Components

A component is anything that has a KiCAD symbol or footprint — resistors, MCUs, vias, mounting holes, or regulatory images. The Component class is the base class for all of them.

class

Component

import { Component } from '@typecad/pcb'

The base class for all components in typeCAD — in KiCAD terms, anything that has a footprint file associated with it. Construct it directly for simple parts, or extend it with named pins for ICs (usually via the add-component tool, below).

Example first

component.ts

import { Component } from '@typecad/pcb';

let u1 = new Component({ footprint: 'Package_SO:SOIC-8_5.3x5.3mm_P1.27mm' });

Options

Option	Type	Description
reference	string	Reference designator (R1, U2...)
value	string	Value of component
footprint	string	KiCAD footprint path, e.g. Package_SO:SOIC-8_5.3x5.3mm_P1.27mm
symbol	string	KiCAD symbol library path
prefix	string	Prefix for reference designator
datasheet	string	Link to component datasheet
description	string	Description of component
voltage	string	Voltage rating of component
wattage	string	Wattage rating of component
mpn	string	Manufacturer Part Number
dnp	boolean	true if Do Not Populate
simulation	object	{ include: true, model: 'ngspice-model' }
pcb	object	Position on the board { x, y, rotation }
text	array	Arbitrary text entries on the board, with property, text, position, styling
fab	object	Fabrication layer text entry — a positioning object or [text, positioning] tuple
referenceLayout	object	Reference designator text position and style (defaults to F.SilkS)
valueLayout	object	Value text position and style (defaults to F.Fab)
fabLayout	object	Fab text position and style (defaults to F.Fab; text defaults to ${REFERENCE})

The three layout properties (referenceLayout, valueLayout, fabLayout) accept an ITextPositioning object and can be set at construction or assigned after creation.

pin `pin(number, config?): Pin`

Creates and registers a pin — see Pins & Power. In generated component files this is how named pins (u1.VCC) are defined.

Connectors & mechanical parts

A few common non-IC parts ship as ready-made classes, alongside the passives — all from the package root:

import { Connector, TestPoint, MountingHole, NetTie } from '@typecad/pcb';

let j1 = new Connector({ number: 4 });            // 1x04 pin header (series presets: 'pin-header', 'JST-SH')
let tp1 = new TestPoint();                        // 1.0 mm pad probe point
let mh1 = new MountingHole({ size: 'M3' });       // M2–M8 presets
let tie1 = new NetTie({ net1: 'VBUS', net2: 'VOUT' });  // ties two nets, pin count follows the nets

typecad add component

The better way to create components. Run typecad-pcb add component from the ./hw directory, or click the add_component button in the VSCode GUI under NPM Scripts. It asks where the component comes from — the KiCAD library, a local file, or an EasyEDA/JLCPCB part — and generates a .ts file like this:

ATtiny85_20S.ts

import { Component } from '@typecad/pcb';
/**
 | Pin # | Name         | Type              |
 | --:   | :--          | :--               |
 | 8     | VCC          | power_in          |
 | 4     | GND          | power_in          |
 | 5     | AREF_PB0     | bidirectional     |
 | 1     | _RESET_PB5   | bidirectional     |
 */
export class ATtiny85_20S extends Component {
    VCC = this.pin(8, { type: 'power_in' });
    GND = this.pin(4, { type: 'power_in' });
    AREF_PB0 = this.pin(5, { type: 'bidirectional' });
    _RESET_PB5 = this.pin(1, { type: 'bidirectional' });

    constructor(reference?: string | undefined) {
        super("Package_SO:SOIC-8_5.3x5.3mm_P1.27mm");
        this.symbol = "MCU_Microchip_ATtiny:ATtiny85-20S";
        if (reference) this.reference = reference;
    }
}

The file extends Component and adds Pin objects — so instead of u1.pin(1) you write u1.VCC. Use the generated class like any other:

use.ts

import { ATtiny85_20S } from './ATtiny85_20S';
let u1 = new ATtiny85_20S();

Finding parts: typecad-pcb search

terminal

typecad-pcb search "voltage regulator"
typecad-pcb search LM358
typecad-pcb search "SOIC-8" --footprint --json

Fuzzy-matches against the KiCAD symbol libraries and returns the symbol name, footprint, and description, in LibraryName:SymbolName format. With --footprint, it searches the installed footprint libraries instead — results include the pad numbers. Options: --format (detailed, compact, table, json), --sort (score, id, manufacturer, package), --limit (default 5).

Previous The PCB class Next Passives