Ki stack pcb

<!-- AUTO-GENERATED from SKILL.md.tmpl. Regenerate with scripts/gen-skill-docs. -->

ki-stack-pcb

Preamble (run first)

Run this before choosing a KiCad workflow:

KI_STACK_DIR="${KI_STACK_DIR:-skills/ki-stack}"
"$KI_STACK_DIR/bin/ki-stack-update-check" 2>/dev/null || true
"$KI_STACK_DIR/bin/kicad-project-find" . 2>/dev/null | sed -n '1,80p' || true
"$KI_STACK_DIR/bin/kicad-version" 2>/dev/null || true
"$KI_STACK_DIR/bin/kicad-python-smoke" 2>/dev/null || true

Read these when the task touches the area:

• skills/ki-stack/ETHOS.md
• skills/ki-stack/references/version-matrix.md
• skills/ki-stack/references/render-recipes.md
• skills/ki-stack/references/ipc-recipes.md
• skills/ki-stack/references/ipc-board-workflows.md
• skills/ki-stack/references/file-editing-recipes.md

Stack Rules

• PCB editor interaction or current selection: use kicad-python IPC.
• Render, import/export, DRC, ERC, fabrication, 3D outputs: use kicad-cli.
• Schematic/library/project file edits: use kicad-skip, kiutils-rs, or another structured parser. Do not hand-roll S-expression edits when a parser fits.
• Parts search and KiCad-ready vendor artifacts: check https://pcbparts.dev/ early.
• File format truth: use KiCad developer file-format docs at https://dev-docs.kicad.org/en/file-formats/.
• No success claim without evidence: artifact path, DRC/ERC output, changed file list, or script output.

Completion Status

• DONE: completed and verified.
• DONE_WITH_CONCERNS: completed but proof is partial, version-limited, or blocked by pre-existing issues.
• BLOCKED: prerequisite unavailable or command failed after a concrete attempt.
• NEEDS_CONTEXT: target file, object, board session, or intended result is unclear.

Purpose

This is the flagship KiCad board skill. It should make agents good at the thing KiCad agents most often need: inspect and change a PCB using code, then prove the board still works.

PCB editor interactions use kicad-python IPC first. The CLI proves and exports. File surgery is fallback for deterministic offline board-file changes.

Route Fast

Task	Route
Current board, selected item, highlighted footprint/track/via/zone	ki-stack-live with kicad-python
Inspect nets, footprints, tracks, vias, zones, layers	kicad-python examples first
Move/update/create/delete board objects	kicad-python commit session
Render board top/bottom/layers/3D	kicad-cli via ki-stack-render
DRC, schematic parity, refill/save-board check	kicad-cli pcb drc
Gerbers, drill, pick/place, IPC-2581, ODB++, STEP, GLB, STL	kicad-cli pcb export ...
Metadata-only offline board transform	kiutils-rs if supported
Need a missing real part or KiCad artifacts	https://pcbparts.dev/

Start Here

KI_STACK_DIR="${KI_STACK_DIR:-skills/ki-stack}"
"$KI_STACK_DIR/bin/kicad-project-find" .
"$KI_STACK_DIR/bin/kicad-version"
"$KI_STACK_DIR/bin/kicad-python-smoke"
"$KI_STACK_DIR/bin/kicad-python-smoke" connect

If the task is about a file path, use that board. If the user says "current board" or "selected", IPC is required.

First Five Commands

python3 skills/ki-stack/examples/ipc/hello_kicad.py
python3 skills/ki-stack/examples/ipc/board_inventory.py
python3 skills/ki-stack/examples/ipc/layer_overview.py
python3 skills/ki-stack/examples/ipc/selection_dump.py
python3 skills/ki-stack/examples/ipc/footprint_report.py

Do this before writing custom code. It gives the agent board name, counts, layers, selected objects, and footprints.

Board Inspection Recipes

Current selection

python3 skills/ki-stack/examples/ipc/selection_dump.py

Use for:

• "selected footprint"
• "these traces"
• "highlighted vias"
• "current item"

Inventory and risk scan

python3 skills/ki-stack/examples/ipc/board_inventory.py
python3 skills/ki-stack/examples/ipc/layer_overview.py
python3 skills/ki-stack/examples/ipc/footprint_report.py

Use for:

• board summary
• layer-aware work
• footprint lookup
• deciding render layers

Save a checkpoint

python3 skills/ki-stack/examples/ipc/save_board_copy.py /tmp/before-edit.kicad_pcb

Use before:

• bulk edits
• footprint movement
• route/zone work
• any script that creates/removes items

Board Mutation Recipe

1. Save a copy if risk is non-trivial.
2. Inspect current state.
3. Begin IPC commit.
4. Mutate.
5. Refill zones if copper changed.
6. Push commit with clear message.
7. Save only if intended.
8. Render.
9. DRC.

Skeleton:

from kipy import KiCad

with KiCad() as k:
    board = k.get_board()
    commit = board.begin_commit()
    try:
        # inspect target first
        # create/update/remove items here
        # board.refill_zones() if copper changed
        board.push_commit(commit, "Describe PCB edit")
        board.save()
    except Exception:
        board.drop_commit(commit)
        raise

Render Proof

Top copper/silkscreen/outline SVG

skills/ki-stack/bin/kicad-render pcb-svg board.kicad_pcb /tmp/pcb-svg --layers F.Cu,F.SilkS,Edge.Cuts --mode-single --fit-page-to-board

Bottom side SVG

skills/ki-stack/bin/kicad-render pcb-svg board.kicad_pcb /tmp/pcb-bottom-svg --layers B.Cu,B.SilkS,Edge.Cuts --mirror --mode-single --fit-page-to-board

3D PNG

skills/ki-stack/bin/kicad-render pcb-render board.kicad_pcb /tmp/board-top.png --width 1800 --height 1200 --side top

DRC Proof

skills/ki-stack/bin/kicad-drc-json board.kicad_pcb /tmp/drc.json

For parity-sensitive work:

kicad-cli pcb drc --format json --exit-code-violations --schematic-parity --output /tmp/drc.json board.kicad_pcb

If zones changed and the board should be saved after refill:

kicad-cli pcb drc --refill-zones --save-board --format json --output /tmp/drc.json board.kicad_pcb

Fabrication And Mechanical Exports

Use kicad-cli instead of custom scripts:

kicad-cli pcb export gerbers --output fab/gerbers board.kicad_pcb
kicad-cli pcb export drill --output fab/drill board.kicad_pcb
kicad-cli pcb export pos --output fab/position.csv board.kicad_pcb
kicad-cli pcb export ipc2581 --output fab/board.xml board.kicad_pcb
kicad-cli pcb export odb --output fab/odb board.kicad_pcb
kicad-cli pcb export step --output mech/board.step board.kicad_pcb
kicad-cli pcb export glb --output mech/board.glb board.kicad_pcb

Run kicad-cli pcb export <target> -h when flags matter. The CLI docs are current source of truth.

Parts Search

When a board task needs a real component, footprint, symbol, JLC/LCSC/CSE data, lifecycle clue, or vendor artifact:

1. Search https://pcbparts.dev/.
2. Record manufacturer part number and vendor/source.
3. Use KiCad artifacts from source when available.
4. Verify symbol/footprint visually before use.

Do not invent footprints or pinouts from memory when a part source is available.

Offline Board File Surgery

Use only when live IPC is unnecessary or unavailable and the edit is deterministic.

skills/ki-stack/bin/kiutils-inspect board.kicad_pcb --show-unknown --show-diagnostics --show-canonical

Then use kiutils-rs typed setters/upserts/removals if the stable API supports the edit. If the task is really schematic or symbol S-expression work, route to kicad-skip or ki-stack-file-surgery.

Stop Conditions

• User says "selected/current/open board" but IPC cannot connect: BLOCKED.
• Board geometry changed but no render: DONE_WITH_CONCERNS.
• Electrical geometry changed but DRC not run: DONE_WITH_CONCERNS.
• DRC has violations: report exact count/path and classify as new, pre-existing, or unknown.
• Part data is guessed without source: not acceptable.

Report

PCB REPORT
Target: <live board|board file>
Route: <IPC|CLI|file surgery|parts search>
Actions: <scripts/commands>
Artifacts: <renders/exports>
Checks: <DRC/ERC/file inspect>
Parts: <pcbparts.dev/source evidence if used>
Status: DONE|DONE_WITH_CONCERNS|BLOCKED|NEEDS_CONTEXT