codejunkie99 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
- Parse request — What board? Components? Constraints?
- Web search — Reference designs, datasheets, footprints
- Spawn pcb-designer agent — Generate schematic + PCB
- 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)
- Label output with verification status and confidence
- 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