kicad-gen

When to Use

• BGA/QFN devices with 100+ pins -- manual placement is error-prone
• Multi-sheet designs where repetitive structure can be scripted
• Pin maps derived from datasheet tables or CSV (auto-assign ball-to-net)
• Schematic must stay synchronized with a separate spec or pin database

Workflow

1. Define components and pin maps in design.yaml
2. Generate sheets   -> circuit-weaver generate
3. Require real ERC  -> circuit-weaver generate --require-kicad
4. Review in KiCad   -> open .kicad_sch files, run Update PCB from Schematic

Give each block a stable unique id and functional section. Circuit Weaver preserves explicit sections as separate sheets, keeps generated support parts with their owning block, and disambiguates sanitized sheet filenames. Read the root and child paths from artifact_manifest.json; never guess main.kicad_sch.

Project-Specific Setup

Spec: ${SPEC_PATH} Output directory: ${OUTPUT_DIR}

If a project supplies custom scripts, record their checked-in paths here. Do not invoke scripts/generate_schematics.py or scripts/pin_maps.py unless those files exist in the current project.

Edit this file to record:

• Which ICs are generated vs hand-drawn
• Pin coverage per IC (total pins, mapped pins, no-connect pins)
• How to re-run generation after spec changes

KiCad Format Rules (Critical)

• _0_1/_1_1 sub-units REQUIRED -- SnapEDA flat format fails silently without them
• lib_id in schematic instances: bare names (no library: prefix)
• Power symbols: bare lib_id (e.g. "VCC" not "power:VCC"), (power) flag required
• 1.27mm grid: all pin endpoints, labels, wires must snap to round(val / 1.27) * 1.27
• Wire stubs REQUIRED between pins and labels -- labels at pin endpoints without wires do not reliably connect
• Version 20231120 (KiCad 8+) for per-symbol instances blocks

Regeneration Protocol

# Transactionally regenerate and require the exact final hierarchy to pass a
# real installed kicad-cli ERC run.
circuit-weaver generate "${SPEC_PATH}" --output "${OUTPUT_DIR}" --require-kicad

# Then in KiCad GUI: Tools -> Update PCB from Schematic

Read valid, kicad_verified, verification_status, and erc from artifact_manifest.json. Internal validation alone is not real KiCad verification. If --require-kicad cannot run or ERC fails, generation fails; do not claim release-quality artifacts.

Never hand-edit generated .kicad_sch files -- changes will be overwritten on next generation.

Pin Coverage Tracking

IC	Total pins	Mapped	No-connect	Coverage
(fill in)

Common Issues

Silent connection failure: Labels placed directly on pin endpoints without a wire stub. Fix: generate wire + label pairs, not label-only.

PCB import failure: Version mismatch -- KiCad 7 expects root-level symbol_instances; KiCad 8+ uses per-symbol instances blocks. Use version 20231120 for KiCad 8+ compatibility.

Symbol not recognized: SnapEDA flat format lacks _0_1/_1_1 sub-unit notation. Rebuild the symbol from scratch using the KiCad S-expression format.