kicad-library

name	kicad-library
description	Library management workflow for KiCAD — creating symbols, footprints, and managing libraries via MCP tools. Triggers on: "create a symbol", "make a footprint", "custom component", "register library", "find a part", "pin numbering", "new symbol", "new footprint", "add to library", "library path", "pad layout".
argument-hint	[component or library task]

KiCAD Library Management Workflow

This skill guides Claude through creating and managing KiCAD symbols, footprints, and libraries using Konnect MCP tools. ALL modifications go through MCP tools — never edit .kicad_sym or .kicad_mod files directly.

---

Toolset Loading

load_toolset('library')    # search_symbols, search_footprints, create_symbol, create_footprint,
                           # register_symbol_library, register_footprint_library, get_symbol_info

Always call get_active_toolsets() first to see what is already loaded.

---

Search First Principle

Always search existing libraries before creating custom components.

search_symbols(query)       # Search all symbol libraries
search_footprints(query)    # Search all footprint libraries

KiCAD ships with extensive libraries. Common parts almost always exist:

• Standard passives (R, C, L) → Device library
• Connectors → Connector_Generic, Connector_USB, Connector_HDMI, etc.
• Common ICs (STM32, ATmega, LM7805, NE555) → manufacturer-specific libraries
• Transistors/MOSFETs → Transistor_FET, Transistor_BJT

Only create a custom symbol/footprint when:

• The part does not exist in any library
• The existing symbol has wrong pin count/arrangement
• You need a proprietary/unusual package

---

Symbol Creation

Pin Numbering Conventions

Component Type	Convention
IC (DIP/SOIC/QFP)	Counter-clockwise from pin 1 (standard IC convention)
Passives (R, C, L)	Pin 1 and Pin 2
Diodes	Pin 1 = Anode (A), Pin 2 = Cathode (K)
Transistors (BJT)	1=Base, 2=Collector, 3=Emitter (BCE)
MOSFETs	1=Gate, 2=Drain, 3=Source (GDS)
Connectors	Sequential from 1
Crystal	Pin 1, Pin 2 (+ case ground if 4-pin)

Pin Types

Type	Use For
input	Logic/analog inputs, gate inputs
output	Logic/analog outputs, push-pull drivers
bidirectional	Data bus lines, I2C SDA, GPIO
tri_state	Outputs with high-impedance state
passive	Resistor/capacitor/inductor pins, crystal pins
power_in	VCC, VDD, GND pins (power consumer)
power_out	Regulator output, power source pins
open_collector	Open-drain/open-collector outputs
open_emitter	Open-emitter outputs
unspecified	Pins with no clear electrical type
no_connect	Pins that must not be connected

Required Symbol Properties

Every symbol must have these fields:

Property	Description	Example
Reference	Designator prefix	U, R, C, J, D, Q, L
Value	Part name or value	STM32F103C8, 10k, 100nF
Footprint	Default footprint assignment	Package_SO:SOIC-8_3.9x4.9mm
Datasheet	URL to datasheet	https://...

Optional but recommended:

• LCSC — LCSC/JLCPCB part number for assembly
• MPN — Manufacturer part number
• Description — Short text description

Symbol Layout Guidelines

• Pin 1 indicator (dot or bar) on the symbol body
• Inputs on the left side, outputs on the right side
• Power pins on top (VCC) and bottom (GND)
• Pin spacing: 2.54mm (100mil) standard grid
• Symbol body: rectangle for ICs, standard shapes for passives/discretes

---

Footprint Creation

Pad Types

Type	Use For
smd	Surface-mount pads (no drill hole)
thru_hole	Through-hole pads (plated drill)
np_thru_hole	Non-plated through hole (mounting holes, slots)

Standard Pad Sizes Reference

Package	Pad Size (mm)	Pitch (mm)	Notes
0402	0.5 x 0.5	—	2 pads, 0.5mm gap
0603	0.8 x 0.8	—	2 pads, 0.8mm gap
0805	1.0 x 1.0	—	2 pads, 1.0mm gap
1206	1.5 x 1.2	—	2 pads, 1.6mm gap
SOT-23	0.9 x 0.7	0.95	3 pads
SOT-23-5	0.9 x 0.7	0.95	5 pads
SOIC-8	1.5 x 0.6	1.27	8 pads, 5.4mm row spacing
SOIC-16	1.5 x 0.6	1.27	16 pads, 5.4mm row spacing
TSSOP-16	1.4 x 0.4	0.65	16 pads, 4.4mm row spacing
QFP-32	1.5 x 0.3	0.8	32 pads, quad-flat
QFP-48	1.5 x 0.3	0.5	48 pads, quad-flat
QFN-32	0.7 x 0.25	0.5	32 pads + exposed pad
QFN-48	0.7 x 0.25	0.5	48 pads + exposed pad

Courtyard

• Extend courtyard 0.25mm beyond the outermost pad edges on all sides
• This ensures minimum spacing between components during assembly
• Use F.CrtYd layer, 0.05mm line width

Footprint Layers

Layer	Purpose
F.Cu	Front copper (pads)
B.Cu	Back copper (pads for bottom-side components)
F.Mask	Front solder mask opening (auto-generated from pads)
F.Paste	Front solder paste (stencil openings)
F.SilkS	Front silkscreen (component outline, pin 1 marker)
F.CrtYd	Front courtyard (assembly spacing)
F.Fab	Front fabrication (true component dimensions)

Footprint Layout Guidelines

• Pin 1 marker on silkscreen (dot, bar, or chamfered corner)
• Component outline on F.Fab layer with true dimensions
• Silkscreen outline 0.1mm outside F.Fab outline
• Reference (%R) on F.SilkS, readable at 1.0mm text height
• Value on F.Fab layer

---

Library Registration

Register a Symbol Library

register_symbol_library(name, path, scope)

Register a Footprint Library

register_footprint_library(name, path, scope)

Scope

Scope	Location	Visible To
global	User-level sym-lib-table	All projects
project	Project-level sym-lib-table	This project only

Recommendation: Use project scope for project-specific custom parts. Use global scope only for reusable personal libraries used across multiple projects.

Library File Locations

• Symbol libraries: *.kicad_sym files
• Footprint libraries: directories containing *.kicad_mod files
• Project-level tables: sym-lib-table and fp-lib-table in project directory

---

IPC Naming Conventions (Brief Reference)

Standard footprint naming follows IPC-7351:

[Type]_[Dimensions]_[Pitch]_[Suffix]

Examples:

• R_0402_1005Metric — 0402 resistor (1.0x0.5mm metric)
• C_0805_2012Metric — 0805 capacitor (2.0x1.2mm metric)
• SOIC-8_3.9x4.9mm_P1.27mm — SOIC-8 with 1.27mm pitch
• QFN-32-1EP_5x5mm_P0.5mm — QFN-32 with exposed pad, 5x5mm body
• SOT-23 — SOT-23 3-pin
• TSSOP-16_4.4x5mm_P0.65mm — TSSOP-16 with 0.65mm pitch

Dimension format: LxW in mm (body dimensions, not pad-to-pad).

---

Common Workflows

Create a New IC Symbol + Footprint

1. search_symbols(part_name) — confirm it does not exist
2. search_footprints(package_name) — check if footprint exists (often it does)
3. Create symbol with correct pin count, names, numbers, and types
4. Assign existing footprint OR create custom footprint from datasheet
5. Register library if new
6. Set Footprint property on symbol to link them

Add LCSC Number to Existing Components

1. Load sch_query toolset
2. Find components missing LCSC field
3. Search JLCPCB parts for matching part numbers
4. Update component fields with LCSC numbers

Create Project-Specific Library

1. Create new .kicad_sym file for symbols
2. Create new directory for footprints
3. Register both with project scope
4. Add custom components as needed

---

Rules

1. Always search before creating — most parts already exist in KiCAD libraries
2. Never edit .kicad_sym or .kicad_mod directly — use MCP tools only
3. Follow pin numbering conventions — IC pins counter-clockwise from pin 1
4. Set pin types correctly — ERC depends on accurate pin types
5. Include all required properties — Reference, Value, Footprint, Datasheet
6. Use 0.25mm courtyard margin — standard clearance for assembly
7. Mark pin 1 clearly — both on symbol and footprint silkscreen
8. Use project scope by default — avoid polluting global libraries
9. Name footprints per IPC — consistent naming helps future reuse
10. Load toolsets first — check get_active_toolsets() and load library before starting