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Superseded 2026-10-22 by ../v1.2/, the master now (v1.1 plus the bench fixes of 2026-10-21).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¶
-
One 5 V rail. The built card had two nets,
+5V(IC1, IC2, IC15 pin 2, RN2, R10, R12, every decoupling cap) andVCC(bus, the implicit power pins of IC17–IC28), with nothing joining them: the+5Vrail had no source (found by the KiCad netlist proof; the bench wire of 2026-09-21 cured the write-through fault). Here+5Vis gone: every former+5Vsymbol, label, pad and track isVCC, 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. -
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.jsonand 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