Standard library

Every footprint family in @pcbjs/lib with its pins, prefix and frame, the helpers for writing footprints, and the value, font and shape utilities. Import from @pcbjs/lib, or from one module such as @pcbjs/lib/ic.

Every footprint is dual-mode: R0603('330') makes a part, <R0603 ref="R1" at="5 5" /> renders, see schematic.md. Ids use the pcbjs: prefix and follow KiCad names. Frames are mm, y down, origin at the body centre unless a family says otherwise. Land patterns follow the KiCad 9 library, and a test places every footprint on an empty board of every fab preset with no finding.

A positive rotation turns a part counter-clockwise on screen, and side="B" mirrors it first: a PinHeader(2) at at="10 10 90deg" has pin 1 at (10, 10) and pin 2 at (12.54, 10), its +y row turned to +x. pcbjs inspect prints where every pad landed.

Generators throw a TypeError naming a bad parameter and the form it takes.

Renaming pins

Every generated footprint takes pinNames, and withPins renames a copy:

import { SOT23, withPins, Crystal3225, SOT223 } from '@pcbjs/lib'

const LDO = SOT23(5, { pinNames: ['VIN', 'GND', 'EN', 'NC', 'VOUT'] })   // a list renames the pins in order
const Y = withPins(Crystal3225, { 2: 'GND1', 4: 'GND2' })                   // a record maps pad numbers or pin names
const REG = withPins(SOT223, ['GND', 'VOUT', 'VIN'])
// LDO('AP2112K-3.3').connect({ VIN, GND, EN: VIN, VOUT: V3 })

• Pads given the same name share one pin. A rename can also split a shared pin.
• A pad named NC is no pin and goes in the footprint's nc list, so it needs no connection.
• prefix and value change the ref prefix and the default value.
• The same arguments give the same factory, so source(SOT23(5), …) finds parts made elsewhere.

Passives, @pcbjs/lib/passives

Factory	Pins	Prefix
R0402, R0603, R0805, R1206	1, 2	R
C0402, C0603, C0805, C1206	1, 2	C
LED0603, LED0805, LED1206	K pad 1 with the silk bar, A pad 2	D
LED(size, color?)	K, A	D
chip(prefix, size, { names?, polarity?, color? })	1, 2 or the two names	the prefix, D for LED

Pad 1 is at -x. chip prefixes are R, C, LED, L and D; sizes 0402, 0603, 0805 and 1206. Named pins stay reachable by number.

Headers and connectors

The headers and connectors take one form: the call makes a part, and its last argument is the value or an options object.

import { PinHeader, PinSocket, JST_PH, JST_XH, USBC } from '@pcbjs/lib'

const J1 = PinSocket(20, { rows: 2, value: 'GPIO 2x20', source: { MPN: 'SSQ-120-03-T-D' } })   // pins 1 to 40
const J2 = PinHeader(4, 'PZ254V-11-04P')
const J3 = JST_PH(6, 'side', { drill: 0.8 })
const J4 = JST_XH(4, { value: 'B4B-XH-A', pinNames: ['V5', 'GND', 'CANH', 'CANL'] })
const J5 = USBC('power6', { source: { MPN: 'TYPE-C-31-M-17' } })
// J4.connect({ V5, GND, CANH, CANL })

Call	Pins	Prefix	Frame
PinHeader(pins, { pitch = 2.54, rows = 1, drill, pad })	1 to pins × rows	J	pin 1 square at the origin, pins along +y, rows along +x
PinSocket(pins, { rows = 1, drill, pad })	1 to pins × rows	J	as PinHeader
JST_PH(pins, 'top' | 'side', { drill, pad, silk })	1 to n	J	2.0 mm, centred, pin 1 at -x
JST_XH(pins, { drill, pad })	1 to n	J	2.5 mm, centred, pin 1 at -x
USBC('full16')	GND, VBUS, CC1, CC2, DP, DN, SBU1, SBU2, SHIELD	J	HRO TYPE-C-31-M-12; signal pads at -y, the mouth at +y
USBC('power6')	GND, VBUS, CC1, CC2, SHIELD	J	HRO TYPE-C-31-M-17

• pins counts one row. A 2 x 20 socket is PinSocket(20, { rows: 2 }) with pins 1 to 40.
• The options take the family's own, pinNames, prefix, silk and the part options such as value, source and model. JST_PH defaults to 'top', USBC to 'full16'.
• .footprint(...) with the same arguments is the footprint factory: JST_XH.footprint(4)('B4B-XH-A') makes a part, and withPins and source(factory, value, spec) take it.
• drill is the drill in mm and pad the copper, a diameter or [w, h] in footprint axes. Defaults follow the datasheets as KiCad 9 does: JST PH 0.75 mm in 1.2 x 1.75 mm, JST XH 0.95 mm in 1.7 x 1.95 mm, 2.54 mm headers and sockets 1.0 mm in 1.7 mm. A changed drill or pad adds _Drill0.8mm or _Pad1.8x2.1mm to the footprint id. For any other change, write the footprint with defineFootprint.
• silk is 'full', 'open' or 'none' on every generated family and PinHeader. 'open', the default of JST_PH(n, 'side') and USBC, leaves the mating side out, so a part flush with the edge draws no silk-over-edge; without a mating side it is 'full'. A mode other than the default adds _SilkFull or _NoSilkScreen to the id. kicadFootprint('Lib:Name', { silk }) of @pcbjs/kicad takes it too.
• A 2-row header numbers across the row: pins 1 and 2 side by side, then 3 and 4, so the odd pins form the first row. At 1.27 mm pitch the pads are 1.0 mm on a 0.6 mm drill, a 0.2 mm ring, where KiCad's 0.65 mm drill falls under JLCPCB's 0.18 mm.
• USB-C: the A and B contacts of DP and DN are joined as one pin each. A route to J1.VBUS ends at its nearest pad, or name one, J1['B4']. Connect unused SBU1 and SBU2 to NC. Let the mouth overhang the board edge.

Test points and holes

Factory	Pins	Prefix	Notes
TestPad(d = 1.5)	1	TP	round SMD pad on F.Cu, out of BOM and placement
PogoPad(d = 1.5, { cols, rows, pitch = 2.54 })	1 to n, down each column	TP, or J for a grid	bare pads for a pogo fixture
MountingHole(d = 3.2, pad?)	none, or 1 with a pad	H	NPTH; pad true or a diameter adds a plated ring

A mounting hole without a pad has no pins, so it is not a part: place it as a plain footprint, const Hole = MountingHole(3.2) and <Hole ref="H1" at="3.5 3.5" />. With a pad it is a part with pin 1, for GND.

ICs, @pcbjs/lib/ic

Factory	Pins	Prefix	Numbering
SOT23(3)	1, 2, 3	Q	1 and 2 down the left, 3 on the right
SOT23(5), SOT23(6)	1 to n	U	1 to 3 down the left, the rest up the right
SOT223	1, 2, 3	U	the tab, pad 4, is pin 2
SOIC(pins, 'N' | 'W')	1 to n	U	1.27 mm; down the left from pin 1, up the right
TSSOP(pins)	1 to n	U	0.65 mm, as SOIC
QFN(pins, size, pitch, ep?, { pad?, vias?, height? })	1 to n, EP	U	counter-clockwise from pin 1 at the top of the left side
LQFP(pins, size, pitch, { ep?, vias? })	1 to n, EP with ep	U	as QFN

• The exposed pad is pad number pins + 1, pin EP. Rename it with { pinNames: { EP: 'GND' } }.
• vias: n adds an n × n grid of thermal vias, 0.3 mm drill at 1 mm pitch, in the exposed pad.

Power, switches, LEDs, crystals, modules

Factory	Pins	Prefix	Notes
CR2032Holder	+ on two tabs, - the centre contact	BT	Keystone 3034; keep F.Cu clear under the cell
BatteryPads({ pitch, dia, drill })	+, -	BT	wire pads, drill: 0 for SMD tabs; out of BOM
TactSwitch(size)	A pads 1 and 2, B pads 3 and 4	SW	sizes 6x6, 5.1x5.1, 4.5x4.5, 4.2x3.2, and 3x4 with two pads
SlideSwitch()	1, 2 common, 3	SW	C&K JS102011SAQN
WS2812B('5050' | '2020')	DIN, DOUT, VDD, GND	D	pad numbers differ per size; use the names
Crystal3225	X1, GND on two pads, X2	Y	withPins splits the lid pads
Crystal2012, Crystal3215, Crystal5032, Crystal49S	1, 2	Y
ESP32C3Mini1	GND, 3V3, EN, IO0 to IO10, IO18, IO19, RXD0, TXD0	U	14 NC pads in nc; antenna at -y

ESP32C3Mini1Footprint({ antennaKeepout }) makes the module with or without the hard keepout under its antenna, on every copper layer. Place the antenna end at or past the board edge.

3D models

Every footprint has a body, generated or fetched on first use, see 3d.md.

Family	Model
passives, LEDs, PinHeader, SOT23, SOT223, SOIC, TSSOP, QFN, LQFP, WS2812B	generated
PinSocket, JST_PH, JST_XH, Crystal3225, Crystal3215, Crystal5032, Crystal49S, CR2032Holder, TactSwitch 6x6, 4.5x4.5, 4.2x3.2 and 3x4	KiCad 3D library
TactSwitch 5.1x5.1, SlideSwitch, Crystal2012, USBC	LCSC C318884, C221660, C97603, C165948, C283540
ESP32C3Mini1	Espressif's KiCad library
TestPad, PogoPad, MountingHole, BatteryPads	none

A part's model option, or the model prop where it is placed, replaces it with a STEP, glTF or WRL file, the library's body the fallback:

import { R0603 } from '@pcbjs/lib'

const R1 = R0603({ value: '330', model: { file: './models/R_0603_1608Metric.step', rotate: [0, 0, 180] } })

• The path is relative to the file holding the literal, as an import is; offset, rotate and scale follow KiCad. Passives, PinHeader and PinSocket share KiCad's origin; JST, centred, takes an offset.
• pcbjs model add <file> --ref J1 fits a vendor file, see models.md; withGenerated(model, props) in @pcbjs/lib/footprint keeps a fallback for your own footprint.

Writing footprints, @pcbjs/lib/footprint

smd(num, x, y, w, h, extra?)                 // roundrect SMD pad centred at x y
tht(num, x, y, dia, drill, extra?)           // round through-hole pad
npth(x, y, drill)                            // non-plated hole
courtyard(w, h, cx = 0, cy = 0, side = 'F.CrtYd')   // rectangle centred at cx cy
silkRect(w, h, width = 0.15)                 // silk rectangle centred on the origin
padRow(n, pitch, { size, at?, axis?, drill?, first?, reverse?, names?, shape?, firstShape? })
padGrid(cols, rows, pitch, { size, at?, rowPitch?, order?, drill?, first?, names?, shape?, firstShape? })
silkOutline(w, h, { cx?, cy?, pads?, clearance?, width?, offset?, layer?, edges? })

• padRow centres n pads on at along axis, numbered from first, 1 by default. padGrid numbers row by row, or column by column with order: 'columns'. Both return pad elements; padRowDefs and padGridDefs return the same as data.
• silkOutline draws a body outline broken wherever it would come within clearance of a pad in pads, so the fab never clips it. A pad there is geometry only, { x, y, w, h } by centre and size, and a PadDef works too. edges picks the sides to draw from top, bottom, left and right.
• A footprint written by hand is a function returning <footprint>, wrapped in defineFootprint, see schematic.md. examples/demo/lib/MyPart.tsx is a SOT-23 written that way.

Brand

<Brand> draws the pcbjs mark and wordmark in silk, js as an outline, from site/brand/wordmark-mono.svg.

<Brand at="24 17" height={5} />
<Brand at="6 6 90" height={4} only="mark" layer="B.SilkS" />

• height = 5 is the ink height in mm; at is its centre, rot turns it, layer = "F.SilkS", and a B. layer reads from below. It is 3.2 times as wide as high; only="mark" or "wordmark" draws one half.
• Below silkMinWidth × 26.25 high, 3.94 mm at 0.15, the js outline would be too thin: a compile error names the minimum, brandMinHeight(silkMinWidth, only?). The mark alone goes to 2.1 mm.

Values, @pcbjs/lib/values

• parseOhms('4k7') is 4700; 330, 4.7k, 10R, 0R, R47, 1M and 47Ω work. parseFarads('100n') is 1e-7. Both return null for text that is not a value.
• formatValue(4700, 'Ω') is 4.7 kΩ. eia96(ohms) is the EIA-96 code or null.
• resistorCode(ohms, size, tolerance?) is the code printed on a chip resistor, which the 3D view shows.

Fonts and shapes

• strokeText(text, { size, thickness, anchor, width?, lineHeight?, letterSpacing? }) from @pcbjs/lib/fonts returns { strokes, width, height, missing }, the polylines <text> draws. See fonts.md.
• rect, roundedRect, circle and slot from @pcbjs/lib/shapes return path data, see layout.md.
• @pcbjs/lib/rules and @pcbjs/lib/stackups are in rules.md and board.md.