GF-PCB — KiCad Schematic & PCB Generation

Tool Detection

which kicad-cli

If not found:

---GATEFLOW-RESULT---
STATUS: ERROR
DETAILS: KiCad not installed. Install for PCB design.
  macOS: brew install --cask kicad
  Linux: sudo apt install kicad
  Download: https://www.kicad.org/download/
---END-GATEFLOW-RESULT---

Workflow

1. Parse request — What board? Components? Constraints?
2. Web search — Reference designs, datasheets, footprints
3. Spawn pcb-designer agent — Generate schematic + PCB
4. Run verification loop: a. KiCad DRC (Design Rule Check) b. KiCad ERC (Electrical Rule Check) c. AI Review (power, decoupling, floating pins, voltages) d. If errors → fix and re-verify (max 3 iterations)
5. Label output with verification status and confidence
6. Deliver with mandatory disclaimer

Output Files

project/
├── schematic.kicad_sch     # Schematic (S-expression)
├── board.kicad_pcb         # PCB layout
├── bom.csv                 # Bill of materials
└── verification_report.md  # DRC/ERC/AI review results

Result Format

---GATEFLOW-RESULT---
STATUS: PASS | FAIL | ERROR
CONFIDENCE: high | medium | low
VERIFICATION:
  DRC: PASS/FAIL (N errors, M warnings)
  ERC: PASS/FAIL (N errors, M warnings)
  AI_REVIEW: PASS/FAIL (N/M checks passed)
FILES: [generated files]
DETAILS: [summary]
---END-GATEFLOW-RESULT---

KiCad CLI Quick Reference

# DRC
kicad-cli pcb drc --format json --severity-all --exit-code-violations --output drc.json board.kicad_pcb

# ERC
kicad-cli sch erc --format json --severity-all --exit-code-violations --output erc.json design.kicad_sch

# BOM
kicad-cli sch export bom --fields "Reference,Value,Footprint,${QUANTITY},Manufacturer,MPN" \
  --group-by "Value,Footprint" --exclude-dnp --output bom.csv design.kicad_sch

# Gerbers + Drill
kicad-cli pcb export gerbers --output gerbers/ board.kicad_pcb
kicad-cli pcb export drill --output gerbers/ --format excellon board.kicad_pcb

# 3D Model
kicad-cli pcb export step --output board.step board.kicad_pcb

Exit codes: 0 = clean, 5 = violations found.

DRC/ERC Interpretation

Common DRC Errors

Error	Meaning	Fix
clearance_violation	Items too close	Increase spacing
shorting_items	Different nets touching	Reroute traces
courtyards_overlap	Components too close	Move apart
track_width	Outside allowed range	Adjust width
annular_width	Via ring too small	Increase via size
copper_sliver	Thin copper (mfg risk)	Adjust pour
hole_near_hole	Drilled holes too close	Increase spacing

Common ERC Errors

Error	Fix
Input power pin not driven	Add PWR_FLAG
Pin not connected	Connect or add no-connect X
Conflicting pin types	Check symbol pin types
Duplicate reference	Re-annotate schematic

AI Review Checklist

Decoupling

• Every IC: 100nF cap within 5mm of power pins
• Bulk caps near power entry
• Current path: Supply -> Cap -> IC pin

Power

• Continuous ground plane
• No signal traces cutting ground under high-speed signals
• Adequate copper weight for current

High-Speed

• Controlled impedance for >50MHz signals
• Length matching for differential pairs
• Via stitching along high-speed paths

Thermal

• Thermal vias under exposed pads (min 4-9)
• Heat sources away from temp-sensitive components

Manufacturing

• Board outline closed on Edge.Cuts
• Min trace >= 0.1mm, min drill >= 0.2mm
• Silkscreen not over pads
• Fiducials present (min 3)

Confidence Scoring

Level	Criteria	DRC Expectation
HIGH	<50 components, 2-layer, <10MHz	Zero violations
MEDIUM	50-200 components, 2-4 layer, <100MHz	May need adjustments
LOW	>200 components, 4+ layers, high-speed/RF/power	Expert review required

Override to LOW if: RF/antenna, DDR/PCIe/USB3+, SMPS >5W, BGA >100 pins.

Manufacturing Package Script

mkdir -p output/{gerbers,assembly,docs}
kicad-cli pcb export gerbers --output output/gerbers/ board.kicad_pcb
kicad-cli pcb export drill --output output/gerbers/ --format excellon board.kicad_pcb
kicad-cli pcb export pos --format csv --output output/assembly/positions.csv board.kicad_pcb
kicad-cli sch export bom --exclude-dnp --output output/assembly/bom.csv design.kicad_sch
kicad-cli sch export pdf --output output/docs/schematic.pdf design.kicad_sch
kicad-cli pcb export step --output output/docs/board.step board.kicad_pcb