https://github.com/bhdl/bhdl/master/bhdl-lib/bhdl/private/library-IC.rkt) file for the available components and their pins.

Basic components:

Resistor R Capacitor C Fuse LED LED0603 Diode 1N4148W FerriteBead Crystal-2

Crystal-4 PinHeader PinHeader2 Transistor AMS1117-3.3

Simple ICs:

CP2102N

ICs:

ATtiny25 ATtiny45 ATtiny85 ATmega128 ATmega16 ATmega48 ATmega88 ATmega168

ATmega328 ATmega8U2 ATmega16U2 ATmega32U2 ATmega16U4 ATmega32U4 ATmega8

GD32VF103CBT6

ESP32-WROVER-E

Aruinos

Arduino-Uno

Arduino-Uno-ICSP

Arduino-Nano

Arduino-Mini

Arduino-Micro

Arduino-MKR

Other components:

Cherry kailh-socket mounting-hole stabilizer-2u

USB-C-6

USB-C-16

USB-Micro

Creating (and Contributing!) Your Own Library

Components can be defined via the define/IC syntax:

(define/IC (LED)

#:FP (fp-diode plus minus)

#:PREFIX "LED")

Notes about the fields:

• #:FP expects a footprint and pin names. These pin names are arbitrary but the order is important, it will be mapped to the exact order of the corresponding footprint. Refer to footprint document for the definition of the footprint pin order.
• #:PREFIX defines what is the prefix to be appearing on PCB. E.g. R1, LED4

This defines a function called LED, and an LED instance can be created via the function call (define myled (LED)). The pins named plus and minus can be accessed to make connections. To enalbe a component to connect in "line connection syntax", you need to specify the #:LEFT and #:RIGHT pins:

(define/IC (LED)

#:FP (fp-diode plus minus)

#:PREFIX "LED"

#:LEFT plus

#:RIGHT minus)

The left and right delcaration makes it possible to use components of more than 2 pins in the line connection syntax. For exampole, 4 pin switches (where 2 groups are connected)

(define/IC (SKRPACE010)

#:FP ((lcsc->fp "C139797")

A1 A2

B1 B2)

#:PREFIX "KEY"

#:LEFT A1

#:RIGHT B1)

One can change the default left and right orientation easily by defining a circuit wrapper, more on this on the make-circuit document.

Many two-pin non-polarized components do not have meaningful names. E.g. a resistor just have pin 1 and pin 2. A pin header just have pin 1 2 3 4 ... For these components, you can write #:auto-FP in place of #:FP, and the numbers (starting from 1) will be added for you based on how many pins the footprint has. You can use 1 and 2 for #:LEFT and #:RIGHT declaration. E.g.

(define/IC (Resistor R)

#:auto-FP (fp-resistor "0603")

#:PREFIX "R"

#:LEFT 1

#:RIGHT 2)

There may be many footprints for an IC. Thus you are allowed to specify multiple footprints:

(define/IC (Resistor R)

#:auto-named-FP ("0603" (fp-resistor "0603"))

#:auto-named-FP ("0805" (fp-resistor "0805"))

#:PREFIX "R")

You can specify which footprint variant to use via

(R #:FP "0603")

If not specified, the first one is used.

For ICs, there are two special notes:

1. ICs typically have well-defined footprints. For that, some syntax sugar names can be used, e.g. #:DIP #:QFN.
2. There are often more than one name for a pin of IC. E.g. For ATTiny-serie MCUs, the PB0 also functions as MOSI, SDA, PCINT0, and more. This must be specified in #:ALIAS to delcare they are aliases for the same pin. All the pin names will be available for making connections.

(define/IC (ATtiny25 ATtiny45 ATtiny85)

#:ALTS ([VCC]

[GND]

[PB0 MOSI DI SDA AIN0 OC0A OC1A AREF PCINT0]

[PB2 SCK USCK SCL ADC1 T0 INT0 PCINT2]

[PB3 PCINT3 XTAL1 CLKI OC1B ADC3]

[PB4 PCINT4 XTAL2 CLKO OC1B ADC2]

[PB5 PCINT5 RESET ADC0 DW])

#:DIP (8 PB5 PB3 PB4 GND PB0 PB1 PB2 VCC)

#:QFN (20 PB5 PB3 DNC DNC PB4

DNC DNC GND DNC DNC

PB0 PB1 DNC PB2 VCC

DNC DNC DNC DNC DNC))

footprints

BHDL can read KiCAD and read EasyEDA footprints. For many components listed on LCSC.com have associated footprints. We thus support getting the footprint directly via the ID. E.g.

(lcsc->fp "C466653")

If the local library $BHDL_LIBRARY_PATH/easyeda does not contain the footprint, it will query EasyEDA website and writes the footprint to $BHDL_LIBRARY_PATH/easyeda/xxx.json for caching. As we run it for more components, our repo will be tracking many components.

This makes it easy to define a new component, e.g. the 1N4148W diode can be defined simply as:

(define/IC (1N4148W)

#:FP (lcsc->fp "C466653") (- +)

#:LEFT +

#:RIGHT -

#:PREFIX "D")

The order of footprint pins are defined as the orders of the pin occurance in the KiCAD or EasyEDA footprints, not the name of footprint pins. Although many footprints have numerical 1 2 3 ..., there are also text name, and there's no heuristic to sort them.

The choice of using this order of pins has a caveat: the pin order might not be the actual numerical order. This can be especially comon in KiCAD footprints where the numerical numbers may be mixed in arbitrary order.