Skip to content

video-v1.1 — KiCad design master for the video card

Superseded 2026-10-22 by ../v1.2/, the master now (v1.1 plus the bench fixes of 2026-10-21). Kept as history; it keeps its MASTER marker so the conversion tool never regenerates it. Was: the master, hand-maintained in KiCad 10 since 2026-09-21; Fusion 360 is abandoned for this card. Started as a copy of the proven conversion of the built card (../v1.0-fusion-export-2026-09-18/, which stays as the record of what was built) with the project renamed to video-v1.1. tools/eagle_to_kicad_all.py never writes here (MASTER marker file).

Changes since the built V1.0

  1. One 5 V rail. The built card had two nets, +5V (IC1, IC2, IC15 pin 2, RN2, R10, R12, every decoupling cap) and VCC (bus, the implicit power pins of IC17–IC28), with nothing joining them: the +5V rail had no source (found by the KiCad netlist proof; the bench wire of 2026-09-21 cured the write-through fault). Here +5V is gone: every former +5V symbol, label, pad and track is VCC, and a 0.254 mm track on F.Cu from (67.28, 112.56) to (66.01, 111.30), next to C28, joins the two former copper islands. Netlist proof vs the board: MATCH, 116/116 nets; DRC has no clearance, short or dangling-track finding; 0 unconnected items.

  2. Silkscreen title "YACC1 Video Card V1.1" (2026-10-02; it still read V1.0 from the conversion). Text only: DRC identical by type before and after (229 cosmetic findings, 0 unconnected); reports/drc.json and the two renders regenerated.

The two items left to do here (the 6845 RS from A0 to A1, pull-ups on the 7416 outputs) are done in ../v1.2/.

Files

File What it is
video-v1.1.kicad_pro project; OSH Park rules (6 mil track, 5 mil clearance, 10 mil drill, 4 mil annular)
video-v1.1.kicad_sch + -sheet1/2 schematic (two sheets, as the Eagle original)
video-v1.1.kicad_pcb 2-layer board
video-v1.1-eagle.kicad_sym, video-v1.1-eagle.pretty/ project libraries (from the conversion; edit freely)
reports/ netlist + netlist-compare.txt (proof), erc.json, drc.json, schematic PDF, top/bottom renders — regenerate after edits

Residual ERC: endpoint_off_grid 35, isolated_pin_label 56, pin_not_driven 2, pin_to_pin 9 (isolated_pin_label = the conversion's per-net global labels, endpoint_off_grid = the same labels/pins on Eagle's 0.1-inch grid; both cosmetic). Residual DRC: items_not_allowed 2, silk_edge_clearance 8, lib_footprint_mismatch 3, text_height 2, silk_overlap 15, silk_over_copper 199 (silk findings are the Eagle drawing as it was; lib_footprint_mismatch = board copies of X1/Q2/IC1 differ cosmetically from the extracted library copies).

Regenerate the reports:

K=/Applications/KiCad/KiCad.app/Contents/MacOS/kicad-cli
$K sch export netlist --format kicadsexpr -o reports/netlist.net video-v1.1.kicad_sch
$K sch erc --format json --severity-all -o reports/erc.json video-v1.1.kicad_sch
$K pcb drc --format json --severity-all -o reports/drc.json video-v1.1.kicad_pcb
$K sch export pdf -o reports/video-v1.1-schematic.pdf video-v1.1.kicad_sch
python3 ../../../../../tools/kicad/compare_netlists.py reports/netlist.net video-v1.1.kicad_pcb > reports/netlist-compare.txt

Last updated 22 October 2026