From RP2040 to ESP32-S3 — Designing the Dilder PCB¶

The breadboard era is ending. After weeks of jumper wires, borrowed breakout boards, and firmware running on a Pico W, it's time to design a real PCB — a single board that holds everything the Dilder needs. And in the process, we swapped the entire MCU.

Why We Left the RP2040¶

The RP2040 served us well for prototyping. It's cheap, it boots instantly, and the Pico W made breadboard development painless. But when we sat down to design a custom PCB, the problems became obvious:

No built-in flash — the RP2040 needs an external QSPI flash chip, crystal oscillator, and a handful of decoupling caps just to wake up
No Bluetooth — the Pico W has WiFi, but adding BLE means an external module
RF certification — designing an antenna or integrating an uncertified radio module is a project unto itself

We looked at the bill of materials for an RP2040-based custom board and counted 7+ passive components just for the MCU subsystem. There had to be a better way.

Enter the ESP32-S3-WROOM-1-N16R8¶

The ESP32-S3-WROOM-1-N16R8 is, frankly, overkill for a Tamagotchi. And that's exactly why we picked it.

16MB flash + 8MB PSRAM — the maxed-out variant, room for every quote Jamal will ever have
WiFi + Bluetooth 5 (LE) — both radios built in, pre-certified
Dual-core 240MHz Xtensa LX7 — more power than we need, but nice to have headroom
USB OTG — native USB, no FTDI chip needed
44 GPIO pins — more than enough for our peripherals

The module is a complete system: flash, PSRAM, crystal, antenna, RF matching network, and shielding can — all in one package. Drop it on a PCB, add power, and you have a working computer. That alone eliminated 7 components from the BOM.

The PCB Design Journey¶

KiCad Setup and JLCPCB Integration¶

We started by setting up KiCad 9 with the JLCPCB fabrication plugin, which lets you export Gerbers in exactly the format JLCPCB expects and includes their parts library for component sourcing. A setup script (setup-kicad-jlcpcb.py) automates the installation so anyone following along can replicate the toolchain.

Component Selection¶

The full BOM came together around the ESP32-S3:

Component	Purpose
ESP32-S3-WROOM-1-N16R8	MCU — WiFi, BLE, flash, PSRAM
LIS2DH12TR	3-axis accelerometer (built-in pedometer)
AMS1117-3.3	3.3V LDO regulator
TP4056	LiPo charging IC (USB-C input)
DW01A + FS8205A	Battery protection (over-discharge, over-current)
USB-C connector	Charging and programming
5-way joystick	Navigation input
8-pin JST-SH connector	ePaper display connection

27 components total, including passives. Compare that to the ~34+ we would have needed with a bare RP2040.

The Schematic¶

The schematic was built in sections: power (USB-C to TP4056 charger to battery protection to AMS1117 LDO), MCU (ESP32-S3 with boot/reset buttons and USB data lines), peripherals (LIS2DH12TR on I2C, joystick on GPIO, ePaper connector with SPI signals). Net labels keep the schematic readable — no rats' nest of wires crossing the sheet.

Board Layout — Iteration After Iteration¶

Layout is where the real decisions happen. We went through multiple placement iterations, optimizing based on signal flow, antenna requirements, and mechanical constraints:

ESP32-S3 at the top — antenna overhanging the board edge for best RF performance
LIS2DH12TR below-left — close to the MCU for clean I2C routing
ePaper connector below-right — 8-pin JST-SH header for the display ribbon cable
Power section in the middle — AMS1117, TP4056, battery protection clustered together
5-way joystick centered above USB-C at the bottom — ergonomic thumb position
USB-C at the very bottom — charging port accessible when held in hand

Component placement was optimized based on which side of the ESP32-S3 module each GPIO pin exits, minimizing trace crossings.

The Antenna Keep-Out Challenge¶

The ESP32-S3-WROOM-1 has a PCB antenna that extends beyond the module's footprint. Espressif's hardware design guidelines are strict: no copper (traces, pours, or planes) under or near the antenna area, on any layer. No components either. The antenna needs to overhang the board edge into free space.

This single requirement drove a major decision: we needed a 4-layer PCB. With only 2 layers, routing traces around the antenna keep-out zone while still connecting all the GPIO pins would have been nearly impossible without making the board much larger. Four layers give us:

Top — signal traces and components
Inner 1 — continuous ground plane (critical for RF and signal integrity)
Inner 2 — power plane (3.3V distribution)
Bottom — additional signal routing

The unbroken ground plane on Inner 1 is especially important — it provides the RF ground reference the antenna needs and keeps return current paths clean for high-speed signals.

The Display Connector Decision¶

This one caused some head-scratching. The Waveshare 2.13" ePaper display we've been using comes in two form factors:

Pico-ePaper-2.13 — a Pico-native module with a 40-pin header that plugs directly onto the Pico W (what we've been using for prototyping)
Waveshare 2.13" e-Paper HAT — a Raspberry Pi HAT version with a 24-pin FPC connector to the raw display panel

For the custom PCB, we considered putting a raw 24-pin FPC connector on the board to connect directly to the display's flex cable. But that would mean:

Sourcing and routing a 24-pin FPC connector (tight pitch, tricky to solder)
Handling the display driver signals directly
Losing compatibility with the HAT's built-in level shifting and connector

Instead, we went with an 8-pin JST-SH connector that carries only the SPI signals (MOSI, CLK, CS, DC, RST, BUSY) plus power and ground. This connects to the Waveshare HAT via its 8-pin ribbon cable header. Simpler routing, proven signal integrity, and we can swap display modules without redesigning the PCB.

FreeRouting — The Autorouter Experiment¶

With 27 components placed, we needed to route the traces. KiCad has a built-in interactive router, but we also tried FreeRouting, an open-source autorouter, to see if it could handle the job.

Results: mixed. FreeRouting can solve simple boards quickly, but our 4-layer design with antenna keep-out zones, ground plane requirements, and mixed-signal routing (SPI, I2C, USB, analog) pushed it past its comfort zone. The autorouter would complete routes but produce suboptimal results — traces taking unnecessary detours, vias placed in awkward locations, ground plane integrity compromised.

The lesson: autorouters are useful for getting a rough first pass or solving simple boards, but for a design like this, interactive routing in KiCad is the way to go. You need human judgment for antenna keep-out compliance, controlled impedance traces for USB, and clean power distribution.

Reference Designs That Helped¶

We didn't design in a vacuum. Three open-source reference designs were particularly useful:

Olimex ESP32-S3-DevKit-Lipo — clean power management with LiPo charging, open hardware with full KiCad files
atomic14 ESP32-S3 boards — minimal designs that show what you can strip away and still have a working system
UnexpectedMaker FeatherS3 — excellent example of antenna placement and 4-layer routing for ESP32-S3

Studying these designs confirmed our approach and caught potential mistakes before they were committed to copper.

Where We Are Now¶

The board sits at 45mm x 80mm, 4-layer, with all 27 components placed and ready for routing. The design lives in hardware-design/Board Design kicad/ with:

Full KiCad project (.kicad_pro, .kicad_sch, .kicad_pcb)
Python build scripts that place components programmatically via KiCad's pcbnew API
Research documentation covering module specs, antenna requirements, and design decisions

The PCB can be regenerated from scratch by running the build script — every component position, every design rule is captured in code, not just in KiCad's GUI state.

What's Next¶

Interactive routing in KiCad — manually route all traces with proper design rules (antenna keep-out, USB impedance, power trace widths)
Design rule check (DRC) — verify the board passes KiCad's and JLCPCB's manufacturing constraints
Generate Gerbers — export fabrication files in JLCPCB format
Order from JLCPCB — ship to Germany, wait for boards
Assemble and test — solder components, flash firmware, see if the octopus boots on custom hardware

From a breadboard held together with optimism and jumper wires to a real PCB. The octopus is getting a proper home.