Kicad Library Skill for Claude

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

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

Add LCSC Number to Existing Components

• Load sch_analysis toolset
• Find components missing LCSC field
• Search JLCPCB parts for matching part numbers
• Update component fields with LCSC numbers

Create Project-Specific Library

• Create new .kicad_sym file for symbols
• Create new directory for footprints
• Register both with project scope
• Add custom components as needed

Rules

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

10. Load toolsets first — check get_active_toolsets() and load library before starting