Skip to the content
4 layers32.6 × 40 mmESP32 C3 Mini, the printed circuit board in 3D

4-layer ESP32-C3 WROOM development board with USB-C, ESD protection, LDO regulation and differential pair routing — designed in KiCad

Size
32.6 × 40 mm
Copper layers
4
Thickness
1 mm
Parts
31
Nets
30
Pads
147
Tracks, vias
164, 32
Pours
9
Routed
Yes
KiCad
KiCad 10.0 (file 20260206)
Created
29 Jun 2026
Updated
30 Jun 2026

Overview

ESP32 C3 Mini is an open-source printed circuit board by marouane-daoudi, from the marouane-daoudi/esp32-c3-dev-board repository on GitHub. It is a 4-layer board of 32.6 × 40 mm with 31 parts on 30 nets, routed with 164 tracks and 32 vias.

It is built around the ESP32-C3-WROOM-02-H4, AP2112K-3.3 and USBLC6-2P6, with the PESD5V0L1UL among its other parts. Its parts include 10 capacitors, 10 resistors, 3 ICs, 3 connectors and 2 diodes. It belongs with the ESP32 and RISC-V boards of this library.

Main components

4

README

README.md

ESP32-C3 Development Board

ESP32-C3 WROOM Development Board

A 4-layer development and testing board for the ESP32-C3-WROOM-02 module. It uses USB-C for 5V input and USB 2.0 data, includes onboard 3.3V LDO regulation, ESD protection on the USB data and VBUS lines, an external crystal, reset and boot buttons, a 3.3V power indicator LED, and breadboard-compatible GPIO headers.

The board was designed in KiCad 10.0 with a focus on power integrity, signal routing, ESD return paths, and low-impedance power distribution.


Specifications

ParameterValue
Target moduleESP32-C3 WROOM-02
PCB layers4-layer FR4
Board width27.94mm (breadboard compatible)
Pin pitch2.54mm
Input5V via USB-C
Regulated output3.3V — AP2112K-3.3TRG1 LDO (600mA max)
ESD protection (data)USBLC6-2SC6 dual ESD diode
ESD protection (VBUS)PESD5V0L1UL
CrystalExternal oscillator for USB timing
Power indicatorGreen LED (NATIONSTAR NCD0805G1)
Design toolKiCad

Pin Header Reference

Left HeaderRight Header
3.3V5V
GNDGND
ENIO3
IO4GND
IO5TXD
IO6RXD
IO7GND
IO9IO10

System overview

Block diagram


Schematic

Schematic


Block-by-block circuit description

USB-C interface

A 16-pin USB-C receptacle provides 5V input power and USB 2.0 data. Three groups of pins are used:

CC1 and CC2 — each connected to GND through a 5.1kΩ resistor. These configuration channel pins tell the upstream power source that this board is a power sink requesting 5V at standard current. Without these resistors, modern USB-C chargers and laptop ports will not supply power. Both pins require their own resistor because the cable can be inserted in either orientation — only one CC pin is active per insertion but both must be terminated.

D+ and D- — USB 2.0 data lines connected to the ESP32-C3 through the USBLC6-2SC6 dual ESD protection IC. This device was chosen for its low line capacitance, which is critical for preserving signal integrity on high-speed differential pairs — excessive capacitance loads the lines and degrades eye diagrams at USB Full Speed. A single IC protects both lines simultaneously.

VBUS — the 5V supply rail, protected and filtered before entering the rest of the circuit through two stages: a PESD5V0L1UL ESD diode clamping surge voltages, followed by a pi filter (capacitor — 0Ω resistor — capacitor) for additional conducted noise filtering. The 0Ω resistor is a deliberate design choice — it can be replaced with a polyfuse for overcurrent protection on future revisions without redesigning the PCB.

LDO voltage regulation

The AP2112K-3.3TRG1 LDO regulates 5V from VBUS down to the 3.3V required by the ESP32-C3. It was chosen over a switching regulator for two reasons: it keeps the design compact, and it produces no switching noise — important for a board with RF and ADC functionality where a switching regulator's ripple could degrade performance.

The AP2112K is rated for 600mA output current, covering the ESP32-C3's typical current demand with sufficient margin. The datasheet recommends 1µF input and output decoupling capacitors. 4.7µF was used instead for two reasons: the same value was already introduced in the pi filter stage (simplifying the BOM), and slightly larger decoupling capacitance improves transient response under sudden load steps.

Crystal oscillator

An external crystal oscillator provides the precise clock reference required for USB Full Speed timing. The ESP32-C3 WROOM module includes an internal RC oscillator but it is insufficiently accurate for USB — USB 2.0 Full Speed requires clock accuracy within ±2500ppm, which only an external crystal can reliably provide. Load capacitors are placed symmetrically on both crystal pins per the datasheet recommendations.

Reset circuitry (EN pin)

A push button pulls the EN pin to GND when pressed, triggering a hard reset of the ESP32-C3. EN is normally held HIGH through a pull-up resistor to VCC. An RC filter is added per the ESP32-C3 datasheet recommendation — the resistor and capacitor form a low-pass filter that prevents mechanical switch bounce from generating spurious reset pulses. Without this filter, a single physical button press can produce multiple rapid transitions on EN, causing repeated resets instead of a clean single reset event.

Boot button (IO9)

The ESP32-C3 determines boot mode by reading IO2, IO8, and IO9 at startup. For normal operation all three must be HIGH. For USB download mode (firmware flashing), IO9 must be LOW while the others remain HIGH. IO2 and IO8 are permanently pulled HIGH through resistors. A dedicated BOOT button pulls IO9 LOW only when pressed — releasing it returns IO9 HIGH through its pull-up resistor, allowing normal operation. The button is only effective when pressed simultaneously with RESET, which forces the chip to sample the boot pins at startup.

Power indicator LED

A green LED (NATIONSTAR NCD0805G1, 0805 package) with a 1kΩ current-limiting resistor indicates active 3.3V power on the board. It was added after the rest of the design was complete as a simple functional indicator.


PCB layout and routing

3D render

Front Back

Front layer (signal + components)

PCB Front

Layer 2 — continuous ground plane

Ground plane

Layer 3 — Long switch connections

Power layer

Back layer (Power distribution planes (VBUS, 3.3V), crystal, additional signals)

PCB Back

4-layer stackup

LayerFunction
Layer 1 (top)Signal routing, components, ESD, LDO, USB-C
Layer 2Continuous solid ground plane
Layer 3Long switch connections (EN and IO9 routing only)
Layer 4 (bottom)Power distribution planes (VBUS, 3.3V), crystal, additional signals

Layer 2 is kept as an uninterrupted solid ground plane throughout the entire board. Every high-speed signal on the top layer is referenced to this plane, ensuring a controlled return path directly beneath each trace. This is the single most important layout decision on the board — a broken ground plane forces return currents to take longer paths, increasing loop inductance and radiating EMI.

Placement strategy

Components were placed by following the power flow of the circuit from input to output, grouping by functional block before routing began:

USB-C connector at the bottom edge → ESD protection immediately adjacent → pi filter following → LDO stage → decoupling capacitors → ESP32-C3 module at the top. This left-to-right, input-to-output placement minimizes trace length on the power path and keeps high-current paths short and direct.

Power distribution — local copper planes

All power connections use custom-shaped local copper planes rather than routed traces. Three separate planes were defined: one for VBUS (5V from USB), one for the LDO input (5V filtered), and one for the 3.3V output. Copper planes provide significantly lower resistance and inductance than traces of equivalent length — critical during transient load events when the ESP32-C3 core suddenly demands current during Wi-Fi transmission bursts.

The 3.3V plane runs from the LDO output capacitor directly to the ESP32-C3 decoupling capacitors, ordered deliberately: the 4.7µF bulk capacitor sees the current first, followed by the 100nF high-frequency decoupling capacitor, then vias transfer the 3.3V to the ESP32-C3 power pin on the front layer. THT pin headers connect directly to the back copper plane, providing clean 3.3V and 5V access at the headers without additional routing.

ESD protection placement

The USBLC6-2SC6 (data line ESD) and PESD5V0L1UL (VBUS ESD) are placed immediately at the USB-C connector pads — the first components the external signals reach after entering the board. Three ground vias are placed directly adjacent to the ESD diode ground pads, providing the shortest possible low-impedance discharge path to the ground plane during an ESD event. Inductance in the discharge path reduces clamping effectiveness — minimizing this path length is as important as the protection device selection itself.

USB differential pair routing

D+ and D- are routed as a tightly coupled differential pair on the top layer, referenced to the continuous ground plane on layer 2. The route is kept short from the USB-C connector through the ESD protection device to the ESP32-C3 module. Trace spacing is kept consistent and the pair is routed with USB impedance control in mind. Routing on the surface layer directly above the ground plane ensures a well-defined return path with minimal loop area.

Crystal routing

The crystal and its load capacitors are placed on the back layer to conserve space on the front. Traces are kept short and routed symmetrically on both oscillator pins — asymmetry in crystal routing introduces parasitic differences between the two pins that can prevent oscillation startup or cause frequency instability. Vias transfer the crystal signals between back and front layers at the ESP32-C3 pins.

General signal routing

GPIO and power pins for the headers were routed straightforwardly. Where traces would have conflicted with high-speed signal areas on the front layer, the THT nature of the pin headers was exploited — signals were dropped to the back layer via vias and routed there, keeping the top layer clean for the differential pair and crystal signals. The EN and IO9 connections to the RESET and BOOT buttons required a long connection routed on layer 3 to avoid interference with other routing layers.

Ground fill

Ground copper fills were applied to all four layers after routing was complete, filling all unused copper areas. This reduces EMI by eliminating antenna-like copper islands, lowers ground impedance across the board, and provides additional shielding between signal layers. Layer 2 was maintained as a completely uninterrupted solid ground plane with no signal routing passing through it at any point.

Antenna keep-out zone

A 5mm keep-out zone is enforced beneath the ESP32-C3 WROOM module's PCB antenna on all four layers. Copper beneath the antenna detunes it by altering the antenna's electromagnetic environment, reducing Wi-Fi range and reliability. No traces, planes, or fills enter this zone.


What I learned building this

This was the most technically demanding board in this portfolio and introduced concepts not present in simpler 2-layer designs:

  • 4-layer stackup design and strategic layer assignment
  • Power planes vs traces — impedance and inductance tradeoffs
  • Local copper planes for low-impedance power distribution
  • Decoupling capacitor ordering and placement as a layout-critical decision, not just a schematic one
  • ESD protection placement rules and discharge path inductance
  • Ground via stitching adjacent to ESD devices for low-inductance discharge paths
  • USB differential pair routing with length matching and controlled impedance
  • Crystal oscillator routing — symmetry and trace length constraints
  • Antenna keep-out zone enforcement across all layers
  • Ground fill strategy and copper island elimination
  • Using THT via penetration to simplify back-layer routing

Manufacturing

Gerber files in /gerbers verified with JLCPCB's online Gerber viewer.

JLCPCB Gerber verification

To order, zip the contents of the gerbers folder and upload to JLCPCB or PCBWay. Select:

  • Layers: 4
  • Material: FR4
  • Thickness: 1.6mm
  • Stackup: JLC04161H-7628 (standard JLCPCB 4-layer)

Repository contents

FolderContents
/kicadSchematic, PCB, and KiCad project files
/gerbersFabrication-ready Gerber and drill files
/images3D renders, PCB layer screenshots, schematic images, and Gerber previews

Acknowledgments

Circuit design and PCB layout process based on the tutorial Design a Custom ESP32-Mini Board in KiCad 9 by [PajoPCB]. No source files were provided in the original video — schematic, PCB layout, component selection, and all KiCad files in this repository were built independently while following the tutorial's design approach.


Author

Marouane Daoudi
Electrical Engineering student
Designed in KiCad

Parts

31
QtyValueFootprintReferences
54u7Capacitor_SMD:C_0805_2012Metric_Pad1.18x1.45mm_HandSolderC1, C2, C3, C4, C5
410KResistor_SMD:R_0402_1005MetricR5, R7, R8, R9
3100nfCapacitor_SMD:C_0402_1005MetricC6, C9, C10
212.5pFCapacitor_SMD:C_0201_0603Metric_Pad0.64x0.40mm_HandSolderC7, C8
25.1KResistor_SMD:R_0402_1005MetricR1, R2
2Conn_01x08_PinConnector_PinHeader_2.54mm:PinHeader_1x08_P2.54mm_VerticalJ2, J3
2SW_PushButton_Switch_SMD:SW_SPST_B3U-1000PSW1, SW2
1100Resistor_SMD:R_0402_1005MetricR6
11KResistor_SMD:R_0402_1005MetricR10
1AP2112K-3.3Package_TO_SOT_SMD:SOT-23-5_HandSolderingU2
1CrystalCrystal:Crystal_SMD_3215-2Pin_3.2x1.5mmY1
1ESP32-C3-WROOM-02RF_Module:ESP32-C3-WROOM-02U3
1GREENLED_SMD:LED_0805_2012Metric_Pad1.15x1.40mm_HandSolderD2
1PESD5V0L1ULDiode_SMD:D_SOD-882D1
1RResistor_SMD:R_0805_2012MetricR3
1TBDResistor_SMD:R_0201_0603MetricR4
1USBLC6-2P6Package_TO_SOT_SMD:SOT-666U1
1USB_C_Receptacle_USB2.0_16PConnector_USB:USB_C_Receptacle_G-Switch_GT-USB-7010ASVJ1

Similar boards

  • 4 layers29 × 31.7 mmESP32-C3-mini, the printed circuit board in 3D

    ESP32-C3-mini

    max-bispham/esp32-module-board-tutorial

    Tutorial design I followed in order to learn kicad, pcb design process and schematic layout

    29 parts
  • 4 layers30.6 × 35.8 mmEsp32-c3-mini, the printed circuit board in 3D

    Esp32-c3-mini

    Srushti-D-Hebbar/esp32-c3-wroom02-development-board

    A custom 4-layer ESP32-C3-WROOM-02 development board designed in KiCad 10 - includes USB-C power/data, schematics, PCB layout, and manufacturing files.

    29 partsMIT
  • 2 layers110.7 × 109.2 mmESP32S3R8 XR GL, the printed circuit board in 3D

    ESP32S3R8 XR GL

    Supriya648/ESP32-S3-XR-Glasses-PCB

    Custom PCB with ESP32-S3 camera module for AI/XR glasses

    80 parts
  • 4 layers72.6 × 35.8 mmEsp32 cam, the printed circuit board in 3D

    Esp32 cam

    akashh218/ESP32-CAM-Devlopment-board

    Custom 4-layer ESP32-S3 camera development board designed in KiCad, featuring camera and microSD interfaces, dual USB-C connectivity, UART programming, GPIO expansion, power management, and RF-aware PCB layout.

    54 parts
  • 2 layersRobot Arm PCB, the printed circuit board in 3D

    Robot Arm PCB

    JoshAyersSBT/Robot_Arm_PCB

    This document consolidates the power architecture, wiring, BOM additions, and system diagram for an ESP32-based robot arm controller using:

    26 parts
  • 4 layers40.4 × 55.5 mmESP32-Dev Kit, the printed circuit board in 3D

    ESP32-Dev Kit

    jishnu085/esp32-c3-custom-board

    Custom ESP32-C3 PCB design using KiCad

    29 parts1
  • 4 layers79.5 × 20 mmMatter usb switch, the printed circuit board in 3D

    Matter usb switch

    IvanVeloz/smart-usb-plug

    A smart plug for USB with energy measurement and Matter over Thread support

    65 parts2GPL-3.0
  • 2 layers54.5 × 90 mmDev board, the printed circuit board in 3D

    Dev board

    21shravan/AT89s51-dev-board

    A modern AT89S52 (8051) development board featuring USB Type-C power, CH340C USB-to-UART, ISP programming, and a complete open-source hardware design documented from schematic to PCB.

    44 parts

Questions

How big is the ESP32 C3 Mini PCB?

It measures 32.6 × 40 mm and has 4 copper layers, 1 mm thick.

What parts does the ESP32 C3 Mini use?

31 parts, built around the ESP32-C3-WROOM-02-H4, AP2112K-3.3, USBLC6-2P6 and PESD5V0L1UL. 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 C3 Mini KiCad files?

From the marouane-daoudi/esp32-c3-dev-board repository on GitHub, at the commit this page was made from: the board is kicad/ESP32_C3_Mini.kicad_pcb and its schematic kicad/Block_diagram.kicad_sch. PCBKit opens the board in the browser, with nothing to install.

Can I use the ESP32 C3 Mini design in my own project?

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