ESP32 PCB Layout and Routing

Overview

This tutorial shows a practical ESP32 board layout flow in tscircuit. The example uses an ESP32-WROOM style module, a USB-C power/input connector, a 3.3 V regulator, boot and reset buttons, and local decoupling capacitors.

The most important layout choices are:

Put the ESP32 module at the board edge so the antenna points away from copper, mounting holes, and large components.
Keep the USB connector, regulator, and bulk capacitor close together so the 5 V input path is short.
Put decoupling capacitors close to the ESP32 3.3 V pins.
Route power nets wider than signal nets, then let the autorouter handle the remaining UART, boot, enable, and indicator traces.

Board Outline And Major Placement

Start with a board size that leaves a clear antenna edge. The ESP32 module sits near the top of the board, the USB connector sits on the left edge, and the regulator stays between USB 5 V and the ESP32 3.3 V rail.

import { ESP32_WROOM_32DC as Esp32Module } from "@tsci/AnasSarkiz.ESP32_WROOM_32DC"

export default () => (
<board width="58mm" height="42mm" autorouter="freerouting">
  <Esp32Module
    name="U1"
    pcbX={8}
    pcbY={7}
    schX={0}
    schY={3}
    pcbRotation="0deg"
  />

  <connector
    name="J_USB"
    pcbX={-25}
    pcbY={-8}
    schX={-6}
    schY={0}
    pinLabels={{
      pin1: "VBUS",
      pin2: "D-",
      pin3: "D+",
      pin4: "GND",
    }}
    standard="usb_c"
  />

  <chip
    name="U2"
    pcbX={-11}
    pcbY={-8}
    schX={-2.5}
    schY={0}
    footprint="sot223"
    pinLabels={{
      pin1: "GND",
      pin2: "VOUT",
      pin3: "VIN",
    }}
  />

  <capacitor name="C1" capacitance="10uF" footprint="0805" pcbX={-17} pcbY={-14} />
  <capacitor name="C2" capacitance="10uF" footprint="0805" pcbX={-5} pcbY={-14} />
  <capacitor name="C3" capacitance="100nF" footprint="0402" pcbX={2} pcbY={-6} />
  <capacitor name="C4" capacitance="100nF" footprint="0402" pcbX={9} pcbY={-6} />

  <pushbutton name="SW_BOOT" pcbX={-7} pcbY={12} schX={-2} schY={-3} />
  <pushbutton name="SW_RESET" pcbX={4} pcbY={12} schX={2} schY={-3} />
  <resistor name="R_BOOT" resistance="10k" footprint="0402" pcbX={-7} pcbY={18} />
  <resistor name="R_EN" resistance="10k" footprint="0402" pcbX={4} pcbY={18} />
  <led name="LED_PWR" footprint="0603" pcbX={-21} pcbY={10} schX={-5} schY={-4} />
  <resistor name="R_LED" resistance="1k" footprint="0402" pcbX={-17} pcbY={10} />
</board>
)

Power Nets

Name the power rails first and give them wider trace widths. The USB connector feeds the regulator, the regulator creates V3_3, and every decoupling capacitor returns to GND.

import { ESP32_WROOM_32DC as Esp32Module } from "@tsci/AnasSarkiz.ESP32_WROOM_32DC"

export default () => (
<board width="58mm" height="42mm" autorouter="freerouting">
  <net name="VBUS" traceWidth="0.5mm" />
  <net name="V3_3" traceWidth="0.35mm" />
  <net name="GND" traceWidth="0.35mm" />

  <Esp32Module name="U1" pcbX={8} pcbY={7} />
  <connector
    name="J_USB"
    pcbX={-25}
    pcbY={-8}
    pinLabels={{ pin1: "VBUS", pin2: "D-", pin3: "D+", pin4: "GND" }}
    standard="usb_c"
  />
  <chip
    name="U2"
    pcbX={-11}
    pcbY={-8}
    footprint="sot223"
    pinLabels={{ pin1: "GND", pin2: "VOUT", pin3: "VIN" }}
  />
  <capacitor name="C1" capacitance="10uF" footprint="0805" pcbX={-17} pcbY={-14} />
  <capacitor name="C2" capacitance="10uF" footprint="0805" pcbX={-5} pcbY={-14} />
  <capacitor name="C3" capacitance="100nF" footprint="0402" pcbX={2} pcbY={-6} />
  <capacitor name="C4" capacitance="100nF" footprint="0402" pcbX={9} pcbY={-6} />

  <trace from=".J_USB > .VBUS" to=".U2 > .VIN" />
  <trace from=".U2 > .VOUT" to="net.V3_3" />
  <trace from=".U1 > .V3_3" to="net.V3_3" />
  <trace from=".C1 > .pos" to="net.VBUS" />
  <trace from=".C2 > .pos" to="net.V3_3" />
  <trace from=".C3 > .pos" to="net.V3_3" />
  <trace from=".C4 > .pos" to="net.V3_3" />

  <trace from=".J_USB > .GND" to="net.GND" />
  <trace from=".U2 > .GND" to="net.GND" />
  <trace from=".U1 > .GND" to="net.GND" />
  <trace from=".C1 > .neg" to="net.GND" />
  <trace from=".C2 > .neg" to="net.GND" />
  <trace from=".C3 > .neg" to="net.GND" />
  <trace from=".C4 > .neg" to="net.GND" />
</board>
)

Boot, Reset, And UART Signals

ESP32 boards normally need pull-ups on EN and IO0, plus buttons that pull those nets to ground. Keep those buttons near the module edge so they are easy to press and the traces stay short.

import { ESP32_WROOM_32DC as Esp32Module } from "@tsci/AnasSarkiz.ESP32_WROOM_32DC"

export default () => (
<board width="58mm" height="42mm" autorouter="freerouting">
  <net name="V3_3" />
  <net name="GND" />

  <Esp32Module name="U1" pcbX={8} pcbY={7} />
  <pushbutton name="SW_BOOT" pcbX={-7} pcbY={12} />
  <pushbutton name="SW_RESET" pcbX={4} pcbY={12} />
  <resistor name="R_BOOT" resistance="10k" footprint="0402" pcbX={-7} pcbY={18} />
  <resistor name="R_EN" resistance="10k" footprint="0402" pcbX={4} pcbY={18} />

  <pinheader
    name="J_UART"
    pcbX={23}
    pcbY={-12}
    pinCount={4}
    gender="male"
    pitch="2.54mm"
    pinLabels={["V3_3", "GND", "TXD0", "RXD0"]}
    footprint="pinrow4"
  />

  <trace from=".R_BOOT > .pos" to="net.V3_3" />
  <trace from=".R_BOOT > .neg" to=".U1 > .IO0" />
  <trace from=".SW_BOOT > .pin1" to=".U1 > .IO0" />
  <trace from=".SW_BOOT > .pin2" to="net.GND" />

  <trace from=".R_EN > .pos" to="net.V3_3" />
  <trace from=".R_EN > .neg" to=".U1 > .EN" />
  <trace from=".SW_RESET > .pin1" to=".U1 > .EN" />
  <trace from=".SW_RESET > .pin2" to="net.GND" />

  <trace from=".J_UART > .V3_3" to="net.V3_3" />
  <trace from=".J_UART > .GND" to="net.GND" />
  <trace from=".J_UART > .TXD0" to=".U1 > .RXD0" />
  <trace from=".J_UART > .RXD0" to=".U1 > .TXD0" />
</board>
)

Routing Checklist

Before sending the board out, check these layout constraints:

Area	What to check
Antenna	Keep the ESP32 antenna beyond the board edge or over a copper-free keepout.
3.3 V rail	Use a wider trace from regulator output to ESP32 3.3 V and decoupling capacitors.
Ground	Give each decoupling capacitor a short route back to ground.
USB	Keep `D+` and `D-` close together and avoid routing them under noisy power parts.
Boot/reset	Confirm `IO0` and `EN` have pull-ups and momentary pull-down buttons.
UART	Cross the external header's `TXD0` to ESP32 `RXD0`, and `RXD0` to ESP32 `TXD0`.

Practical Iteration Flow

During placement, set routingDisabled on the board for fast previews. Once the module, regulator, connector, buttons, and capacitors are in stable positions, remove routingDisabled, keep the power net widths, and let the autorouter complete the signal routes.

If the router struggles, move decoupling capacitors closer to the ESP32, increase board width near the USB connector, or separate the UART header from the power input path. Small placement changes usually solve more routing problems than adding manual trace paths early.

Overview​

Board Outline And Major Placement​

Power Nets​

Boot, Reset, And UART Signals​

Routing Checklist​