Loading…

 Legal / Impressum

Left thumb module, 11 keys (left-T11) — 2 LEDs, the pilot board

The first board redrawn in KiCad from its EasyEDA Pro source, netlist-driven, through the qualification gate.

Code
left-T11
Side
left
Slot
thumb
Variant
T11
Status
qualified
Released
none yet

Files from dev@f162cad · 2026-10-17 · KiCad 10.0.6· not a released revision

See its 10 wires Interactive BOM ↗ Parts list (CSV)

Faces

Top face of the Left thumb module, 11 keys
Top
Bottom face of the Left thumb module, 11 keys
Bottom

3D model

Parts

All 4 parts
ReferenceValueFootprintManufacturerMPNLCSCKeyQty
D1-D11 1N4148WS T4 lynx:SOD-323_L1.8-W1.3-LS2.5-RD CJ(江苏长电/长晶) 1N4148WS T4 C2128 a1,a2,b1,b2,c1,c2,c3,d1,d2,e1,e2 11
J1 PH2.54-1X10P-H25 lynx:HDR-TH_10P-P2.54-V-M JXTCONN(聚兴泰) PH2.54-1X10P-H25 C42431810 —1
LED1,LED2 SK6812mini-012 lynx:LED-SMD_4P-L3.7-W3.5-P1.75-BR-SK6812MINI OPSCO(欧思科) SK6812mini-012 C2886570 —2
SW1-SW11 K9-1267T lynx:SW-TH_K9-1267T 韩国韩荣 K9-1267T C107266 a1,a2,b1,b2,c1,c2,c3,d1,d2,e1,e2 11

Schematic

Schematic of the Left thumb module, 11 keys

Opens full size in a new tab.

Interactive BOM: © 2025-2026 lynx-v4 contributors · CERN-OHL-S-2.0 AND MIT

Design notes

Left thumb module, 11 keys (left-T11) — 2 LEDs, the pilot board

The first board redrawn in KiCad from its EasyEDA Pro source, netlist-driven, through the qualification gate. Source of truth for this board: this KiCad project since the gate was ticked on 2026-09-25. The frozen export (ProPrj_CAT-v4_Thumb_Left_Keys-11_2026-08-01.epro2 in the private EasyEDA archive, board left_thumb-module_keys_v0.4.0_1, PCB PCB_L-T-k_1) is the archived original. The KiCad files were generated from electronics/baseline/T11-left/, placed and routed with the source's copper, trace for trace, the GND pour on top filled by KiCad. No deviations from the source.

Gate record (2026-09-25)

StepStateEvidence
Archive the original export✅private EasyEDA archive, sha256 6ced7394…047e17
Produce the KiCad project✅generated, deterministic (uuid5), saved by kicad-cli 10.0.6
Resolve symbols, footprints, 3D models✅electronics/lib/ (check_lib.py left-T11: all pads match; the SOD-323 pad width is an accepted difference in lib/parts.toml); the project's own library since 2026-09-26, copper unchanged
Schematic ↔ PCB association, parity✅footprints carry path to their symbol; pcb drc --schematic-parity: no entry
Diff connectivity✅check_board.py: 61 connected pads, 22 nets, identical net classes in schematic and board vs the baseline, both directions; 12 no-connects match the baseline's open pads
Diff pad numbering, polarity✅pad ↔ net per pad number, and every source trace ends on the pad of its own net (DRC: no short, nothing unconnected) — the diode's anode/cathode and the LED's DIN/DOUT follow from it
Diff placement✅every pad of every footprint within 0.01 mm of the baseline's absolute pad position (orientation and side solved from the pads, not assumed)
Diff outline, holes, layers✅outline bbox 60.96 × 35.0 mm and 11 vertices; 4 holes at the baseline positions; 2 copper layers
Connector labels✅every header pad labelled with its wiring-harness.toml signal's silk alias (TI1…, LED_DATA) at the source's label position
Diff copper✅all 147 source traces and 11 vias at their source position, width and net; the GND pour on the source's rectangle; every net one piece (GND through the filled pour), DRC 0 unconnected items
ERC✅0 errors, 0 warnings (./lx pcb check left-T11 --routed)
DRC✅/⚠️0 errors; copper-to-edge held to 0.2 mm, the four source pads below reported as warnings by left-thumb-module-11-keys.kicad_dru; one dangling track end (finding 4); silkscreen warnings inherited from the library footprints
Manufacturing outputs vs the last ordered packagen/ano package recovered (electronics/README.md)
Human review✅Stas, in KiCad 10.0.6, 2026-09-25

Findings while redrawing

  1. Outer switch pads touch the board edge. SW4/SW9 pad 3 and SW6/SW11 pad 1 (the outer pads of the outer columns, x = ±29.08 mm, Ø2.8 mm pads) are tangent to the outline at x = ±30.48 — 0.0 mm copper-to-edge, in the source too; JLCPCB asks 0.2 mm on a routed edge. Named in left-thumb-module-11-keys.kicad_dru; a before-next-order item.
  2. The K9-1267T is used on pins 2 and 3 with pin 1 open, reproduced from the pad ↔ net table; the datasheet check of electronics/docs/before-next-order.md still applies.
  3. Silkscreen: the pulled footprints' silk overlaps between the diode and switch outlines and runs over pads (the DRC warnings). Cosmetic; the source had the same.
  4. The source has a 0.26 mm stub of LED_DOUT1 running past LED2 pad 1 to nowhere (DRC track_dangling). Reproduced; harmless, removable on review.
  5. D6, D8, D11 (the diodes turned 90°) were placed reversed by the first redraw (commit f02226e): the generators rotated footprints clockwise where KiCad turns them counter-clockwise, and the placement check shared that error. The source's traces exposed it; fixed in tools/electronics/layout.py.

Hand-over

Edit this board in KiCad from now on. The generators refuse to overwrite a routed board (--force would discard the KiCad edits); place_from_baseline.py left-T11 --silk-only still refreshes the connector labels, and check_board.py left-T11 --routed shows what an edit changed against the source.