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 — the datasheet decides, not a convention

There is no safe universal pin-numbering rule for a real part. Physical lead numbers are defined by the exact manufacturer part number and package suffix. BJT and MOSFET lead order varies between manufacturers, packages and variants; bottom-view, mirrored, socketed and connector drawings reverse it. A symbol can be syntactically valid and still be electrically wrong when its pins and the footprint's pads describe different physical leads.

Even KiCad's own generic symbols do not follow one order — Device:LED is pin 1 = K (cathode), pin 2 = A (anode), the opposite of the "pin 1 = anode" rule people expect. Check, do not assume.

Before creating or wiring a package-sensitive part:

1. search_symbols / list_symbols_in_library first — prefer an existing library symbol over authoring a new one.
2. Confirm the exact manufacturer part number and package suffix.
3. Note the drawing view of every datasheet figure (top, bottom, component, solder, mating). An unstated view is the most common source of mirrored parts.
4. Walk the physical leads from the documented key, in the documented direction.
5. Reconcile three counts: datasheet leads, symbol pins, footprint pads. Document any intentional duplicate or mechanical-only pad.
6. Read the result back with get_symbol_info and get_footprint_info rather than trusting what you just wrote.
7. Refuse to use the part in a real schematic while any mirror, reversal, duplicate, missing lead or view ambiguity is unresolved.

Physical pin-map acceptance contract

For every custom or package-sensitive part, complete this record before the symbol and footprint are accepted. "Looks sequential" and a matching pin count are not evidence.

Record the manufacturer, exact MPN and package suffix, datasheet document number/revision, source URL, relevant page numbers, symbol library ID, and footprint library ID. Then add one row for every physical lead:

Apply these rules to the table:

• Walk from the datasheet's documented key, notch, dot, flat, bevel, or other datum in the stated direction. State top, bottom, component, solder, pin, or mating view in every row; never silently translate between views.
• Give repeated physical leads separate rows even when they share one electrical function. List exposed pads, shields, mounting tabs, and mechanical holes separately and state whether each is an electrical pad, a duplicated connection, or intentionally absent from the symbol.
• Reconcile and record the datasheet physical-lead count, symbol electrical-pin count, footprint electrical-pad count, duplicate-pad count, and mechanical-only feature count. Explain every difference.
• Treat a symbol pin number and footprint pad number as the same physical lead only when the evidence row proves it. Names such as A/K, G/D/S, B/C/E, COM, or VCC do not establish the physical number.

Acceptance procedure:

1. Create or select the exact symbol and footprint only after completing the source columns above.
2. Query the symbol back with get_symbol_info and the footprint with get_footprint_info(include_pads=true). The returned pad coordinates and rotations are footprint-local. Compare every returned pin/pad number, name, type, coordinate, drill, size, and layer set to the table and datasheet.
3. Place a disposable symbol and footprint in a scratch project. Render the schematic and board, then inspect the pin-1/key marker, numbering direction, top/bottom orientation, pad geometry, drill/slot geometry, courtyard, fab, and silkscreen. For mating parts, inspect the mating view as well.
4. Read the disposable instances back; do not accept only the values requested during creation as proof they were written.
5. Refuse acceptance and keep the part out of a real schematic or PCB if any lead is missing, duplicated without explanation, mirrored, reversed, assigned to a different function, or ambiguous in view/direction. Record an unavailable datasheet figure, query, or render as BLOCKED, never as pass.

The rows below are starting hypotheses for generic parts only. Verify each against the actual symbol with get_symbol_info before relying on it.

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