Skip to content

AvatarSD/KiSkill / skills/kicad-schematic

kicad-schematic

Verified

Generate and modify KiCad schematics (.kicad_sch) and PCBs (.kicad_pcb) programmatically, with geometric verification, headless ERC, and rendered visual inspection. Use when asked to draw/implement/extend a schematic, inject circuit blocks into an existing KiCad project, stage footprints on a PCB, or verify schematic wiring/rotation. Trigger phrases: "draw in kicad", "create schematic", "implement schematic", "add to the schematic", "kicad_sch", "footprints on the pcb".

KiCad schematic generation

Engine: $(kx root)/kicad_lib/ — lossless sexp parser (sexp.py, token-equal round-trip proven on 2.3 MB boards; byte-identity only for .kicad_mod — sch re-serializes with ~0.5% whitespace drift) and the kx CLI (python3 -m kicad_lib.cli probe|check FILE from the repo root). Prefer kx probe over ad-hoc grep for inventory; prefer sexp.py over regex surgery for edits (kx is on PATH via ~/.local/bin). Persist with sexp.save_file(path, root) — PATH FIRST. Python imports need PYTHONPATH= or cwd=; the package is not pip-installed. Sibling skills: kicad-project (state machine), kicad-component (find/fetch parts), kicad-review (diff/ERC), kicad-improve (self-improvement loop). Design: doc/DESIGN.md in that repo.

Battle-tested workflow for writing .kicad_sch/.kicad_pcb files from Python without KiCad GUI. The engine and worked examples ship in this repo (kx root):

  • kicad_lib/ops.py — standalone sheet, scaffold symbols, full-wire layout, driven by the built-in geometric verifier (kicad_lib/verify.py).
  • kicad_lib/live_ops.py — inject a block into an EXISTING schematic using real library symbols (extends-flattening, multi-unit parts, mirrors), label-stitched islands.
  • kicad_lib/pcb.py — stage footprints in the PCB, path-linked to schematic symbols so Update-PCB adopts them. See tests/test_*.py for runnable end-to-end usage against tests/fixtures/.

0. The loop (never skip a stage)

  1. Probe target file + libraries (uuids, pin geometry, occupancy, refs).
  2. Generate with explicit coordinates; run the geometric verifier.
  3. ERC headless; compare against a baseline run as a violation set.
  4. Render SVG → PNG → look at it. Geometry that passes checks can still be unreadable (text collisions, symbol overlap). Iterate.
  5. Commit per slice. Checkpoint-commit the project BEFORE first modification.

1. Environment

KiCad 10 is a flatpak (org.kicad.KiCad); there is no host kicad-cli:

flatpak run --command=kicad-cli org.kicad.KiCad sch erc --output erc.rpt --severity-error FILE.kicad_sch
flatpak run --command=kicad-cli org.kicad.KiCad sch export svg --output OUTDIR --no-background-color FILE.kicad_sch
flatpak run --command=kicad-cli org.kicad.KiCad sch export netlist --output out.net FILE.kicad_sch
flatpak run --command=kicad-cli org.kicad.KiCad pcb export svg --output out.svg --layers F.Cu,B.Cu,Edge.Cuts,F.SilkS FILE.kicad_pcb
  • Flatpak /tmp is sandboxed — outputs must land under $HOME.
  • Official libs: ~/.local/share/flatpak/runtime/org.kicad.KiCad.Library.Symbols/x86_64/stable/active/files/symbols/*.kicad_sym ~/.local/share/flatpak/runtime/org.kicad.KiCad.Library.Footprints/x86_64/stable/active/files/footprints/*.pretty/*.kicad_mod
  • Rasterize SVG with cairosvg (installed), crop with PIL, then Read the PNG.
  • If a project lock file (~NAME.kicad_pro.lck) exists, KiCad is open — warn the user to close/reload before and after edits.

2. File format essentials (.kicad_sch, format 20260306, generator "eeschema" 10.0)

Top-level order: (kicad_sch (version) (generator) (generator_version) (uuid) (paper) (lib_symbols ...) <junctions/wires/labels/symbols/sheets> (sheet_instances ...) (embedded_fonts no)). Order of body items is loose.

  • Preserve the existing file uuid (it's the root sheet uuid; instance paths reference it). For a sub-sheet keep the uuid KiCad created.
  • Every placed symbol needs (instances (project "NAME" (path "/<ROOT_UUID>" (reference "R1") (unit 1)))). Sub-sheet instance paths are /<root_uuid>/<sheet_symbol_uuid>.
  • lib_symbols is a cache of full symbol definitions named "Lib:Name". Wires connect ONLY at exact pin endpoints — geometry comes from the cache.
  • Wire: (wire (pts (xy x1 y1) (xy x2 y2)) (stroke (width 0) (type default)) (uuid ...)). Junction: (junction (at x y) (diameter 0) (color 0 0 0 0) (uuid ...)).
  • Labels: local (label "net" (at x y rot) ...), global (global_label "net" (shape input|output) ...), hierarchical (hierarchical_label ...) (sub-sheets only; on a root sheet use local/global).
  • Paren-balance check before writing; strings may contain parens — the balanced extractor must be quote-aware.

3. Coordinates, rotation, mirror

World coords: mm, +Y down. Library pin coords: +Y up. Everything (symbol origins AND wire endpoints) must sit on the 1.27 mm grid or wires will not connect.

Pin world position for a symbol at (x, y, rot), lib pin offset (u, v):

def rot_xy(u, v, rot, mirror=""):        # = kicad_lib.geom.rot_xy
    x, y = {0: (u, -v), 90: (-v, -u), 180: (-u, v), 270: (v, u)}[rot]
    if mirror == "x": y = -y            # mirror AFTER rotation, in WORLD axes
    if mirror == "y": x = -x            # (proven vs a kicad-cli netlist)
    return (x, y)
# world = (x + dx, y + dy)

KiCad may re-save rot 90 + mirror y as the equivalent rot 270 + mirror x.

  • Device:R is vertical at rot 0 (pin1 top); rot 90 → pin1 left.
  • KiCad PNPs draw emitter at bottom; (mirror x) flips it up (idiomatic).
  • Property text angle is RELATIVE to symbol rotation — for a rot-90/270 symbol set property angle 90 so the text renders horizontal.
  • Real symbol heights differ from scratch-built ones — transistor circles are ~11 mm; totem pairs need ≥15.24 mm center spacing.

4. Sourcing symbols

Real library symbols (preferred — "select real components"):

  • Extract (symbol "NAME" ...) blocks from the lib with a balanced parser.
  • Resolve (extends "BASE"): take the base body, apply the derived symbol's property overrides, rename BASE_X_Y sub-units to NAME_X_Y, then prefix the top name to "Lib:NAME" for the cache.
  • Cache Value property must equal the bare symbol name, else ERC reports lib_symbol_mismatch against the configured library.
  • Parse pin positions per unit from (pin ... (at x y a) ... (number "N")).
  • Multi-unit parts (LM393 = unit1 A, unit2 B, unit3 power): one reference, several (symbol ...) instances each with its own (unit N); all units carry identical properties. One dual comparator serves two channels.
  • Watch coincident pins (e.g. DMP3013SFV has 3 drain pins at one point — all get the same net, emit all pin uuid entries).

Scaffold symbols (standalone sheets / quick drafts): define your own minimal R/C/Q/M/opamp boxes in lib_symbols so pin geometry is fully under your control. Sub-unit names inside a definition are bare ("R_0_1", never "lib:R_0_1"). Power symbol header is (power global). If KiCad will open the project standalone, also emit scaffold.kicad_sym + a project sym-lib-table entry (URI ${KIPRJMOD}/scaffold.kicad_sym) or ERC warns.

5. Placement and routing

  • Describe nets as polylines of waypoints, where a waypoint is either a literal point or ("ref","pin"); consecutive points become axis-parallel wire segments. Skip zero-length segments.
  • Full wires for a self-contained sheet; label-stitched islands (driver island / power island / comparator island joined by short local labels) when injecting into a crowded page — labels merge nets with the existing drawing (out1, Vin_p, VCC...) for free.
  • Probe free space BEFORE placing: collect (at ...)/(xy ...) coords into a coarse occupancy grid — but remember it misses label TEXT extents and sheet boxes; always confirm against a render. Probe (sheet (at)(size)) blocks explicitly. Title block ≈ bottom-right 110×30 mm — keep clear.
  • If the page is full, grow the paper (A4 → A3); existing content keeps coordinates.
  • T-junctions: a wire endpoint or pin touching another wire's interior DOES connect; emit a (junction ...) there. Pins may sit pin-on-pin or pin-on-wire-interior — both connect.
  • GND/VCC: one power:GND/power:VCC symbol per drop, short stub wire to the pin. Standalone sheets need one PWR_FLAG (power_out pin) on each passive-driven rail or ERC raises power_pin_not_driven.

6. Geometric verifier (run before every write)

Implemented: kicad_lib/verify.py (Seg/Pin/verify()) + kicad_lib/geom.py (rot_xy, pin_world, snap) — mutation-tested by tests/test_verify.py. Build your net model with these; do NOT rewrite the verifier per-generator.

Mandatory checks over all generated segments + pins:

  1. Everything on the 1.27 mm grid; no diagonal segments.
  2. No two segments of DIFFERENT nets may touch, cross, T-touch, or overlap collinearly (treat all GND*/VCC* stub nets as one net each).
  3. Same-net collinear overlap (double-draw) and same-net crossing without a shared endpoint are errors too.
  4. No pin of net A lying on a wire of net B.
  5. Every declared pin claimed by exactly one net; every label anchor on a segment of its net.
  6. (Scaffold symbols) no wire through a symbol body bbox.
  7. Junction emission: ≥3 connection items at a point, or endpoint/pin on a same-net segment interior.

Float hygiene: round(coord, 3) everywhere — 160.02 + 7.62 produces 167.64000000000001 which the clash checks will flag against 167.64. Mutation-test the verifier once (plant a crossing, expect failure).

7. References and ERC

  • References are global across ALL sheets of a project. Collision-check against every .kicad_sch in the project dir, not just the target file. Duplicate refs silently cross-merge multi-unit symbols and corrupt ERC.
  • GOTCHA: kicad-cli sch erc does NOT catch duplicate designators or unannotated symbols (R?) — even at --severity-all. They are Annotation-tool checks (SCH_REFERENCE_LIST), not ERC violations, so a headless ERC pass stays 0/0 green while two R1s cross-merge. Verify refs with kx ref-audit FILE (multi-unit aware: U1A/U1B/U1C sharing U1 is fine; a repeated unit or two lib_ids on one ref is the real dup) or the GUI Annotate dialog — never trust headless ERC for annotation.
  • #PWR0NNN refs: pick an unused high block.
  • ERC totals are noisy. Always: run ERC on the pre-edit baseline (git show HEAD:file > baseline.kicad_sch), normalize each violation to type: @locations, and set-diff new vs baseline. Judge only the NEW entries; report regrouping moves pre-existing items around.
  • Expected-benign classes: isolated_pin_label on block I/O, undriven inputs awaiting later wiring, pre-existing unwired-MCU noise.
  • missing_unit/missing_input_pin: EVERY unit of a multi-unit part (dual/quad opamp, gate pack) must be placed, AND a spare you don't use still goes on a sheet + tied off (opamp: in+ → GND, in− → out; logic: inputs to a defined level) or its inputs throw missing_input_pin. kx unit-audit FILE lists placed-vs-expected units per ref (reads the count from lib_symbols) and front-runs ERC; ERC is the authority on tie-off. (kicad.info unused-pin threads; KLC S4.5)
  • No-connect discipline: a genuinely unused pin needs a (no_connect …) flag to silence pin_not_connected — DOCUMENT the intent, never lower severity. Inverse trap no_connect_connected: a NC flag on a pin/node that IS wired (flag and wiring contradict) — delete the flag OR the wire, not both. NC means "nothing else attaches here"; one ERC entry lands at the flag, one at the connected pin. (kicad.info t/46229, t/21294)
  • The exported netlist is the ground truth for connectivity: parse (net (name)(node (ref)(pin))) blocks and assert each designed net has exactly the expected members. Do this at least once per block.
  • power_pin_not_driven ("Input power pin not driven by output power pins") is a missing DRIVER DECLARATION, not a wiring fault. Each power/ground rail needs one driver: a power_out pin (regulator) OR a power:PWR_FLAG. Fix by adding PWR_FLAG — NOT a ground symbol like PWRGND (name trap: PWRGND is just a GND graphic; PWR_FLAG declares the net driven) — at the rail's PASSIVE source (connector / battery / regulator INPUT). Never flag a regulator OUTPUT (already power_out; flagging it can trip "two outputs"). One flag per rail.
  • GOTCHA: kicad-cli sch export netlist drops PWR_FLAG and power-symbol nodes, so a flagged and a flag-stripped schematic have IDENTICAL netlist driver content (both zero power_out) — the netlist cannot see this class of error. NEVER audit power drivers from the netlist; use kx power-audit FILE (reads PWR_FLAG instances from the schematic) plus kicad-cli ERC (the authority). (kicad.info t/35552, t/57016)

8. Visual inspection (non-negotiable)

flatpak run --command=kicad-cli org.kicad.KiCad sch export svg --output svg_out --no-background-color FILE.kicad_sch
python3 -c "import cairosvg; cairosvg.svg2png(url='svg_out/FILE.svg', write_to='out.png', output_width=2600)"
# crop: px = x_mm/paper_w*img_w (A4 297x210, A3 420x297), then Read the PNG

Look for: symbol body overlap, value/ref text collisions (move per-ref via a TEXT_POS override table), labels overlapping existing drawing text, junction dots present, pins facing their wires. Fix and re-render until clean. Matplotlib net-colored previews of the segment model help debug the generator, but only the KiCad render proves the file.

9. Injecting into an existing schematic

  • Checkpoint-commit first; idempotency = git checkout -- file then rerun the generator (uuids regenerate — re-derive anything uuid-dependent after).
  • Splice lib symbols right after (lib_symbols, body before (sheet_instances; skip lib defs already cached.
  • Reuse existing nets by label name (out1, Vin_p, VCC) and existing cached symbols (e.g. the project's own cap symbol) where possible.
  • Bind MCU pins by adding a 5.08 mm stub wire + local label at the pin endpoint (get pin world pos from the cached MCU symbol + instance (at)). Only bind pins the design doc justifies; leave the rest to the user.

10. PCB footprint staging (.kicad_pcb)

Goal: place footprints so KiCad's Update PCB from Schematic adopts them (no duplicates) and fills nets:

  1. Export the netlist; for each ref take (tstamps "<uuid>") from its (comp ...) block — that uuid IS the link.
  2. Load .kicad_mod, take the balanced (footprint ...) block, rename to "Lib:Name", strip (version)/(generator*) headers, insert after the layer clause: (uuid), (at X Y), (path "/<tstamp-uuid>"), (sheetname "/"), (sheetfile "..."); set Reference/Value properties; refresh all item uuids. Leave pads netless — sync fills them.
  3. Stage in a grid clear of the board outline (probe Edge.Cuts extent).
  4. Parse-check via pcb export svg, render, eyeball, commit.

11. Live IPC editing (KiCad v11 nightly, GUI open)

KiCad 10 has NONE of this for schematics: kx env → backends.ipc.sch = list-only (10.0.7, standalone and project manager alike: no get_items, every schematic item type rejected on create/update, no save/revert/run_action — live.sch_capabilities() measures it per server). On 10, an open generated schematic is updated with §12's live regeneration instead. Also: the .venv's kipy 0.8.0 ships a kipy.schematic layer that does not import against its own protos — the code below needs the master bootstrap.

When kx env reports ipc_alive: true + scope pcb+sch, edit the schematic INSIDE the running eeschema instead of the file (the file is LOCKED then — never write it). kipy master via repo .venv (bootstrap: tools/bootstrap_kipy.sh); worked example tests/test_live_ipc.py:

from kipy import KiCad
import kipy.schematic_types as st
from kipy.geometry import Vector2          # nanometers: mm * 1e6
k = KiCad(socket_path="ipc:///tmp/kicad/api.sock")
sch = k.get_schematic()                    # the OPEN document
refs = [s.reference_field.text.value for s in sch.get_symbols()]
t = st.SchematicText(); t.value = "note"
t.position = Vector2.from_xy(50_800_000, 25_400_000)
c = sch.begin_commit(); sch.create_items(t); sch.push_commit(c, "msg")
  • Every push_commit is a single undo step in the GUI — small definitive steps map 1:1 onto user-visible, user-revertable edits.
  • remove_items() deletes live. get_lines/get_labels/get_text mirror reads.
  • PERSISTENCE GAP (nightly 10.99 standalone): save/revert are unhandled over IPC — the USER saves. Verify expected state on disk afterwards with kx probe / kx check. Full handler map: kicad-project skill.

kx live wraps this as VERIFIED atomic ops (kicad_lib/live_ops.py, worked example tests/test_live_ops.py — re-execs the .venv itself):

kx live snap                   inventory + violations (mm, with ids)
kx live check                  geometric verifier on the live model
kx live wire X1 Y1 X2 Y2       verify -> push or refuse (exit 1+JSON)
kx live junction X Y | label X Y TEXT | text X Y TEXT
kx live rm ID...               remove by KIID (from snap)

Net-blind gate: live backend sees wires not nets — grid/diagonal/zero/ overlap/T-junction checked; cross-net + pin rules only at file level after save. A refusal sends NOTHING (GUI never sees invalid state); a push is exactly one GUI undo step.

12. Generated schematics: hand edits survive regeneration

A gen script that rewrites .kicad_sch wipes the operator's GUI edits. kicad_lib/regen.py (kx regen) closes the loop — wire it into the script's build entry point:

  1. Session(project_dir, snap_dir, overrides.json); guard_locks() refuses while KiCad has ~*.lck files.
  2. absorb(sheets) diffs each sheet against its snapshot sidecar. Absorbed into overrides.json: symbol move/rotate/mirror, field move/hide/justify, value/footprint/property change/add/remove, flags (DNP, in_bom, ...), text-note and sheet-block moves. Re-hung (no loss): stubs/labels of a moved symbol, drag segments. Anything else (added wire/label/part, deleted part, renamed label, a power symbol's value) raises Refused and nothing is written; force=True discards those (listed) and still absorbs the rest.
  3. The generator asks overrides.symbol(sheet, "REF/UNIT"), places at geometry(ov) BEFORE hanging stubs, then apply_symbol(node, ov); records item owners (uuid → "REF/UNIT") and sym_state() of the script's own node as base; restamp(doc, seed, owners) just before each save (stable uuids: byte-identical reruns, symbol uuid = PCB footprint link kept); snapshot() after each save.
  4. connectivity(root) diffs the kicad-cli netlist against the last one — must be unchanged when only overrides were absorbed. report() lists value/footprint/DNP overrides as "move into the gen script" (the override prunes itself once the script says the same).

Bootstrap the first snapshots only from pristine (git-clean) generator output. CLI: kx regen status|absorb DIR SNAPDIR OVERRIDES [--force].

Live regeneration — the operator keeps the schematic OPEN

kicad_lib/live_sch.py turns step 1's refusal into save → regenerate → revert, so changes appear in the operator's open editor (same window):

kx live sch status --dir PROJ [--dir PROJ2]     # held projects + editors
kx live sch regen --dir PROJ [--host H] -- python3 gen/build_all.py

or in the gen script itself: with live_sch.session([dirs], host=H): generate() (Xena: build_all.py --live).

  1. SAVE each open schematic editor (its unsaved GUI edits reach the disk; verified by the "" leaving the window title). Cannot save (a dialog is open, the "" stays) → NotLive, NOTHING is written; fall back to the plain run (which then refuses on the lock).
  2. The generator runs with KX_REGEN_SAVED_BY=user@host,…; guard_locks() lets exactly those holders' locks through, so absorb reads the saved edits by the usual rules (refusals still refuse).
  3. REVERT the editors (File > Revert, confirmed) — when a sheet on disk changed, OR the editor was already stale (a git checkout/merge rewrote the sheets after it loaded them: each reload records the sheets' digest against the editor's lock in ~/.cache/kx/live_sch.json; no record + a sheet newer than the lock counts as stale). A revert that fails raises ReloadFailed: tell the operator to File > Revert before saving. kx live sch reload --dir PROJ does only this check + revert (after a merge, no generator needed). Non-modal frames (3D Viewer, library browsers, simulator) are not dialogs: they do not stop a live run.

KiCad 10 has no IPC for 1 and 3, so x11_editor.py types them into the editor's own window with xdotool (Xvfb, X11, or XWayland — the flatpak is an X11 client on Wayland too). The lock file names the editor's host: local is driven directly, another host over ssh HOST python3 - (needs xdotool + python3 THERE; --host overrides the ssh target). Revert returns the editor to the root sheet. A .kicad_pro the generator changes is NOT reloaded by Revert — say so (Xena's build_all warns). Proven headless: tests/test_live_sch_x11.py (both editor modes), hermetic logic: tests/test_live_sch.py.

13. Done checklist

  • Geometric verifier: 0 violations (and it failed when mutation-tested).
  • ERC set-diff vs baseline: no unexplained NEW entries.
  • Netlist spot-check: designed nets have exactly the expected members.
  • Rendered PNG inspected at readable zoom; no overlaps.
  • Refs unique across every sheet file in the project.
  • Paren balance + file written with original uuid/paper preserved.
  • Checkpoint commit before, one commit per slice after; scratch outputs (svg_out/, *.rpt, *.net, *.png) cleaned or ignored, never committed.
slack-gif-creatoranthropics/skillsKnowledge and utilities for creating animated GIFs optimized for Slack. Provides constraints, validation tools, and animation concepts. Use when users request animated GIFs for Slack like "make me a GIF of X doing Y for Slack."Stars: 198kUpdated Claude CodeCodexVerifiedInstall
ponytailDietrichGebert/ponytailLazy senior dev mode for any coding task: the smallest change that fully solves it, and a reply a busy human understands in one read.Stars: 196kUpdated Claude CodeCodexVerifiedInstall
ponytail-debtDietrichGebert/ponytailHarvest every shortcut: comment into one debt ledger, so deferrals get tracked instead of forgotten. One-shot report.Stars: 196kUpdated Claude CodeCodexVerifiedInstall
ponytail-debtDietrichGebert/ponytailList every `shortcut:` comment (and older `ponytail:` ones) as a debt ledger. One-shot report, changes nothing. Use for "ponytail debt", "what did ponytail defer", "list the shortcuts", /ponytail-debt.Stars: 196kUpdated Claude CodeCodexVerifiedInstall