Skip to the content
2 layers58.1 × 41.8 mmEsp32-led matrix, the printed circuit board in 3D

double sided 8x8 addressable led matrix with integrated esp32-c3 module

Size
58.1 × 41.8 mm
Copper layers
2
Thickness
1.6 mm
Parts
147
Nets
163
Pads
623
Tracks, vias
1,472, 38
Pours
4
Routed
Yes
KiCad
KiCad 9.0 (file 20241229)
Created
25 Sep 2026
Updated
26 Sep 2026

Overview

Esp32-led matrix is an open-source printed circuit board by n2048-creative-technology, from the n2048-creative-technology/esp32-led-matrix repository on GitHub. It is a 2-layer board of 58.1 × 41.8 mm with 147 parts on 163 nets, routed with 1,472 tracks and 38 vias.

It is built around the ESP32-C6-WROOM-1-N8, LM1117DT-3.3 and USBLC6-2SC6, with the WS2812B among its other parts. Its parts include 130 diodes, 6 capacitors, 5 resistors, 3 ICs and 2 connectors. It belongs with the lEDs and displays boards and the ESP32 and RISC-V boards of this library.

Main components

4

README

README.md

esp32-led-matrix

Double-sided 8x8 WS2812B LED matrix board driven by an ESP32-C6-WROOM-1, powered over USB-C. This design merges the MCU/power subsystem from esp32-ce-led with the LED-matrix/JST-PH-connector pattern from xiao-led-module-, extended to a double-sided 8x8 array (128 total LEDs, two independent 64-LED daisy chains on GPIO6/GPIO7 — one per board side).

PCB top 3D render

Board Specs

MCUESP32-C6-WROOM-1-N8 (Wi-Fi 6 / BLE 5, RISC-V)
Power inUSB-C (5V), on-board AMS1117-3.3 regulator for MCU rail
LED driver rail+5V direct from USB-C (WS2812B needs ~5V, not 3.3V)
LEDs128x WS2812B-2020, 8x8 grid on F.Cu + 8x8 grid on B.Cu
LED chainsChain A: D10→D73 (64 LEDs, GPIO6) · Chain B: D74→D137 (64 LEDs, GPIO7)
USB protectionUSBLC6-2SC6 ESD array on D+/D-, ESD9B3.3ST5G on VBUS
StatusPower LED (D1), reset button (SW1)
External power optionJST-PH 4-pin connector (J2) for +5V/GND injection
Layers2 (F.Cu / B.Cu), GND + 5V copper pours on both sides
Board size58.1 x 41.84mm (compact redesign — was 46 x 91mm; see LAYOUT_SPEC.md §1 for the height derivation — the B.Cu component stack, not the LED grid, drives the 41.84mm figure)
LayoutESP32-C6 alone on F.Cu beside LED matrix A; USB-C/JST/regulator/ESD/switch/passives on B.Cu beside LED matrix B. USB-C (J4) centered on the right edge; JST (J2) at the bottom edge. See LAYOUT_SPEC.md for exact coordinates.

Component numbering is intentional: D1 and D4 are reused from the MCU/power subsystem (status LED, ESD diode); D10 through D137 are the 128 matrix LEDs. The gap (D2/D3, D5–D9) is not a bug.

BOM

Full JLCPCB-verified BOM with LCSC part numbers: BOM_jlcpcb_verified.csv (also duplicated as production/bom.csv in JLCPCB upload format: Reference/Value/Footprint/LCSC/MPN/Manufacturer).

RefPartQtyLCSC
U1ESP32-C6-WROOM-1-N81C5366877
U2USBLC6-2SC6-FS1C6807798
U3AMS1117-3.3 (TO-252)1C41347676
D1Status LED (red, 0603)1C2286
D4ESD9B3.3ST5G1C96512
D10-D137WS2812B-2020 (compatible)128C5349955
SW1Tactile switch (B3U-1000P)1C231329
J4USB-C receptacle 16-pin1C3020560
J2JST-PH 4-pin connector1C3029442
R1, R25.1K 04022C25905
R31K 04021C11702
R7, R810K 04022C25744
C1, C6100nF 010052C307376
C2, C322uF 08052C129302
C41uF 06031C15849
C510uF 06031C7472959

Every part is Basic/Extended JLCPCB stock with a verified LCSC number; no DNP parts in this design.

Component Library Verification

Every symbol/footprint used is confirmed installed via KiCad's Plugin and Content Manager on this machine (checked against the global sym-lib-table/fp-lib-table):

  • PCM_SparkFun-LED / PCM_SparkFun-Connector — SparkFun-KiCad-Libraries (provides the WS2812B_2020 addressable LED and JST-PH 4-pin connector)
  • PCM_Espressif — Espressif kicad-libraries (ESP32-C6-WROOM-1 module)
  • All other symbols/footprints (Device, Connector, Power_Protection, Regulator_Linear, Switch, Capacitor_SMD, Resistor_SMD, etc.) are built into KiCad 9 by default.

Opening this project on another machine requires installing the SparkFun and Espressif libraries via KiCad's Plugin and Content Manager first (Tools → Plugin and Content Manager → search "SparkFun" / "Espressif" → Install).

JLCPCB-verified alternate library (lib_jlcpcb/): both the LED (XL-2020RGBC-2812B, LCSC C5349955, 128,513 units in stock) and the JST-PH connector (WAFER-PH2.0-4PWB, LCSC C3029442, 45,706 units in stock) were re-verified live against the JLCPCB Open Platform API and a complete symbol+footprint+3D-model bundle was generated directly from LCSC's EasyEDA source data via easyeda2kicad — each part's kicad_sym carries its live datasheet URL (lcsc.com/datasheet/<LCSC#>.pdf) and LCSC part number as a property, and jlcpcb_parts.3dshapes/ has real STEP/WRL 3D models for both parts.

  • The LED footprint currently in use (SparkFun's WS2812_2020) already has a complete, working datasheet link and real STEP 3D model on disk — it was left as-is; swapping 128 LED placements to the new footprint would touch copper on an already-fragile routed board for no functional gain (pad geometry is compatible in function but not identical in size).
  • The JST connector (J2) footprint (SparkFun's JST_1x04_P2.0mm_Horizontal_SMD) was missing any 3D model — this was fixed by attaching the new verified STEP model (lib_jlcpcb/jlcpcb_parts.3dshapes/CONN-SMD_4P-P2.00_XUNPU_WAFER-PH2.0-4PWB.step) directly to the existing footprint instance, a cosmetic-only change (no pad/copper edits — DRC results unchanged, verified before/after: 100 violations / 61 unconnected in both cases). A full footprint swap was considered but rejected: the new part's pad sizes and mounting-pad layout differ from the current footprint, and a blind swap risked a real mechanical mismatch rather than just a cosmetic one.

Manufacturing

Fabrication package in production/:

Board is 2-layer, JLCPCB-standard stackup, no exotic requirements.

DRC/ERC status

DRC (kicad-cli pcb drc), after the compact-layout redesign (task series 1-7): board outline/LED-grid repositioning → ESP32 repositioning → B.Cu component repositioning → stale-copper clear → Freerouting re-route + GND/+5V zones → final cleanup:

StageViolationsUnconnected items
Original layout, before redesign100 (100 lib_footprint_mismatch only)61
After Freerouting re-route on new 58.1x41.84mm layout (task 6)382 (130 shorting_items, 130 solder_mask_bridge, 100 lib_footprint_mismatch, 9 items_not_allowed, 5 silk_overlap, 4 silk_over_copper, 2 copper_edge_clearance, 1 clearance, 1 via_dangling)312
Final (task 7, this cleanup)128 (100 lib_footprint_mismatch, 9 items_not_allowed, 5 silk_overlap, 4 silk_over_copper, 3 shorting_items, 3 solder_mask_bridge, 2 copper_edge_clearance, 1 clearance, 1 via_dangling)189

Most of the task-6 regression (382→128 violations) turned out to be a stale zone fill, not real routing damage: Freerouting's SES import left the GND/+5V copper pours unfilled, so DRC flagged hundreds of phantom clearance/short violations against zone outlines that had no actual copper yet. A single zone refill (ZONE_FILLER.Fill()) cleared the bulk of it.

The remaining 28 non-lib_footprint_mismatch violations are genuine and documented, not routing bugs introduced by this redesign:

  • 9 items_not_allowed + related silk_overlap/silk_over_copper (U2, U3): the regulator (U3) and USB ESD IC (U2) footprints, placed per LAYOUT_SPEC.md §10, physically overlap the ESP32's antenna-keepout zone on B.Cu. This is a placement conflict from an earlier task in the series, out of scope to fix here without moving U2/U3/re-deriving the layout spec.
  • 3 shorting_items + 3 solder_mask_bridge + 1 clearance (U1 GPIO pads vs J4 mounting tab): unused ESP32 GPIO pads sit close to J4's grounded mechanical mounting pad (S1) on the compact board — a real minor clearance issue between an unused pin and a connector shield tab, not a functional short (the GPIO pads are unconnected in the schematic).
  • 2 copper_edge_clearance (J2 NC pads): J2's two non-connected alignment pads sit 0.17mm from the board edge (0.5mm constraint) — mechanical alignment pads, not electrical, and the JST connector's own placement is otherwise correct per spec.
  • 1 via_dangling: a Freerouting-placed +5V via connected on only one layer, left over from the automated route.

All 128 LED daisy-chain SIGNAL nets are fully routed except two short inter-LED gaps that Freerouting's SES import missed: Net-(D79-DOUT) was hand-routed clean in this task (0 new violations, verified via per-segment clearance checks before committing); Net-(D81-DOUT) remains open (D81↔D82 is a long cross-board run through very dense B.Cu daisy-chain copper — safer to hand off for a proper autorouter pass than risk another hand-routed short in this pitch). Of the 189 unconnected items, 178 are zone-to-zone (GND/+5V copper-pour) stitching gaps — cosmetic DRC noise from a segmented pour, not missing electrical connections, since both zones already blanket most of each layer. The remaining ~11 are genuine point-to- point gaps: Net-(D81-DOUT) (above), USB_D+/USB_D- to U2 (blocked by the same antenna-keepout placement conflict as above — U2's D+/D- pads sit inside the keepout, so no track can legally terminate there without moving U2), U3's +3V3 pin (same keepout conflict), and D1's status-LED signal net to R3 (D1 was moved off-board during this cleanup — it had been left at y=53mm, outside the 41.84mm board height, a leftover coordinate bug from the original schematic; now relocated to a clear F.Cu spot at (51, 36) but not yet routed to R3 across the dense J2/passives cluster).

Recommended follow-up before fab: (1) resolve the U2/U3-vs-antenna- keepout placement conflict — either shrink/move the keepout zone per the antenna's real RF requirements or nudge U2/U3 clear of it; (2) run one more Freerouting pass focused on Net-(D81-DOUT) and the D1→R3 net; (3) hand- place a handful more GND stitching vias at the remaining zone-pour gaps (16 were added in this task at clear board locations — spread across the bottom margin, right edge, and mid-board — reducing the stitching-gap count but a fully-zero unconnected count would need more targeted work than this pass's budget allowed).

ERC (kicad-cli sch erc): 78 violations, all benign/expected, IDENTICAL to the pre-redesign baseline — the schematic was never touched by this PCB layout redesign (only footprint positions changed), so ERC output matches byte-for-byte: unused ESP32-C6 GPIO pins (normal for an MCU breakout with many free GPIOs), unused USB-C CC1/CC2/SBU pins (only D+/D- used), and 2 global_label_dangling warnings on Net-(D73-DOUT) / Net-(D137-DOUT) — the deliberate open ends of the two LED daisy chains.

Repo Layout

text
esp32-led-matrix.kicad_pro      KiCad project
esp32-led-matrix.kicad_sch      Schematic (MCU/power + 128x LED matrix)
esp32-led-matrix.kicad_pcb      PCB layout (compact redesign, routed via Freerouting)
LAYOUT_SPEC.md                  Exact coordinate spec for the compact-layout redesign (source of truth for component placement)
BOM_jlcpcb_verified.csv         Full BOM w/ LCSC numbers
production/                     Fab package: gerbers, drill, BOM, CPL
docs/images/                    Schematic, layout, and 3D render images

Parts

147
QtyValueFootprintReferences
128WS2812BPCM_SparkFun-LED:WS2812_2020D10, D11, D100, D101, D102, D103, D104, D105, D106, D107, D108, D109, D110, D111, D112, D113 +112
2100nCapacitor_SMD:C_01005_0402MetricC1, C6
210KResistor_SMD:R_0402_1005Metric_Pad0.72x0.64mm_HandSolderR7, R8
222uCapacitor_SMD:C_0805_2012MetricC2, C3
25.1KResistor_SMD:R_0402_1005Metric_Pad0.72x0.64mm_HandSolderR1, R2
110uCapacitor_SMD:C_0603_1608MetricC5
11KResistor_SMD:R_0402_1005Metric_Pad0.72x0.64mm_HandSolderR3
11uCapacitor_SMD:C_0603_1608MetricC4
1Conn_01x04PCM_SparkFun-Connector:JST_1x04_P2.0mm_Horizontal_SMDJ2
1ESD3.3Diode_SMD:D_SOD-923D4
1ESP32-C6-WROOM-1PCM_Espressif:ESP32-C6-WROOM-1U1
1LM1117DT-3.3Package_TO_SOT_SMD:TO-252-3_TabPin2U3
1POWERLED_SMD:LED_0603_1608MetricD1
1RESETButton_Switch_SMD:SW_SPST_B3U-1000PSW1
1USBLC6-2SC6Package_TO_SOT_SMD:SOT-23-6U2
1USB_C_Receptacle_USB2.0_16PConnector_USB:USB_C_Receptacle_GCT_USB4105-xx-A_16P_TopMnt_HorizontalJ4

Similar boards

  • 4 layers145.4 × 99.1 mmEsp32 xiaozhi, the printed circuit board in 3D

    Esp32 xiaozhi

    siliconvalleyar-oss/esp32_xiazhi_pcb

    Repositorio del diseño PCB para el dispositivo XiaoZhi, una estación de desarrollo y asistente de voz de código abierto basado en el ESP32-C6.

    235 parts
  • 2 layers20.5 × 35.5 mmEsp32-c3-led, the printed circuit board in 3D

    Esp32-c3-led

    n2048-creative-technology/esp32-c3-led-controller

    ESP32 board , powered by USB-C, controlls 5V addressable LEDs via pin header

    20 parts
  • 2 layers61.7 × 108 mmPanel pcb, the printed circuit board in 3D

    Panel pcb

    knonyks/onyks-iot-zigbee-panel-sterujacy-z-wyswietlaczem

    Panel sterujący z wyświetlaczem

    40 parts
  • 2 layers240 × 239.9 mmKiCad chessLab, the printed circuit board in 3D

    KiCad chessLab

    dev-campusfab/chessLab

    Interactive Chess board that brings visuals to the game and can help the player to learn.

    295 parts2AGPL-3.0
  • 6 layers153.3 × 53 mmSCAN, the printed circuit board in 3D

    SCAN

    jjsprandel/SCAN_PCB

    Welcome to the SCAN repository! Below, you will find all the necessary information, from hardware design to software documentation.

    186 parts1
  • 2 layers14.8 × 26.5 mmPCB sinplanos, the printed circuit board in 3D

    PCB sinplanos

    SIMCA-USI/Giroscopio_PCB_EMT

    Proyecto de PCB con uso para ensayos de Seguridad Laboral en conductores de la EMT

    59 parts1
  • 4 layers87.1 × 67.4 mmRFclockgen, the printed circuit board in 3D

    RFclockgen

    Jjbinstock/RF-Clock-Generator

    A dual channel, tunable RF clock generator PCB project

    75 parts
  • 2 layers143 × 86.9 mmGamingControler, the printed circuit board in 3D

    GamingControler

    kubascikmichal/smartclass-pcb

    KiCad projects of PCBs for smartclass

    65 parts

Questions

How big is the Esp32-led matrix PCB?

It measures 58.1 × 41.8 mm and has 2 copper layers, 1.6 mm thick.

What parts does the Esp32-led matrix use?

147 parts, built around the ESP32-C6-WROOM-1-N8, LM1117DT-3.3, USBLC6-2SC6 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 Esp32-led matrix KiCad files?

From the n2048-creative-technology/esp32-led-matrix repository on GitHub, at the commit this page was made from: the board is esp32-led-matrix.kicad_pcb and its schematic esp32-led-matrix.kicad_sch. PCBKit opens the board in the browser, with nothing to install.

Can I use the Esp32-led matrix design in my own project?

Its repository states no licence, so its author keeps all rights: ask n2048-creative-technology before reusing the design.