Skip to content

docs: add ESP32 PCB layout and routing tutorial #679

New issue

Have a question about this project? Sign up for a free GitHub account to open an issue and contact its maintainers and the community.

Sign up for GitHub

By clicking “Sign up for GitHub”, you agree to our terms of service and privacy statement. We’ll occasionally send you account related emails.

Already on GitHub? Sign in to your account

Open
victorhblancom-design wants to merge 1 commit into
base: main
Choose a base branch
from
Open

docs: add ESP32 PCB layout and routing tutorial #679

Changes from all commits
Commits
Show all changes
1 commit
Select commit
File filter

Filter by extension

Filter by extension
Conversations
Failed to load comments.
Loading
Jump to
Jump to file
Failed to load files.
Loading
Diff view
Diff view
226 changes: 226 additions & 0 deletions docs/tutorials/esp32-pcb-layout-and-routing.mdx
View file
Open in desktop
Original file line number Diff line number Diff line change
@@ -0,0 +1,226 @@
---
title: ESP32 PCB Layout and Routing
description: Place and route an ESP32 module board with USB power, boot/reset controls, antenna keepout, and stable power traces.
---

import CircuitPreview from "@site/src/components/CircuitPreview"

## 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.

<CircuitPreview
splitView
defaultView="pcb"
code={`
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`.

<CircuitPreview
splitView
defaultView="pcb"
code={`
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.

<CircuitPreview
splitView
defaultView="schematic"
code={`
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.