kicad-tool

name	kicad-tool
description	Use for ANY read or write on `.kicad_sch` / `.kicad_pcb` files — never `Read`/`cat`/`grep`/`Edit` them directly. Also use when the user asks what pins connect to what other pins, what net a pin is on, which components share a net, or the value/MPN/footprint of a component ref. All query, edit, render, inspect, ERC/DRC, netlist, and validate ops go through this CLI.

KiCad Tool

Single owner of repository-local KiCad commands. Other skills must call this CLI, never the helper modules.

.kicad_sch / .kicad_pcb are huge S-expr files: raw Read/cat blows context and raw Edit corrupts UUIDs and lib_symbols. Pass the top-level schematic to erc / netlist / validate; pass the edited child sheet to inspect / render-region (or via --sheet for validate).

Entrypoint

kicad-tool <domain> <command> ...

KICAD_CLI overrides the executable. Default: /Applications/KiCad/KiCad.app/Contents/MacOS/kicad-cli.

Bootstrap (first run)

Before any subcommand:

1. command -v kicad-tool — if found, skip the rest.
2. Otherwise inspect the host's Python (which python3, pipx --version, uv --version, $VIRTUAL_ENV, PEP 668 EXTERNALLY-MANAGED) and pick a fitting install method. Source URL is always git+https://github.com/mash/kicad-skills.git — this transitively pulls the kiutils fork (pinned in pyproject.toml; upstream lacks API used here). Never pip install kiutils — that grabs upstream and breaks the tool. Examples — pick one, don't run blindly:
   • pipx install git+… (preferred when available)
   • uv tool install git+…
   • pip install git+… inside an active venv
   • Full repo cloned for skill dev: pip install -e . from repo root
   • PEP 668-locked system Python: install pipx first instead of --break-system-packages
3. Confirm with the user before touching system Python or using --break-system-packages.
4. Re-check command -v kicad-tool. If still missing, fall back to python3 -m kicad_tool <args> and tell the user how to fix PATH (pipx ensurepath, etc.).

Verify: kicad-tool --help.

Argument conventions

• <schematic> is always the first positional. Required args are positional in table order.
• Coordinates are a single X,Y (bbox: X1,Y1,X2,Y2); rotation is --rotation R.
• --flag only for optional knobs, mutex selectors (e.g. --uuid vs --at vs --through for sch query wire), and the universal --dry-run (edits) / --format {json,text} (all).
• Output is text by default for every command. Text and --format json carry identical information (text is YAML-like, JSON is JSON). Use --format json only when piping to jq / a script; for plain reading, stick with text.
• On runtime failure the tool prints the offending subcommand's usage: line to stderr after the error message. Read the error tail; do not invoke --help separately.
• Do not invent flags for required args. --bbox, --ref, --symbol etc. do not exist.

Commands

Command	Purpose	Key flags
sch render-region <sheet> <X1,Y1,X2,Y2>	Cropped PNG of a sheet bbox (mm). Use whenever the model needs to see part of a schematic. Take the bbox wide enough to include neighboring symbols, rails, and labels — minimum-tight bbox loses the context needed to judge layout.	-o/--output <path> (default tmp/region.png)
sch inspect <sheet>	Score + collisions (re-renders SVG internally)	--only-text <regex>, --margin
sch erc <top>	ERC, hierarchical	-o/--output <path>
sch netlist <top>	Netlist export	-o/--output <path>
sch validate <top>	erc + netlist + inspect(--sheet) in one call	--sheet <edited>, --save-baseline DIR, --baseline DIR
pcb drc <board>	PCB DRC, always including schematic parity and always refilling + saving zones (kicad-cli does not refill on its own, so this keeps the report and the saved fill in sync with the current outline — note it rewrites the .kicad_pcb). Prints the resolved (absolute) report path — read that path, not a fixed one, since the default is CWD-relative and a stale report from another CWD is a known footgun. Check the report's ** Created on ... ** line for freshness	-o/--output <path> (default tmp/pcb-drc.rpt), --exit-code-violations
pcb validate <board> <top.kicad_sch>	DRC + ref/footprint-lib parity vs schematic	--save-baseline DIR, --baseline DIR
pcb render-region <board> <X1,Y1,X2,Y2>	Cropped PNG of the board (default agent layer set)	--layers F.Cu,F.SilkS,..., -o/--output <path>
pcb sync <board> <top.kicad_sch>	Add missing footprints (5 mm staging grid); swap footprints whose schematic Footprint property changed; refresh footprint bodies whose layout has drifted from the library .kicad_mod (KiCad GUI's "Update Footprints from Library") — all preserving position, rotation, board side, schematic-link (path/sheetname/sheetfile), pad nets, and user-added properties (e.g. MPN/LCSC/Manufacturer); update each pad's (net "...") to match the schematic netlist; idempotent. Tracks/vias/zones are not touched — orphaned net names from pad rename are reported.	-o/--output <path>, --dry-run

PCB DRC in Codex sandbox

On macOS, kicad-cli pcb drc may abort inside Codex's normal sandbox before writing a report, even when the same command works in the user's terminal. If kicad-tool pcb drc ... --format json reports returncode: -6, empty stdout/stderr, and no report file, re-run the exact kicad-tool pcb drc ... command with sandbox_permissions="require_escalated" and a narrow prefix_rule such as ["kicad-tool", "pcb", "drc"]. A successful DRC process can still print DRC: exit=0 while the generated .rpt contains violations, because the bare wrapper does not pass KiCad's --exit-code-violations — open the report (or pass --exit-code-violations to gate on it).

Query (read-only)

Positional <schematic.kicad_sch>. Text by default; --format json only when piping to jq. Same content either way.

Command	Purpose
sch query symbol <sch> <REF>	Symbol position, properties (Value/MPN/LCSC/Footprint), pin map
sch query pin <sch> <REF.PIN> [--netlist PATH]	Pin coords, orientation, and (with netlist) net
sch query net <sch> <NAME_OR_REF.PIN> --netlist PATH	Members and labels of a net (REF.PIN dispatched by .)
sch query region <sch> <X1,Y1,X2,Y2>	All elements inside a bbox
sch query wire <sch> (--uuid U | --at X,Y | --through X,Y)	Locate a wire
sch query label <sch> (--name N | --uuid U)	Locate labels
sch query lib-symbol <sch> <LIB_ID>	Library symbol pins/units (large; prefer query symbol <REF> if a placed instance exists)
sch query list <sch> <KIND> [--netlist PATH]	KIND ∈ symbols/labels/wires/junctions/nets (nets requires --netlist)

PCB equivalents (same shape):

Command	Purpose
pcb query footprint <board> <REF>	Position, layer, rotation, properties, locked state, pad summary
pcb query pad <board> <REF.PAD>	Absolute pad geometry and net
pcb query net <board> <NAME_OR_REF.PAD>	Members of a net
pcb query region <board> <X1,Y1,X2,Y2>	Footprints/drawings/tracks/vias/zones in bbox
pcb query list <board> <KIND>	KIND ∈ footprints/tracks/vias/zones/drawings/nets
pcb query zone <board> (--uuid U | --name N | --net NET --layer LAYER)	Single zone: uuid, name, net, layer, priority, settings, polygon points, bbox, area_mm2 (shoelace outline area, mm²). Mutex selectors; --layer required with --net
pcb query via <board> (--uuid U | --at X,Y [--tolerance MM])	Single via: uuid, at, size, drill, layers, net, free, locked. --at returns the unique via within tolerance (default 0.05 mm); multiple matches return ambiguous with candidates

Edit (structural mutations)

Positional <schematic.kicad_sch> / <board.kicad_pcb>. Text summary by default (dry-run also prints a unified diff); supports --dry-run. --format json for the structured payload.

Command	Purpose
sch edit symbol add <sch> <LIB_ID> <REF> <X,Y> [--lib-file PATH]	Add a symbol instance. If <LIB_ID> is already in the schematic's embedded (lib_symbols ...), clones an existing same-lib_id sibling (must be annotated, unmirrored, unit-1) and inherits its Value/Footprint/rotation/on_board/in_bom. Otherwise, with --lib-file <library.kicad_sym>, imports the symbol definition into (lib_symbols ...) and synthesizes a fresh instance (works for pinless symbols like Mechanical:MountingHole and for top schematics with empty (lib_symbols)). Adjust Value/Footprint/attributes afterwards with set-property / set-attribute.
sch edit symbol move <sch> <REF> <X,Y> [--rotation R]	Move/rotate a symbol
sch edit symbol move-property <sch> <REF> <KEY> <X,Y> [--rotation R]	Move a property field
sch edit symbol add-pin <sch> <LIB_ID> <NUMBER> <NAME> <X,Y> --length L --type T [--rotation R] [--shape S] [--lib-file PATH]	Add a pin (updates embedded lib_symbols + .kicad_sym)
sch edit symbol delete <sch> <REF>	Delete a symbol; reports connected taps but does not remove them
sch edit symbol set-property <sch> <REF> <KEY> <VALUE>	Set any property (built-in or user-defined: MPN/LCSC/Manufacturer/...)
sch edit symbol set-attribute <sch> <REF> <in_bom|on_board> <yes|no>	Set a schematic symbol boolean attribute; use on_board no for off-board BOM parts
sch edit wire add <sch> <X1,Y1> <X2,Y2> [--type solid|default]	Add a wire segment
sch edit wire delete <sch> <UUID>	Delete a wire
sch edit label add <sch> <KIND> <NAME> <X,Y> [--rotation R]	KIND ∈ global/hier/local
sch edit label move <sch> <UUID> <X,Y> [--rotation R]	Move a label
sch edit label delete <sch> <UUID>	Delete a label
sch edit junction add <sch> <X,Y>	Add a junction
sch edit junction delete <sch> <UUID>	Delete a junction
pcb edit footprint move <board> <REF> <X,Y> [--rotation R]	Move/rotate a footprint
pcb edit footprint move-property <board> <REF> <KEY> <X,Y> [--rotation R]	Move a property field
pcb edit footprint set-property <board> <REF> <KEY> <VALUE>	Set a property (refuses Reference — use schematic + pcb sync)
pcb edit footprint move-layer <board> <REF> front|back [--at X,Y] [--rotation R]	Flip to F.Cu / B.Cu (mirrors geometry, preserves property positions)
pcb edit zone set-polygon <board> (--uuid U | --name N | --net NET --layer LAYER) <X1,Y1> <X2,Y2> <X3,Y3> [...]	Replace a zone's outline polygon (≥3 points). Strips stale (filled_polygon ...) (KiCad refills). Rejects degenerate polygons (zero area, consecutive duplicate points)
pcb edit zone add <board> <NET> <LAYER> <X1,Y1> <X2,Y2> <X3,Y3> [...] --copy-settings-from-uuid U	Add a new zone, inheriting settings (hatch/connect_pads/clearance/min_thickness/fill/thermal) from an existing zone. Net and layer must already exist. --name, --priority optional overrides. Secondary path: explicit settings flags instead of --copy-settings-from-uuid
pcb edit zone delete <board> (--uuid U | --name N | --net NET --layer LAYER)	Delete a zone block entirely. Tracks/vias/other zones untouched
pcb edit zone set-property <board> (--uuid U | --name N) <priority|clearance|min_thickness|thermal_gap|thermal_bridge_width|name> <VALUE>	Edit a single zone setting (KEY whitelisted). Strips (filled_polygon ...) after mutation
pcb edit via add <board> <NET> <X,Y> [--size MM] [--drill MM] [--layers F.Cu,B.Cu] [--free]	Add a new via. Net must exist. Defaults size/drill from board (setup) (via_size/via_drill), else 0.8/0.4. UUID is deterministic from (net,xy,layers) — re-adding the same triple is idempotent
pcb edit via delete <board> (--uuid U | --at X,Y [--tolerance MM])	Delete a single via by uuid or nearest position. Multiple candidates within tolerance → error
pcb edit via move <board> (--uuid U | --at X,Y [--tolerance MM]) <NEW_X,NEW_Y>	Move a via. Only (at ...) is rewritten; size/drill/net/layers/uuid unchanged
pcb edit via set-property <board> (--uuid U | --at X,Y [--tolerance MM]) <size|drill|net|layers|free|locked> <VALUE>	Set a single via field (KEY whitelisted). layers is comma-separated; free/locked accept yes/no/true/false/0/1; net is name-validated

Locked footprints are refused. Only the targeted block is rewritten; UUIDs and surrounding formatting are preserved.

Inspect / Validate JSON

sch inspect (and sch validate's nested inspect key) returns:

• score — nested object, not a number. Access as score.total, score.collision_count, etc. Sub-fields:
  • total (lower better), collision_count
  • wire_hits, component_hits, text_hits, collision_area
  • wire_corner_count / wire_corner_penalty (two-segment bends + wire-endpoint T-junctions)
  • diagonal_wire_count / diagonal_wire_penalty
  • symbol_wire_conflict_count / symbol_wire_penalty (wires crossing symbol bodies)
  • symbol_wire_clearance_count / symbol_wire_clearance_penalty (wires too close to symbols)
  • symbol_wire_edge_hug_count / symbol_wire_edge_hug_penalty
• wire_length — total length, segment count, longest segment (non-score metric).
• collisions — text/label/property/wire/symbol records.
• symbol_wire_conflicts — body overlaps + clearance violations.
• filters — applied only_text, margin.

sch validate wraps three stages: { "erc": {...}, "netlist": {...}, "inspect": {...} }. Read score/collisions through d["inspect"]["score"], not the top level.

Scripts

• scripts/kicad_tool.py — module behind the kicad-tool console script (do not invoke directly).
• scripts/score_schematic.py, scripts/kicad_sch_bbox_collisions.py, scripts/text_collision_core.py — import-only helpers.