Kicad Library

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