Skip to the content
2 layers30 × 64 mmCustomized ESP-32, the printed circuit board in 3D

Two-layer ESP32-WROOM-32 dev board in KiCad: USB-C, CP2102N with auto-reset, AMS1117, breadboard headers. Rev B after a design review of rev A.

Size
30 × 64 mm
Copper layers
2
Thickness
1.6 mm
Parts
28
Nets
62
Pads
199
Tracks, vias
544, 45
Pours
2
Routed
Yes
KiCad
KiCad 9.0 (file 20241229)
Created
14 Oct 2026
Updated
17 Oct 2026

Overview

Customized ESP-32 is an open-source printed circuit board by pazambranosauc, from the pazambranosauc/esp32-devboard repository on GitHub. It is a 2-layer board of 30 × 64 mm with 28 parts on 62 nets, routed with 544 tracks and 45 vias.

It is built around the ESP32-WROOM-32, AMS1117-3.3 and MMBT3904. Its parts include 9 resistors, 7 capacitors, 3 ICs, 3 connectors and 2 transistors. It belongs with the microcontroller boards boards and the ESP32 boards of this library.

Main components

3

README

README.md

ESP32 Development Board (KiCad)

A two-layer ESP32-WROOM-32 development board designed from a blank schematic: USB-C, an AMS1117-3.3 regulator, a CP2102N USB-UART bridge with two-transistor auto-reset, and two breadboard-spaced 20-pin headers. It's sized for hand assembly: 0603 passives, 1206 tantalums, 2.54 mm headers.

Status: Rev B layout complete, not yet fabricated. Rev A was cancelled before production after a design review found three faults (below). Bring-up results will be added here once the boards arrive.

TopBottom
3D render, top3D render, bottom

Specs

Board30.0 × 64.0 mm, 2 layers, GND pour on both layers
MCUESP32-WROOM-32 (antenna keep-out on every layer, no copper under the antenna)
USBUSB-C receptacle (GCT USB4105), USB 2.0, 5.1 kΩ on CC1 and CC2 so it works either way up
USB-UARTCP2102N (QFN-24), DTR/RTS auto-reset through two MMBT3904s
Power5 V USB → AMS1117-3.3, 10 µF tantalum in and out, 100 nF decoupling at each IC
I/O2 × 20-pin 2.54 mm headers, rows 25.4 mm apart (fits a breadboard)
ButtonsEN (reset) and IO0 (boot)
Routing0.25 mm signals, 0.5 mm power (USB_VBUS, VDD, GND), necked down to 0.2 mm at fine-pitch pins

How it works

text
USB-C ─┬─ VBUS ──┬─ AMS1117-3.3 ── VDD (3.3 V) ─┬─ ESP32-WROOM-32
       │         └─ CP2102N VREGIN / VBUS        └─ CP2102N VIO, pull-ups, headers
       ├─ D+/D− ─── CP2102N ── TXD/RXD ───────────── ESP32 RXD0/TXD0
       │                    └─ DTR/RTS ─ Q1/Q2 ──── EN / IO0   (auto-reset into bootloader)
       └─ CC1/CC2 ─ 5.1 kΩ each to GND (identifies the board as a USB sink)

Rev B schematic

Rev A → Rev B: what broke and what I changed

Rev A was laid out and submitted to JLCPCB. A net-by-net review of the board file found three faults, so I cancelled the order before it went into production.

#Rev A faultWhy it was missedRev B fix
1The 3.3 V regulator had no input. USB 5 V (USB_VBUS) only reached the CP2102N's VREGIN pin. The AMS1117's input was on a separate net (UART_VBUS) tied only to the CP2102N's VBUS sense pin. The input caps were in series instead of to GND. The board would never have powered on.A PWR_FLAG on the regulator input told ERC the net was powered, which hid the error.USB 5 V feeds the regulator and both CP2102N VBUS pins, the caps go to GND, and the masking PWR_FLAG is removed.
2The reset and boot buttons did nothing. Each switch pulled EN or IO0 to GND through a reverse-biased LED, so the pin never went low.ERC can't see it: every connection is valid, only the diode direction is wrong.The switches go directly to EN and IO0, and the LEDs are removed.
3Auto-reset was AC-coupled. The transistor bases were driven through 100 nF capacitors instead of resistors, giving only edge pulses where esptool needs IO0 held low while EN rises.ERC can't see it: the topology is right, only the component type is wrong.10 kΩ base resistors (R10, R11).

Also changed for Rev B:

  • USB-C plug → receptacle, so it works with a normal cable. CC1 and CC2 each have their own 5.1 kΩ, and both D+/D− contact pairs are tied.
  • 1.00 mm → 2.54 mm headers. The 1 mm headers had 0.15 mm between pads, far below JLCPCB's 0.5 mm minimum for through-holes, and wouldn't fit a breadboard.
  • 0201 resistors and 1808 caps → 0603, and 10 µF electrolytics → 1206 tantalums, for hand soldering.
  • ESP32 ground-pad vias 0.2 → 0.3 mm, JLCPCB's 2-layer minimum.
  • EN RC 10 kΩ / 1 µF, as Espressif recommends.
  • GND pour on both layers, replacing a front-only pour that had broken into islands.

The original Rev A schematic is kept in hardware/rev-a/, with a screenshot, for comparison.

Layout, front copperLayout, back copper
FrontBack

Verification so far

  • ERC: re-run on the final schematic before fabrication.
  • DRC: 0 errors, 0 unconnected items. Accepted violations, each documented:
    • 4 × hole clearance: the USB4105's GND pads sit 0.19 mm from its own plastic locating-peg holes in the manufacturer footprint. JLCPCB trims copper around non-plated holes.
    • 1 × library mismatch on U2: from the deliberate via-drill change.
  • Independent net check: a script compared every pad on the board against the schematic netlist (62 nets, 0 mismatches) and confirmed every net is fully connected in copper.
  • Not yet verified: fabrication, assembly and power-up. Planned bring-up:
    1. Check 3.3 V with no ESP32 fitted.
    2. Check the CP2102N enumerates.
    3. Scope EN and IO0 during an auto-reset.
    4. Flash a blink sketch.

Bill of materials

RefValueFootprintQty
U2ESP32-WROOM-32RF_Module:ESP32-WROOM-321
U3CP2102N (e.g. CP2102N-A02-GQFN24)QFN-24-1EP_4x4mm_P0.5mm_EP2.6x2.6mm1
U1AMS1117-3.3SOT-223-3_TabPin21
P1USB-C receptacle, 16-pin (GCT USB4105-GF-A)USB_C_Receptacle_GCT_USB4105-xx-A_16P_TopMnt_Horizontal1
Q1, Q2MMBT3904SOT-232
C1, C3, C910 µF tantalum (C1 ≥ 16 V, C3/C9 ≥ 10 V)CP_EIA-3216-18_Kemet-A_HandSolder3
C2, C4, C8100 nFC_0603_1608Metric3
C51 µFC_0603_1608Metric1
R1, R5, R7, R8, R10, R1110 kΩR_0603_1608Metric6
R2, R35.1 kΩR_0603_1608Metric2
R61 MΩR_0603_1608Metric1
SW1, SW2Tactile switch (Alps SKRK)SW_Push_SPST_NO_Alps_SKRK2
J1, J21×20 male header, 2.54 mmPinHeader_1x20_P2.54mm_Vertical2

Open the project

KiCad 9. Open hardware/Customized ESP-32.kicad_pro; open the schematic and board through the project so they stay linked.

text
hardware/
  Customized ESP-32.kicad_pro   project
  Customized ESP-32.kicad_sch   schematic (rev B)
  Customized ESP-32.kicad_pcb   board (rev B)
  Customized ESP-32.kicad_dru   custom design rules
  rev-a/                        original rev A schematic, kept for comparison
docs/images/                    renders, layout and schematic screenshots

Pedro Zambrano-Saucedo · Electrical Engineering, UTEP · Portfolio

Parts

28
QtyValueFootprintReferences
610kΩResistor_SMD:R_0603_1608Metric_Pad0.98x0.95mm_HandSolderR1, R5, R7, R8, R10, R11
3100nFCapacitor_SMD:C_0603_1608Metric_Pad1.08x0.95mm_HandSolderC2, C4, C8
210μFCapacitor_Tantalum_SMD:CP_EIA-3216-18_Kemet-A_HandSolderC1, C9
25.1kΩResistor_SMD:R_0603_1608Metric_Pad0.98x0.95mm_HandSolderR2, R3
2Conn_01x20_PinConnector_PinHeader_2.54mm:PinHeader_1x20_P2.54mm_VerticalJ1, J2
2MMBT3904Package_TO_SOT_SMD:SOT-23Q1, Q2
2SW_PushButton_Switch_SMD:SW_Push_SPST_NO_Alps_SKRKSW1, SW2
110µFCapacitor_Tantalum_SMD:CP_EIA-3216-18_Kemet-A_HandSolderC3
11MΩResistor_SMD:R_0603_1608Metric_Pad0.98x0.95mm_HandSolderR6
11µFCapacitor_SMD:C_0603_1608Metric_Pad1.08x0.95mm_HandSolderC5
1AMS1117-3.3Package_TO_SOT_SMD:SOT-223-3_TabPin2U1
1CP2102N-Axx-xQFN24Package_DFN_QFN:QFN-24-1EP_4x4mm_P0.5mm_EP2.6x2.6mmU3
1ESP32-WROOM-32RF_Module:ESP32-WROOM-32U2
1USB_C_Receptacle_USB2.0_16PConnector_USB:USB_C_Receptacle_GCT_USB4105-xx-A_16P_TopMnt_HorizontalP1

The 26 most common of 28 parts.

Similar boards

  • 2 layers76.3 × 49.6 mmEls esp32, the printed circuit board in 3D

    Els esp32

    guidoschreuder/els-esp32

    Port of Clough42's electronic leadscrew to ESP32

    63 parts6
  • 2 layers40.9 × 58 mmUpsy desky, the printed circuit board in 3D

    Upsy desky

    mikes-techzone/upsy-desky

    This repository contains the source files for the Upsy Desky, a device which lets you connect your standing desk to any home automation system.

    48 parts
  • 2 layers77.2 × 44.5 mmEsp32 rtc display, the printed circuit board in 3D

    Esp32 rtc display

    beer88/PCB-Projects-Kicad

    This repository contains a collection of PCB design projects developed using KiCad, covering a range of applications in embedded systems, automation, and hardware development.

    55 parts1
  • 4 layers46.8 × 34.8 mmSmartWatch V4, the printed circuit board in 3D

    SmartWatch V4

    Bellafaire/ESP32-Smart-Watch

    An open source smartwatch based on the ESP32 compatible with the Arduino IDE.

    74 parts258MIT
  • 2 layers46 × 41.4 mmESP32.24, the printed circuit board in 3D

    ESP32.24

    OpenMYR/ESP32-Hobby-Servo

    Open MYR ESP32 controller board, 15 port servo direct

    54 parts6
  • 2 layers90 × 60 mmSabvoton controller, the printed circuit board in 3D

    Sabvoton controller

    dkomeza/sabvoton-controller

    A controller for the sabvoton ebike esc.

    72 parts3
  • 2 layers25.2 × 59.4 mmEsp32-pcb, the printed circuit board in 3D

    Esp32-pcb

    krwc/doge32

    Yet another ESP32 PCB

    50 parts3

Questions

How big is the Customized ESP-32 PCB?

It measures 30 × 64 mm and has 2 copper layers, 1.6 mm thick.

What parts does the Customized ESP-32 use?

28 parts, built around the ESP32-WROOM-32, AMS1117-3.3 and MMBT3904. 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 Customized ESP-32 KiCad files?

From the pazambranosauc/esp32-devboard repository on GitHub, at the commit this page was made from: the board is hardware/Customized ESP-32.kicad_pcb and its schematic hardware/Customized ESP-32.kicad_sch. PCBKit opens the board in the browser, with nothing to install.

Can I use the Customized ESP-32 design in my own project?

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