/OT/U1.
ERC WARNING: Unconnected pin: INPUT pin 6/Vpp/~MCLR~/GP3 of PIC10F220-I/OT/U1.

6 warnings found during ERC.
0 errors found during ERC.

If you have pins that you intentionally want to leave unconnected, then attach them to the special-purpose NC (no-connect) net and the warnings will be supressed:

>>> pic10[1,3,4] += NC
>>> ERC()
ERC WARNING: Unconnected pin: POWER-IN pin 2/VSS of PIC10F220-I/OT/U1.
ERC WARNING: Unconnected pin: POWER-IN pin 5/VDD of PIC10F220-I/OT/U1.
ERC WARNING: Unconnected pin: INPUT pin 6/Vpp/~MCLR~/GP3 of PIC10F220-I/OT/U1.

3 warnings found during ERC.
0 errors found during ERC.

In fact, if you have a part with many pins that are not going to be used, you can start off by attaching all the pins to the NC net. After that, you can attach the pins you're using to normal nets and they will be removed from the NC net:

my_part[:] += NC  # Connect every pin to NC net.
...
my_part[5] += Net()  # Pin 5 is no longer unconnected.

The NC net is the only net for which this happens. For all other nets, connecting two or more nets to the same pin merges those nets and all the pins on them together.

Net and Pin Drive Levels

Certain parts have power pins that are required to be driven by a power supply net or else ERC warnings ensue. This condition is usually satisfied if the power pins are driven by the output of another part like a voltage regulator. But if the regulator output passes through something like a ferrite bead (to remove noise), then the filtered signal is no longer a supply net and an ERC warning is issued.

In order to satisfy the ERC, the drive strength of a net can be set manually using its drive attribute. As a simple example, consider connecting a net to the power supply input of a processor and then running the ERC:

>>> pic10 = Part('microchip_pic10mcu','pic10f220-i/ot')
>>> a = Net()
>>> pic10['VDD'] += a
>>> ERC()
...
ERC WARNING: Insufficient drive current on net N$1 for pin POWER-IN pin 5/VDD of PIC10F220-I/OT/U1
...

This issue is fixed by changing the drive attribute of the net:

>>> pic10 = Part('microchip_pic10mcu','pic10f220-i/ot')
>>> a = Net()
>>> pic10['VDD'] += a
>>> a.drive = POWER
>>> ERC()
...
(Insufficient drive warning is no longer present.)
...

You can set the drive attribute at any time to any defined level, but POWER is probably the only setting you'll use. For any net you create that supplies power to devices in your circuit, you should probably set its drive attribute to POWER. This is equivalent to attaching power flags to nets in some ECAD packages like KiCad.

You can also set the drive attribute of part pins to override their default drive level. This is sometimes useful when you are using an output pin of a part to power another part.

>>> pic10_a = Part('microchip_pic10mcu','pic10f220-I/OT')
>>> pic10_b = Part('microchip_pic10mcu','pic10f220-I/OT')
>>> pic10_b['VDD'] += pic10_a[1]  # Power pic10_b from output pin of pic10_a.
>>> ERC()
ERC WARNING: Insufficient drive current on net N$1 for pin POWER-IN pin 5/VDD of PIC10F220-I/OT/U2
... <additional unconnected pin warnings> ...

>>> pic10_a[1].drive = POWER  # Change drive level of pic10_a output pin.
>>> ERC()
... <unconnected pin warnings, but insufficient drive warning is gone> ...

Pin, Net, Bus Equivalencies

Pins, nets, and buses can all be connected to one another in a number of ways. In order to make them as interchangeable as possible, some additional functions are defined for each object:

__bool__ and __nonzero__: Each object will return True when used in a boolean operation. This can be useful when trying to select an active connection from a set of candidates using the or operator:

>>> a = Net('A')
>>> b = Bus('B', 8)
>>> c = Pin()
>>> d = a or b or c
>>> d
A:
>>> type(d)
<class 'skidl.Net.Net'>

Indexing: Normally, indices can only be used with a Bus object to select one or more bus lines. But Pin and Net objects can also be indexed as long as the index evaluates to zero:

>>> a = Net('A')
>>> c = Pin()
>>> a[0] += c[0]
WARNING: Attaching non-part Pin  to a Net A.
>>> a[0] += c[1]
ERROR: Can't use a non-zero index for a pin.
Traceback (most recent call last):
  File "<stdin>", line 1, in <module>
  File "C:\xesscorp\KiCad\tools\skidl\skidl\Pin.py", line 251, in __getitem__
    raise Exception
Exception

Iterators: In addition to supporting indexing, Pin, Net and Bus objects can also be used as iterators.

>>> bus = Bus('bus', 8)
>>> for line in bus:
    ...:     print(line)
    ...:
bus0:
bus1:
bus2:
bus3:
bus4:
bus5:
bus6:
bus7:

Width: Bus, Net, and Pin objects all support the width property. For a Bus object, width returns the number of bus lines it contains. For a Net or Pin object, width always returns 1.

>>> a = Net('A')
>>> b = Bus('B', 8)
>>> c = Pin()
>>> a.width
1
>>> b.width
8
>>> c.width
1

Selectively Supressing ERC Messages

Sometimes a portion of your circuit throws a lot of ERC warnings or errors even though you know it's correct. SKiDL provides flags that allow you to turn off the ERC for selected nets, pins, and parts like so:

my_net.do_erc = False      # Turns of ERC for this particular net.
my_part[5].do_erc = False  # Turns off ERC for this pin of this part.
my_part.do_erc = False     # Turns off ERC for all the pins of this part.

Going Really Deep

If all you need to do is design the circuitry for a PCB, then you probably know all the SKiDL you need to know. This section will describe the features of SKiDL that might be useful (or not) to some of the avant-garde circuit designers out there.

Circuit Objects

Normally, SKiDL puts parts and nets into a global instance of a Circuit object called default_circuit (which, of course, you never noticed). But you can create other Circuit objects:

>>> my_circuit = Circuit()

and then you can create parts, nets and buses and add them to your new circuit:

>>> my_circuit += Part("Device",'R')  # Add a resistor to the circuit.
>>> my_circuit += Net('GND')          # Add a net.
>>> my_circuit += Bus('byte_bus', 8)  # Add a bus.

In addition to the += operator, you can also use the methods add_parts, add_nets, and add_buses. (There's also the much less-used -= operator for removing parts, nets or buses from a circuit along with the rmv_parts, rmv_nets, and rmv_buses methods.)

You can also place parts, nets, and buses directly into a Circuit object by using the circuit parameter of the object constructors:

>>> my_circuit = Circuit()
>>> p = Part("Device", 'R', circuit = my_circuit)
>>> n = Net('GND', circuit = my_circuit)
>>> b = Bus('byte_bus', 8, circuit = my_circuit)

Hierarchical circuits also work with Circuit objects. In the previous multi-level hierarchy example, the subcircuit could be instantiated into a Circuit object like this:

my_circuit = Circuit()   # New Circuit object.

gnd = Net('GND')         # GLobal ground net.
input_net = Net('IN')    # Net with the voltage to be divided.
output_net = Net('OUT')  # Net with the divided voltage.
my_circuit += gnd, input_net, output_net  # Move the nets to the new circuit.

# Instantiate the multi-level hierarchical subcircuit into the new Circuit object.
multi_vdiv(3, input_net, output_net, circuit = my_circuit)

The actual circuit parameter is not passed on to the subcircuit. It's extracted and any elements created in the subcircuit are sent there instead of to the default circuit. (If the circuit argument is omitted, the subcircuit function uses the default circuit as the target of its operations.)

You can do all the same operations on a Circuit object that are supported on the default circuit, such as:

# Check the circuit for errors.
my_circuit.ERC()

# Generate the netlist from the new Circuit object.
my_circuit.generate_netlist(sys.stdout)

Naturally, the presence of multiple, independent circuits creates the possibility of new types of errors. Here are a few things you can't do (and will get warned about):

You can't make connections between parts, nets or buses that reside in different Circuit objects.
Once a part, net, or bus is connected to something else in a Circuit object, it can't be moved to a different Circuit object.

Converting Existing Designs to SKiDL

You can convert an existing schematic-based design to SKiDL like this:

Generate a netlist file for your design using whatever procedure your ECAD system provides. For this discussion, call the netlist file my_design.net.
Convert the netlist file into a SKiDL program using the following command:
```
netlist_to_skidl -i my_design.net -o my_design.py -w
```

That's it! You can execute the my_design.py script and it will regenerate the netlist. Or you can use the script as a subcircuit in a larger design. Or do anything else that a SKiDL-based design supports.

SPICE Simulations

Now you can describe a circuit using SKiDL and run a SPICE simulation on it! Go here to get the complete details.

Files

index.md

Latest commit

History