pcbsight 0.5.1

PCB review built exclusively for AI agents: a .kicad_pcb in, exact connectivity/clearance/current findings out.

pcbsight

PCB review built exclusively for AI agents. A .kicad_pcb in; exact connectivity, clearance, current and pair findings out, with coordinates.

A layout is judged by eyeballing the copper. But an open net is a union-find question over copper that actually touches, a clearance is a segment-to-segment distance minus the widths, current capacity is IPC-2221 arithmetic at the net's narrowest point, and differential-pair skew is a subtraction. None of it needs eyes.

pip install "git+https://github.com/VortexJer/AISight#subdirectory=pcbsight"

pcbsight inspect board.kicad_pcb --clearance 0.15
# -> [FAIL] net 'GND' is 2 separate island(s) - unconnected pad(s): J1.2
# -> [FAIL] track-track: '+5V' to 'SIG' at 0.08 mm (required 0.15)
#           where: F.Cu near (28.75, 16.37)
# -> current: '+5V' min width 0.2 mm -> 0.746 A at dT=10 C (external)
# -> pair: USB_P / USB_N - skew 3.0 mm (~19.8 ps on FR4)
# -> out/board.png   (copper as drawn, findings circled in red)

pcbsight impedance 0.3 0.2      # ~51 ohm microstrip (IPC-2141 estimate)

Exit codes: 0 ok, 1 bad input, 2 a FAIL-level finding. Deterministic.

What it measures

connectivity	union-find over copper that geometrically touches (tracks by width, vias across layers, pads by extent): islands per net, the unconnected pads named
clearance	exact segment distances minus copper widths, per layer, different nets only; FAIL below 50 % of the rule (etch-short territory), warn above
current	IPC-2221 external/internal curve at the net's narrowest track, with copper weight and dT stated
diff pairs	found by net name (_P/_N, +/-, deduped); width match and length skew in mm and ~ps
impedance	IPC-2141 microstrip estimate, labelled an estimate

Footprint pads are composed through the footprint's placement — rotation included, because a pad's (at ...) is local and skipping the rotation silently misplaces every pad of every rotated footprint (test_rotated_footprint_pads_are_composed).

Proof it works: known ground truth

examples/01-board is a small 2-layer board generated twice: clean, and with four defects injected at exact magnitudes.

injected	measured
GND bottom trace stops 18.5 mm short of J1	[FAIL] net 'GND' is 2 separate island(s) ... unconnected pad(s): J1.2
SIG routed 0.08 mm from +5V	clearance 0.08 mm (exact), coordinates given
+5V necked to 0.2 mm	min width 0.2 mm -> 0.746 A (the 1.0 mm run: 2.39 A, on the published IPC curve)
USB pair: one side +3 mm detour, width 0.25 vs 0.3	skew 3.0 mm (~19.8 ps), width_matched: false

The clean board reports OK, exit 0, zero findings — asserted in the tests, both directions.

the broken board: the neck in the top trace, the blue GND run stopping short, the 0.08 mm findings circled

The complex example: a 4-motor rover controller

examples/02-rover is the full thing — MCU, IMU, four motor connectors, battery, USB-C, LED, decoupling: 14 nets, 13 components, built blind (netlist only, no sight of the copper) against the same board taken to zero findings by a real 2-layer maze router.

routed blind (12 of 14 nets open, 26 clearance violations, findings circled) vs the clean 2-layer route — same components, same nets

pcbsight diff rover_blind.kicad_pcb rover_clean.kicad_pcb
  tracks: 12 -> 113   vias: 0 -> 27
  net 'GND': 6 island(s) -> 1 ... every motor pair reached
  clearance findings: 26 -> 0

The intro example: before / after in miniature

The repair of the broken board, told entirely by diff — no re-inspection choreography, one command against both files:

pcbsight diff board_broken.kicad_pcb board_clean.kicad_pcb
  net 'GND': 2 island(s) -> 1
  clearance findings: 2 -> 0
  current '+5V': 0.745 A -> 2.392 A (min width 0.2 -> 1.0 mm)
  pair USB_P / USB_N: skew 3.0 -> 0.0 mm
  GONE [net-open]        net 'GND' is 2 separate island(s) ... unconnected pad(s): J1.2
  GONE [clearance]       track-track: '+5V' to 'SIG' at 0.08 mm (required 0.2)
  GONE [diff-pair-skew]  pair USB_P / USB_N is skewed 3.0 mm (~19.8 ps on FR4)
  GONE [diff-pair-width] pair USB_P / USB_N mixes widths [0.25, 0.3] mm

before: the GND run (blue) stops short, the neck in the +5V trace, the 0.08 mm findings circled · after: routed, clean, matched

Two of its own defects the example caught

1. The first "clean" board routed +5V straight through the GND and SIG pads — pcbsight flagged its own reference at 0.0 mm clearance. The example was wrong; the check was not. It stays in the generator as a comment.
2. USB_P/USB_N matched two suffix rules (_P/_N and P/N) and was reported twice. Pairs are now deduped by the net pair, and the test asserts exactly one.

Honest limitations

• Zones/pours are not read: a net routed only through a copper pour will read as open here. Where pours carry nets, confirm in KiCad's own DRC — this tool complements it, it does not replace it.
• Current numbers assume a lone trace in still air (that is what IPC-2221 tabulates); planes and vias change the real number.
• The impedance estimate is IPC-2141 (~10 %); controlled impedance needs the fab's field-solved stackup.
• Arcs, curved traces, keepouts and mask/paste layers are not parsed.

Siblings, same philosophy: solidsight (geometry — export the board outline there to check the enclosure fit), animationsight, texturesight, shadersight.

License

MIT