ESP32 PCB Layout and Routing

Overview

This tutorial starts from an ESP32 schematic-style connection list and turns it into a practical PCB layout. The example board uses a simplified ESP32-WROOM module footprint, a 6-pin programming header, boot and reset buttons, an indicator LED, and ground pours on both copper layers.

The goal is not to copy every pin from a production ESP32 module. It is to show the layout moves you make after the circuit is connected:

put the module antenna at the board edge
keep decoupling capacitors close to 3.3 V pins
place boot and reset passives beside their ESP32 pins
route UART and strap signals away from the antenna region
pour ground after the critical component placement is stable

Complete Board

const esp32PinLabels = {
pin1: ["GND_1"],
pin2: ["3V3"],
pin3: ["EN"],
pin10: ["GPIO25"],
pin24: ["GPIO2"],
pin25: ["BOOT_IO0"],
pin29: ["GPIO5"],
pin34: ["RX0"],
pin35: ["TX0"],
pin36: ["GPIO22"],
pin37: ["GPIO23"],
pin38: ["GND_3"],
} as const

const Esp32WroomDemo = (props: {
name: string
pcbX?: number
pcbY?: number
schX?: number
schY?: number
}) => (

<chip
{...props}
pinLabels={esp32PinLabels}
schPortArrangement={{
  leftSide: {
    pins: ["3V3", "EN", "BOOT_IO0", "RX0", "TX0", "GND_1"],
    direction: "top-to-bottom",
  },
  rightSide: {
    pins: ["GPIO2", "GPIO5", "GPIO22", "GPIO23", "GPIO25", "GND_3"],
    direction: "top-to-bottom",
  },
}}
footprint={
  <footprint>
    <silkscreenrect pcbX={0} pcbY={0} width="18mm" height="25mm" />
    <silkscreentext
      text="ESP32-WROOM"
      pcbX={0}
      pcbY={0}
      fontSize="1.1mm"
      anchorAlignment="center"
    />
    <smtpad
      portHints={["pin1"]}
      pcbX="-9.4mm"
      pcbY="7.5mm"
      width="1.5mm"
      height="0.9mm"
      shape="rect"
    />
    <smtpad
      portHints={["pin2"]}
      pcbX="-9.4mm"
      pcbY="5mm"
      width="1.5mm"
      height="0.9mm"
      shape="rect"
    />
    <smtpad
      portHints={["pin3"]}
      pcbX="-9.4mm"
      pcbY="2.5mm"
      width="1.5mm"
      height="0.9mm"
      shape="rect"
    />
    <smtpad
      portHints={["pin10"]}
      pcbX="-9.4mm"
      pcbY="0mm"
      width="1.5mm"
      height="0.9mm"
      shape="rect"
    />
    <smtpad
      portHints={["pin24"]}
      pcbX="-9.4mm"
      pcbY="-2.5mm"
      width="1.5mm"
      height="0.9mm"
      shape="rect"
    />
    <smtpad
      portHints={["pin25"]}
      pcbX="-9.4mm"
      pcbY="-5mm"
      width="1.5mm"
      height="0.9mm"
      shape="rect"
    />
    <smtpad
      portHints={["pin29"]}
      pcbX="9.4mm"
      pcbY="-5mm"
      width="1.5mm"
      height="0.9mm"
      shape="rect"
    />
    <smtpad
      portHints={["pin34"]}
      pcbX="9.4mm"
      pcbY="-2.5mm"
      width="1.5mm"
      height="0.9mm"
      shape="rect"
    />
    <smtpad
      portHints={["pin35"]}
      pcbX="9.4mm"
      pcbY="0mm"
      width="1.5mm"
      height="0.9mm"
      shape="rect"
    />
    <smtpad
      portHints={["pin36"]}
      pcbX="9.4mm"
      pcbY="2.5mm"
      width="1.5mm"
      height="0.9mm"
      shape="rect"
    />
    <smtpad
      portHints={["pin37"]}
      pcbX="9.4mm"
      pcbY="5mm"
      width="1.5mm"
      height="0.9mm"
      shape="rect"
    />
    <smtpad
      portHints={["pin38"]}
      pcbX="9.4mm"
      pcbY="7.5mm"
      width="1.5mm"
      height="0.9mm"
      shape="rect"
    />
  </footprint>
}
/>
)

export default () => (
<board width="44mm" height="54mm" autorouter="sequential-trace">
  <Esp32WroomDemo name="U1" pcbX={0} pcbY={8} schX={0} schY={0} />

  <pcbnoterect
    pcbX={0}
    pcbY={22}
    width="22mm"
    height="8mm"
    color="#d97706"
    strokeWidth={0.2}
    isStrokeDashed
  />
  <pcbnotetext
    pcbX={0}
    pcbY={22}
    text="ANTENNA KEEPOUT"
    fontSize={0.9}
    color="#d97706"
    anchorAlignment="center"
  />

  <pinheader
    name="J1"
    pinCount={6}
    pinLabels={{
      pin1: "GND",
      pin2: "3V3",
      pin3: "TXD",
      pin4: "RXD",
      pin5: "EN",
      pin6: "BOOT",
    }}
    pcbX={0}
    pcbY={-20}
    schX={-7}
    schY={-6}
  />

  <resistor name="R_EN" resistance="10k" footprint="0402" pcbX={-13} pcbY={8} schX={-5} schY={4} />
  <pushbutton name="SW_RESET" footprint="pushbutton" pcbX={-17} pcbY={2} schX={-5} schY={1} />
  <resistor name="R_BOOT" resistance="10k" footprint="0402" pcbX={-13} pcbY={-2} schX={-5} schY={-2} />
  <pushbutton name="SW_BOOT" footprint="pushbutton" pcbX={-17} pcbY={-8} schX={-5} schY={-5} />

  <capacitor name="C1" capacitance="100nF" footprint="0402" pcbX={-13} pcbY={14} schX={4} schY={3} />
  <capacitor name="C2" capacitance="10uF" footprint="0603" pcbX={-16} pcbY={14} schX={4} schY={0} />

  <resistor name="R_LED" resistance="1k" footprint="0402" pcbX={12} pcbY={-8} schX={5} schY={-3} />
  <led name="D1" color="blue" footprint="0603" pcbX={16} pcbY={-8} schX={8} schY={-3} />

  <trace from=".J1 > .pin1" to="net.GND" />
  <trace from=".J1 > .pin2" to="net.V3_3" />
  <trace from=".J1 > .pin3" to=".U1 > .RX0" />
  <trace from=".J1 > .pin4" to=".U1 > .TX0" />
  <trace from=".J1 > .pin5" to=".U1 > .EN" />
  <trace from=".J1 > .pin6" to=".U1 > .BOOT_IO0" />

  <trace from=".U1 > .3V3" to="net.V3_3" />
  <trace from=".U1 > .GND_1" to="net.GND" />
  <trace from=".U1 > .GND_3" to="net.GND" />
  <trace from=".C1 > .pos" to="net.V3_3" />
  <trace from=".C1 > .neg" to="net.GND" />
  <trace from=".C2 > .pos" to="net.V3_3" />
  <trace from=".C2 > .neg" 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=".R_BOOT > .pos" to="net.V3_3" />
  <trace from=".R_BOOT > .neg" to=".U1 > .BOOT_IO0" />
  <trace from=".SW_BOOT > .pin1" to=".U1 > .BOOT_IO0" />
  <trace from=".SW_BOOT > .pin2" to="net.GND" />

  <trace from=".U1 > .GPIO2" to=".R_LED > .pos" />
  <trace from=".R_LED > .neg" to=".D1 > .pos" />
  <trace from=".D1 > .neg" to="net.GND" />

  <copperpour connectsTo="net.GND" layer="top" clearance="0.25mm" />
  <copperpour connectsTo="net.GND" layer="bottom" clearance="0.25mm" />

</board>
)

Placement Strategy

Place the ESP32 module before the small parts. The antenna end should sit at the edge of the PCB, with no copper, traces, headers, or mounting hardware under the keepout rectangle. In the example, the dashed rectangle marks the space to keep clear above the module.

After the module is locked in, place parts by electrical priority:

Part	Placement rule
`C1`, `C2`	Put decoupling capacitors next to the 3.3 V and ground pads.
`R_EN`, `SW_RESET`	Keep the reset pullup and button near `EN`.
`R_BOOT`, `SW_BOOT`	Keep the boot pullup and button near `BOOT_IO0`.
`J1`	Put the programming header where a cable can reach it without crossing the antenna side.
`D1`, `R_LED`	Move optional indicators away from RF and boot/reset routing.

Routing Order

Route the board in this order:

Connect the local 3.3 V decoupling loop from U1 to C1 and C2.
Connect EN and BOOT_IO0 to their pullups and buttons.
Route UART TXD and RXD from the header to the module.
Route optional GPIO signals such as the indicator LED.
Add the top and bottom ground pours after traces and placement are stable.

This keeps the short, sensitive power and strap nets from being pushed around by less important routing. It also makes the remaining signals easier to inspect in the PCB viewer.

Adapting the Example

For a production design, replace the simplified Esp32WroomDemo footprint with a verified footprint for the exact module variant. Keep the same layout principles:

preserve the antenna keepout from the module datasheet
use one 100 nF capacitor per nearby power pin and add a local bulk capacitor
keep reset and boot straps short and readable
avoid routing high-speed or noisy traces under the antenna
review the routed board in both PCB and schematic views before exporting fabrication files

Overview​

Complete Board​

Placement Strategy​

Routing Order​

Adapting the Example​

Overview

Complete Board

Placement Strategy

Routing Order

Adapting the Example