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,
                           # edit_footprint_pad, set_footprint_graphics, set_footprint_metadata,
                           # set_footprint_models, get_footprint_info, register_symbol_library,
                           # register_footprint_library, get_symbol_info
load_toolset('pcb_components') # update_footprints_from_library for placed instances

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

Refresh Placed Footprints

Editing a .kicad_mod library file does not change copies already embedded on a board. After a library edit, call update_footprints_from_library; it is Konnect's MCP equivalent of KiCad Tools → Update Footprints from Library.

This operation is not update_pcb_from_schematic. Schematic sync updates schematic-owned fields while preserving artwork. Library refresh replaces supported library-owned pads, graphics, attributes, metadata, and 3D models while preserving the placed footprint's reference, value, position, rotation, board side, locked state, KIID, symbol metadata, instance overrides, and pad nets by logical pad number.

Always dry-run first:

update_footprints_from_library(
  board,
  references?,
  library_ids?,
  dry_run,
  expected_plan_revision?
)

• Use dry_run=true and review status, coverage, changes, and diagnostics.
• Apply with dry_run=false and the exact returned expected_plan_revision.
• Keep the requested board open in live KiCad; there is no closed-board file fallback.
• One successful apply is one KiCad undo entry.
• A stale plan, unresolved library, removed connected pad, or unsupported library content returns a non-mutating conflict for the whole selection.

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

Pin Types

Required Symbol Properties

Every symbol must have these fields:

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

Pad Side and Shape Details

create_footprint defaults SMD pads to the front-side layer set ["F.Cu", "F.Paste", "F.Mask"]. For bottom-side SMD pads, set layers=["B.Cu", "B.Paste", "B.Mask"] explicitly. Through-hole pads default to ["*.Cu", "*.Mask"].

Each pad may also set:

• rotation in degrees; omit it for 0.
• roundrect_rratio from 0 through 0.5 when shape="roundrect".
• layers using only canonical pad layers: F.Cu, B.Cu, F.Paste, B.Paste, F.Mask, B.Mask, *.Cu, and *.Mask.

create_footprint(
  ...,
  pads=[{
    number: "1",
    type: "smd",
    shape: "roundrect",
    x: -8.075,
    y: 4.7,
    width: 2.5,
    height: 2.55,
    layers: ["B.Cu", "B.Paste", "B.Mask"],
    rotation: 180,
    roundrect_rratio: 0.2
  }]
)

Standard Pad Sizes Reference

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

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

Existing Footprint Graphics

Use set_footprint_graphics to add or change line, arc, rectangle, circle, or polygon primitives in an existing .kicad_mod. Never patch the file directly.

set_footprint_graphics(
  footprint path,
  selector={layer: "B.CrtYd"},
  mode="replace",
  graphics=[...]
)

• append preserves existing supported graphics on the selected layer.
• replace replaces all supported graphics on the selected layer in one atomic write.
• delete removes all supported graphics on the selected layer.
• Text, pads, properties, models, groups, and graphics on other layers are preserved.
• Replacement/deletion stops with a conflict if a selected graphic belongs to a group; do not work around this by editing the file.
• Polygons close automatically. Supply at least three distinct points; repeating the first point at the end is optional.
• Use get_footprint_info with graphics inclusion enabled and a layer filter to verify the resulting type, geometry, stroke width, fill, and item ID.

Existing Footprint Metadata

Use set_footprint_metadata to replace a footprint description, search tags, or KiCad footprint attributes without changing pads, graphics, properties, groups, or 3D models.

set_footprint_metadata(
  footprint_path=".../Part.kicad_mod",
  description="Optional replacement",
  tags=["keyboard", "hot_swap"],
  attributes=["exclude_from_pos_files"]
)

• Supply at least one metadata field.
• Only supplied fields change.
• Empty tags or attributes removes the corresponding block.
• exclude_from_pos_files omits the footprint from pick-and-place output without implicitly adding exclude_from_bom.
• Use edit_footprint_pad with new_number and optional match_all=true to renumber one or every matching direct-child pad atomically.

Existing Footprint 3D Models

Use set_footprint_models to append, replace, or delete top-level 3D model associations without changing any non-model footprint content.

set_footprint_models(
  footprint_path=".../Part.kicad_mod",
  mode="replace",
  models=[{
    path: "../models/Part.step",
    offset: {x: 0, y: 0, z: 0},
    scale: {x: 1, y: 1, z: 1},
    rotate: {x: 0, y: 0, z: 90}
  }]
)

• append and replace require at least one model.
• delete requires models to be omitted or empty and removes every top-level model.
• Omitted transforms default to offset 0/0/0, scale 1/1/1, and rotation 0/0/0.
• Multiple model blocks are written in payload order in one atomic operation.

Library Registration

Register a Symbol Library

register_symbol_library(nickname, library_path, scope?, project?, replace_existing?)

Register a Footprint Library

register_footprint_library(nickname, library_path, scope?, project?, replace_existing?)

• Registration is idempotent by default: an existing nickname is left unchanged.
• Set replace_existing=true to update a stale URI for that nickname in place.
• Project-local and same-repository sibling libraries are written as portable ${KIPRJMOD} URIs; existing options, descriptions, and unrelated entries are preserved.

Scope

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(query) — pass the part name; confirm it does not exist
2. search_footprints(query) — pass the package name; check if the 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_analysis 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
11. Use layer-scoped graphic edits deliberately — replace and delete affect every supported primitive on the selected layer