Skip to the content
2 layers192 × 192 mmWordclock led, the printed circuit board in 3D

QLOCKTWO-style English word clock — ESP32-C5 + WS2812B, Rust (esp-idf-svc)

Size
192 × 192 mm
Copper layers
2
Thickness
1.6 mm
Parts
240
Nets
120
Pads
711
Tracks, vias
423, 232
Pours
2
Routed
Yes
KiCad
KiCad 10.0 (file 20260206)
Created
30 Aug 2026
Updated
7 Nov 2026

Overview

Wordclock led is an open-source printed circuit board by Traveler0014, from the Traveler0014/word-clock repository on GitHub, published under the MIT licence. It is a 2-layer board of 192 × 192 mm with 240 parts on 120 nets, routed with 423 tracks and 232 vias.

It is built around the 74AHCT1G125SE and WS2812B. Its parts include 117 capacitors, 114 diodes, 2 connectors, 1 resistor and 1 IC.

Main components

2

README

hardware/README.md

hardware/ — 灯板 PCB 设计(KiCad)

把原方案的 10 行灯条 + 27 处行间飞线,替换成单块 192×192mm 的 LED 面板 PCB。 含原理图 + PCB + Gerber + 预览图 + 可复现的生成脚本。

方案背景与取舍见 ../docs/led-pcb.md。 本目录是其中「方案 A:灯板 + 现有 ESP32-C5-DevKitC」的具体实现。

文件

文件内容
wordclock-led.kicad_proKiCad 工程
wordclock-led.kicad_sch原理图(平坦单页 A1:114 颗灯 + 电平转换 + 电源/接口)
wordclock-led.kicad_pcbPCB(2 层,已铺铜填充)
wordclock-led-sch.pdf原理图 PDF(便于评审)
gen/gen_sch.py原理图生成脚本(纯标准库,任意 python3)
gen/gen_pcb.pyPCB 生成脚本(需 KiCad 自带 python + pcbnew)
preview/pcb_top.png / pcb_bottom.png3D 预览
fab/*Gerber + 钻孔(F.Cu/B.Cu/Mask/Paste/Silk/Edge + drl + job)

fab/pcba.step 不入库(.gitignore 已排除):它与 pcba.step 字节完全一致, 只是给「自洽的 fab 包」用。要直接丢给板厂/贴片厂时手动拷:cp pcba.step fab/。

板子规格

项值
尺寸 / 层数192.0 × 192.0 mm,2 层,1.6 mm,1oz(建议 2oz 或限制亮度)
灯114 × WS2812B 5050(110 字母阵 11×10 + 4 角点)
灯距 pitch15.0 mm(字母阵 165×150,居中留边 13.5 / 21)
角点距板角 7 mm(腔/窗由结构件做,φ11 / φ5)
数据链蛇形(行 0 左→右,奇数行反向),链尾 109 在左下;角点按周长环 110→111→112→113。原理图用显式串联导线画出(奇数行 mirror y 让 DIN/DOUT 朝向链方向,VDD/VSS 保持上下)
走线数据走线全程无直角:转弯一律 45° 倒角
电源顶层 GND 铺铜区,底层 +5V 平面;每颗 LED/电容就近打过孔到 +5V
去耦每颗灯 1 × 100nF 0402(C1–C114),入口 1000µF + 22µF + 100nF
电平转换U1 = 74AHCT1G125(SOT-23-5,5V 供电),输出串 R1 = 33Ω
安装孔4 × M3(四边中点,和原外壳螺丝位一致)
丝印板名、5V IN (J2) / ESP32-C5 (J1)、+5V/GND

与 ESP32-C5 的连接

text
ESP32-C5-DevKitC-1                灯板 (J1)                板上
  GPIO4 ── 杜邦/JST 4pin DATA ──► J1.3 ──► U1.A ── 74AHCT1G125(5V) ──► R1(33Ω) ──► D1.DIN
  GND   ────────────────────────► J1.2/4 (GND)
  5V    ◄─────────────────────── J1.1 (仅当 JP1 短接)
                                   J2 = 5V/3A 外部电源输入(5V,5V,GND,GND)
连接器引脚网络说明
J1(接 DevKitC)1/+5V_DEV经 JP1 可选给开发板供 5V
2, 4GND
3/DIN_IN来自 C5 GPIO4 的 3.3V 数据
J2(电源输入)1, 2+5V5V/3A,双针并联
3, 4GND
JP1(焊桥)1–2+5V ↔ /+5V_DEV默认断开;短接则灯板 5V 反给开发板
  • 开发期:DevKitC 用 USB 供电时 JP1 保持断开(否则双电源互灌);两者务必共地(J1.2/4)。
  • 成品:外部 5V 接 J2,JP1 短接,由灯板同时给开发板供电,或继续让开发板独立供电。
  • 数据电平:板载 74AHCT125 已做 3.3V→5V,不要再外接电平转换。

若后续要出「集成版 v2」(ESP32-C5-WROOM-1 直接上板),参考 ../docs/led-pcb.md §5 方案 B: 原生 USB-Serial-JTAG(IO13/14)+ IO4(RMT) + IO1(ADC 光敏) + IO23/24(I2C), 天线强烈建议用 WROOM-1U 外置,USB 控制台需改 sdkconfig。

⚠ 元件高度与勘误

  • 正面最高元件:C117 电解 11.5mm > 排针 8.5mm > C116 2.52mm > 灯珠 1.61mm。 结构件按 14mm 格栅净高设计。完整实测表见 ../docs/pcba-heights.md。
  • J1/J2 已换料:原 BOM 的 C492419(XFCN PZ254V-12-4P)是双排 2×2,插不进 PinHeader_1x04;已改用 LCSC C19190970 = HDGC HDGCPH-PZ01-04(单排 1×4,金镀), 板面高 8.54 mm。
  • STEP 外包络是 192×202(上下各 ~4.85mm 工艺边),实际板子 192×192。

固件

无需改动:仍 GPIO4、仍 114 颗、蛇形索引与 wordclock-core::xy_to_index 一致。 PCB 网络名与原理图完全一致(/D0…/D113、/DOUT、/DIN_IN、/S1、/+5V_DEV、+5V、GND), 所以在 KiCad 里「从原理图更新 PCB」不会断开已布好的线。

角点顺序在板上是 110 左下 → 111 右下 → 112 右上 → 113 左上。 固件只看「点亮前 n 颗」,功能不受影响;若想 minute=1 固定点某角,改 Frame::dots() 一行即可 (原 docs/wiring.md 的 110~113 标注需同步修正)。

校验记录

  • ERC:0 error / 0 warning
  • DRC:0 violation / 0 未连接;走线无直角(转弯均 45°)
  • 网络一致性:原理图 netlist 与 PCB 焊盘网络逐网比对,120 网 0 mismatch
  • 串联链:/D0…/D113、/DOUT 逐节校验(D{i}.DOUT → D{i+1}.DIN)全部正确
  • Gerber/钻孔:kicad-cli 导出成功

重新校验(KiCad 10 命令行):

bash
kicad-cli sch erc   --severity-error wordclock-led.kicad_sch
kicad-cli pcb drc   --severity-error wordclock-led.kicad_pcb
kicad-cli pcb export gerbers -o fab/ -l "F.Cu,B.Cu,F.Mask,B.Mask,F.Paste,B.Paste,F.Silkscreen,B.Silkscreen,Edge.Cuts" wordclock-led.kicad_pcb
kicad-cli pcb export drill   -o fab/ wordclock-led.kicad_pcb

重新生成

text
hardware/
├── gen/gen_sch.py     # 任意 python3(Linux 亦可),读 KiCad 符号库
└── gen/gen_pcb.py     # 必须用 KiCad 自带 python(带 pcbnew 模块)
bash
cd hardware
python3 gen/gen_sch.py                                   # 生成 .kicad_sch
"C:/Program Files/KiCad/10.0/bin/python.exe" gen/gen_pcb.py   # 生成 .kicad_pcb(含铺铜)

脚本里的几何参数(板尺寸、pitch、元件坐标、走线)都在文件顶部,改完全局重跑即可。 两脚本自动探测 KiCad 安装路径(Windows D:\... 或 WSL /mnt/d/...)。 每次生成 UUID 随机,故与已提交版本会有 diff,属正常。

gen_pcb.py 的铺铜需要「保存→重新加载→填充→再保存」的往返: 无头模式下直接对新建 board 调 ZONE_FILLER 会崩(已在脚本内处理)。

打样 / 装配注意

  • 2 层 192×192 已能覆盖当前电流(实测 <0.5A);全白跑满 6.8A 时请用 2oz 或限亮。
  • 每颗 5050 的 GND 焊盘实心连到 GND 铺铜(利于散热与载流);返修时热风要够功率。
  • C117(1000µF 直立电解)在板正面顶边(146, 11.5),高度约 12mm。
  • 控制区(顶边 y≈3..19)元件在正面:结构件需在该处留凹槽/让位, 或把控制区整体移到板背(+5V 平面留 keepout 即可)。见「待决」。
  • 建议先打 1 片 验证:先只上 5V 测短路/静态电流,再用现有固件自检全链。

待决 / 风险

  1. "200×200"口径:若指含外壳的成品,PCB 可再缩到 ~192→实际外框 200;当前 PCB 192 + 4mm 壁 ≈ 200×200,正好。
  2. 控制区位置:现放正面顶边,结构件要配合;若想更干净可移到背面。
  3. 角点顺序:如需 minute=1 → 左上,改固件映射(1 行)。
  4. 散热/密封:密封腔 + 1/4 限亮预计 OK;全白需通风。
  5. 是否做集成版 v2(C5 上板):见 ../docs/led-pcb.md §5。

Parts

240
QtyValueFootprintReferences
114100nFCapacitor_SMD:C_0402_1005MetricC1, C10, C11, C100, C101, C102, C103, C104, C105, C106, C107, C108, C109, C110, C111, C112 +98
114WS2812BLED_SMD:LED_WS2812B_PLCC4_5.0x5.0mm_P3.2mmD1, D10, D11, D100, D101, D102, D103, D104, D105, D106, D107, D108, D109, D110, D111, D112 +98
4MountingHoleMountingHole:MountingHole_3.2mm_M3H1, H2, H3, H4
2Conn_01x04Connector_PinHeader_2.54mm:PinHeader_1x04_P2.54mm_VerticalJ1, J2
11000uFCapacitor_THT:CP_Radial_D10.0mm_P5.00mmC117
1100nFCapacitor_SMD:C_0603_1608MetricC115
122uFCapacitor_SMD:C_1210_3225MetricC116
133Resistor_SMD:R_0603_1608MetricR1
15V_LINKJumper:SolderJumper-2_P1.3mm_Open_RoundedPad1.0x1.5mmJP1
174AHCT1G125Package_TO_SOT_SMD:SOT-23-5U1

Similar boards

  • 2 layers68 × 100 mmKeyboard featherwing, the printed circuit board in 3D

    Keyboard featherwing

    arturo182/keyboard_featherwing_hw

    The Keyboard FeatherWing is an easy way to add a handheld Qwerty keyboard and a 2.6” color display (+ more) to your project! It fits well in your hands and is great for typing with your thumbs, early 2000s-style.

    58 parts43
  • 2 layersTopBoard, the printed circuit board in 3D

    TopBoard

    Libre-Talk/Wave

    Smart Speaker satellite

    184 parts22
  • 4 layers51.8 × 68.3 mmButton Matrix RP2040, the printed circuit board in 3D

    Button Matrix RP2040

    hazenluk/RP2040_AS3394

    An AS3394 Voice Card with built in RP2040

    229 parts3
  • 2 layers435 × 123 mmNec pc-8801-type a, the printed circuit board in 3D

    Nec pc-8801-type a

    djvs/nec-pc-8801-type-a

    NEC PC 8801 Type A keyboard PCB (work in progress)

    268 parts2CC-BY-SA-4.0
  • 2 layers290 × 210 mmT8-Sequencer, the printed circuit board in 3D

    T8-Sequencer

    lluisestape-upc/T8-Sequencer

    16-step ESP32 groovebox: two-layer 290x210 mm KiCad board, DRC-clean and fabrication-ready, with the Python scripts that generated and repaired it

    104 parts2MIT
  • 2 layers158.8 × 100.2 mmChocobanan rev.1, the printed circuit board in 3D

    Chocobanan rev.1

    leonrat/Chocobanan

    An alice-like 40% split keyboard

    108 parts1
  • 2 layers78.1 × 83.9 mmBadge recon-2026, the printed circuit board in 3D

    Badge recon-2026

    reconkrad1337-arch/badge-recon-2026

    This is the official repository of the REcon Badge 2026. Here you will find the source code, schematics, and documentation for the badge.

    74 parts1GPL-3.0
  • 2 layers88.6 × 69.9 mmExpressionController, the printed circuit board in 3D

    ExpressionController

    amonbenson/expad

    A four-jack USB MIDI adapter for expression and sustain pedals, built on a Raspberry Pi Pico 2 W. It works out what is plugged into each jack - whichever contact a pedal's wiper is on, and whether it is a potentiometer…

    147 partsMIT

Questions

How big is the Wordclock led PCB?

It measures 192 × 192 mm and has 2 copper layers, 1.6 mm thick.

What parts does the Wordclock led use?

240 parts, built around the 74AHCT1G125SE and WS2812B. The full list of its parts is on this page, with links to each part's symbol and footprint where PCBKit's library has them.

Where can I download the Wordclock led KiCad files?

From the Traveler0014/word-clock repository on GitHub, at the commit this page was made from: the board is hardware/wordclock-led.kicad_pcb and its schematic hardware/wordclock-led.kicad_sch. PCBKit opens the board in the browser, with nothing to install.

Can I use the Wordclock led design in my own project?

Its repository publishes it under the MIT licence: you may reuse it on that licence's terms (keep the author's notice, and for a copyleft licence share your changes alike).