ESP32 PCB Layout Routing Guide

Overview

This guide walks through a review-focused ESP32 board layout flow in tscircuit. It is meant for the point where the schematic is already close, but the board still needs careful placement, power routing, antenna clearance, and pre-fab checks.

The examples use a module-style ESP32 footprint so the layout decisions are easy to inspect:

• Place the module at a board edge with the antenna facing outward.
• Reserve a copper-free antenna area before routing any signals.
• Keep the USB input, regulator, and bulk capacitors in one short power path.
• Route 3.3 V and ground first, then route boot, reset, UART, and GPIO signals.
• Use routingDisabled while arranging parts, then enable the autorouter for final checks.

Espressif's hardware design guidance for ESP32 boards calls out the same review areas: stable power, reset and boot strapping, clock/RF layout, UART download connections, and antenna clearance. See the ESP32 schematic checklist when adapting this layout to a production design.

Start With Placement

Begin by putting the ESP32 module on the top edge of the board. The dashed rectangle marks the antenna keepout. Treat it as a visual contract: no copper pour, vias, mounting hardware, tall connectors, or noisy power routing should be placed under the antenna area.

export default () => (
<board width="64mm" height="42mm" routingDisabled>
  <chip
    name="U_ESP32"
    pcbX={8}
    pcbY={8}
    footprint={
      <footprint>
        <smtpad portHints={["V3_3"]} pcbX={-9} pcbY={-8} width={1.2} height={2} shape="rect" />
        <smtpad portHints={["EN"]} pcbX={-6} pcbY={-8} width={1.2} height={2} shape="rect" />
        <smtpad portHints={["IO0"]} pcbX={-3} pcbY={-8} width={1.2} height={2} shape="rect" />
        <smtpad portHints={["TXD0"]} pcbX={0} pcbY={-8} width={1.2} height={2} shape="rect" />
        <smtpad portHints={["RXD0"]} pcbX={3} pcbY={-8} width={1.2} height={2} shape="rect" />
        <smtpad portHints={["GND"]} pcbX={6} pcbY={-8} width={1.2} height={2} shape="rect" />
        <smtpad portHints={["GPIO18"]} pcbX={9} pcbY={-8} width={1.2} height={2} shape="rect" />
        <smtpad portHints={["GPIO23"]} pcbX={12} pcbY={-8} width={1.2} height={2} shape="rect" />
        <silkscreenpath
          route={[
            { x: -12, y: -10 },
            { x: 14, y: -10 },
            { x: 14, y: 10 },
            { x: -12, y: 10 },
            { x: -12, y: -10 },
          ]}
        />
      </footprint>
    }
  />

  <pcbnoterect
    pcbX={8}
    pcbY={18}
    width={28}
    height={10}
    strokeWidth={0.25}
    color="#d97706"
    isStrokeDashed
  />
  <pcbnotetext
    pcbX={8}
    pcbY={18}
    text="ANTENNA KEEP OUT"
    fontSize={1.2}
    anchorAlignment="center"
    color="#d97706"
  />

  <connector
    name="J_USB"
    pcbX={-27}
    pcbY={-8}
    standard="usb_c"
    pinLabels={{ pin1: "VBUS", pin2: "D-", pin3: "D+", pin4: "GND" }}
  />
  <chip
    name="U_REG"
    pcbX={-13}
    pcbY={-8}
    footprint="sot223"
    pinLabels={{ pin1: "GND", pin2: "VOUT", pin3: "VIN" }}
  />
  <capacitor name="C_IN" capacitance="10uF" footprint="0805" pcbX={-19} pcbY={-15} />
  <capacitor name="C_OUT" capacitance="10uF" footprint="0805" pcbX={-6} pcbY={-15} />
  <capacitor name="C_ESP_A" capacitance="100nF" footprint="0402" pcbX={2} pcbY={-4} />
  <capacitor name="C_ESP_B" capacitance="100nF" footprint="0402" pcbX={10} pcbY={-4} />
  <pinheader name="J_UART" pinCount={4} footprint="pinrow4" pcbX={25} pcbY={-12} />
  <pushbutton name="SW_BOOT" pcbX={-4} pcbY={12} />
  <pushbutton name="SW_RESET" pcbX={8} pcbY={12} />
</board>
)

Use this first preview as a placement review:

Region	Placement goal
Antenna edge	Module antenna at the board edge, with a visible keepout.
Input power	USB, regulator, and input/output capacitors grouped tightly.
ESP32 decoupling	100 nF capacitors close to the module 3.3 V and ground pads.
Human controls	Boot and reset buttons reachable from the board edge.
Programming header	UART header away from the regulator and USB power path.

Route Power Before Signals

Route power deliberately before asking the autorouter to solve every signal. Make VBUS, V3_3, and GND wider than normal GPIO traces. The exact width depends on current, copper weight, and board house rules, but using named nets with explicit trace widths makes the intent visible in the design.

export default () => (
<board width="64mm" height="42mm" autorouter="sequential-trace">
  <net name="VBUS" traceWidth="0.55mm" />
  <net name="V3_3" traceWidth="0.4mm" />
  <net name="GND" traceWidth="0.4mm" />

  <connector
    name="J_USB"
    pcbX={-27}
    pcbY={-8}
    standard="usb_c"
    pinLabels={{ pin1: "VBUS", pin2: "D-", pin3: "D+", pin4: "GND" }}
  />
  <chip
    name="U_REG"
    pcbX={-13}
    pcbY={-8}
    footprint="sot223"
    pinLabels={{ pin1: "GND", pin2: "VOUT", pin3: "VIN" }}
  />
  <chip
    name="U_ESP32"
    pcbX={8}
    pcbY={8}
    footprint={
      <footprint>
        <smtpad portHints={["V3_3"]} pcbX={-9} pcbY={-8} width={1.2} height={2} shape="rect" />
        <smtpad portHints={["EN"]} pcbX={-6} pcbY={-8} width={1.2} height={2} shape="rect" />
        <smtpad portHints={["IO0"]} pcbX={-3} pcbY={-8} width={1.2} height={2} shape="rect" />
        <smtpad portHints={["TXD0"]} pcbX={0} pcbY={-8} width={1.2} height={2} shape="rect" />
        <smtpad portHints={["RXD0"]} pcbX={3} pcbY={-8} width={1.2} height={2} shape="rect" />
        <smtpad portHints={["GND"]} pcbX={6} pcbY={-8} width={1.2} height={2} shape="rect" />
      </footprint>
    }
  />
  <capacitor name="C_IN" capacitance="10uF" footprint="0805" pcbX={-19} pcbY={-15} />
  <capacitor name="C_OUT" capacitance="10uF" footprint="0805" pcbX={-6} pcbY={-15} />
  <capacitor name="C_ESP_A" capacitance="100nF" footprint="0402" pcbX={2} pcbY={-4} />
  <capacitor name="C_ESP_B" capacitance="100nF" footprint="0402" pcbX={10} pcbY={-4} />

  <trace from=".J_USB > .VBUS" to=".U_REG > .VIN" />
  <trace from=".J_USB > .GND" to="net.GND" />
  <trace from=".U_REG > .GND" to="net.GND" />
  <trace from=".U_REG > .VOUT" to="net.V3_3" />
  <trace from=".U_ESP32 > .V3_3" to="net.V3_3" />
  <trace from=".U_ESP32 > .GND" to="net.GND" />
  <trace from=".C_IN > .pos" to="net.VBUS" />
  <trace from=".C_IN > .neg" to="net.GND" />
  <trace from=".C_OUT > .pos" to="net.V3_3" />
  <trace from=".C_OUT > .neg" to="net.GND" />
  <trace from=".C_ESP_A > .pos" to="net.V3_3" />
  <trace from=".C_ESP_A > .neg" to="net.GND" />
  <trace from=".C_ESP_B > .pos" to="net.V3_3" />
  <trace from=".C_ESP_B > .neg" to="net.GND" />
</board>
)

Power routing review points:

• Keep the regulator output path short and direct.
• Put the bulk output capacitor on the same side of the regulator output as the ESP32 3.3 V route.
• Give each decoupling capacitor a short ground return instead of sending the return path across the board.
• Avoid sending switching or high-current traces through the antenna keepout.

Add Boot, Reset, And UART

ESP32 download mode depends on the boot strap pins. A practical board should make EN, IO0, TXD0, RXD0, V3_3, and GND easy to inspect. Put boot and reset controls close to the module, and cross the external UART header so a USB UART adapter's TXD0 connects to ESP32 RXD0.

export default () => (
<board width="64mm" height="42mm" autorouter="sequential-trace">
  <net name="V3_3" traceWidth="0.35mm" />
  <net name="GND" traceWidth="0.35mm" />

  <chip
    name="U_ESP32"
    pcbX={8}
    pcbY={8}
    footprint={
      <footprint>
        <smtpad portHints={["V3_3"]} pcbX={-9} pcbY={-8} width={1.2} height={2} shape="rect" />
        <smtpad portHints={["EN"]} pcbX={-6} pcbY={-8} width={1.2} height={2} shape="rect" />
        <smtpad portHints={["IO0"]} pcbX={-3} pcbY={-8} width={1.2} height={2} shape="rect" />
        <smtpad portHints={["TXD0"]} pcbX={0} pcbY={-8} width={1.2} height={2} shape="rect" />
        <smtpad portHints={["RXD0"]} pcbX={3} pcbY={-8} width={1.2} height={2} shape="rect" />
        <smtpad portHints={["GND"]} pcbX={6} pcbY={-8} width={1.2} height={2} shape="rect" />
      </footprint>
    }
  />
  <pinheader
    name="J_UART"
    pinCount={4}
    footprint="pinrow4"
    pcbX={25}
    pcbY={-12}
    pinLabels={["V3_3", "GND", "TXD0", "RXD0"]}
  />
  <pushbutton name="SW_BOOT" pcbX={-4} pcbY={12} />
  <pushbutton name="SW_RESET" pcbX={8} pcbY={12} />
  <resistor name="R_BOOT" resistance="10k" footprint="0402" pcbX={-4} pcbY={17} />
  <resistor name="R_EN" resistance="10k" footprint="0402" pcbX={8} pcbY={17} />

  <trace from=".R_BOOT > .pin1" to="net.V3_3" />
  <trace from=".R_BOOT > .pin2" to=".U_ESP32 > .IO0" />
  <trace from=".SW_BOOT > .pin1" to=".U_ESP32 > .IO0" />
  <trace from=".SW_BOOT > .pin2" to="net.GND" />
  <trace from=".R_EN > .pin1" to="net.V3_3" />
  <trace from=".R_EN > .pin2" to=".U_ESP32 > .EN" />
  <trace from=".SW_RESET > .pin1" to=".U_ESP32 > .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=".U_ESP32 > .RXD0" />
  <trace from=".J_UART > .RXD0" to=".U_ESP32 > .TXD0" />
</board>
)

Before fabrication, verify these nets by name in the schematic and PCB views:

Net	Expected route
EN	10 k pull-up to V3_3, reset button to GND, short trace to module.
IO0	10 k pull-up to V3_3, boot button to GND, short trace to module.
TXD0	ESP32 transmit pin to external header receive pin.
RXD0	ESP32 receive pin to external header transmit pin.
V3_3	Header power pin tied to regulator output and ESP32 3.3 V rail.
GND	Header ground, buttons, regulator, capacitors, and module tied together.

Turn Routing Back On

Keep routingDisabled during placement experiments so previews stay quick. When component positions are stable, remove it and use an autorouter. Start with sequential-trace for a small board, then move to auto-cloud or a higher autorouterEffortLevel when the board becomes dense.

<board
  width="64mm"
  height="42mm"
  autorouter="sequential-trace"
  defaultTraceWidth="0.18mm"
  minTraceWidth="0.15mm"
>
  {/* final component placement and traces */}
</board>

If the router struggles, change placement before adding manual trace paths:

• Move decoupling capacitors closer to the ESP32 3.3 V and ground pads.
• Rotate the UART header so its pins leave the module without crossing power.
• Move the regulator so VIN, VOUT, and ground paths are direct.
• Increase board height below the module instead of routing under the antenna.

Pre-Fab Review Checklist

Use this checklist before exporting Gerbers:

Area	Acceptance check
Antenna	Antenna area is on the edge, marked, and free of traces, vias, fills, and tall parts.
Power input	USB VBUS reaches the regulator with a short, wider trace.
3.3 V rail	Regulator output reaches ESP32 and decoupling capacitors without a long detour.
Ground	Decoupling capacitors have short returns and enough ground stitching near the module.
Boot mode	EN and IO0 each have pull-ups and a button path to ground.
UART	Header TXD0 and RXD0 cross to the ESP32 receive/transmit pins.
USB data	D+ and D- are kept together and away from regulator copper.
Silkscreen	Boot, reset, UART pin order, and antenna keepout are labeled.

The main win is to make the important constraints visible in code. A reviewer can see the keepout, named rails, explicit trace widths, and boot/download nets before opening a board viewer, and the PCB preview can confirm that the physical layout matches the ESP32 design intent.