Skip to the content
2 layers21 × 33 mm24g2usb pico2w, the printed circuit board in 3D

Universal controller firmware for building adapters, dongles, and custom controllers.

Size
21 × 33 mm
Copper layers
2
Thickness
1.6 mm
Parts
5
Nets
14
Pads
28
Tracks, vias
24, 8
Routed
Yes
KiCad
KiCad 9.0 (file 20241229)
Created
18 Sep 2022
Updated
3 Nov 2026

Overview

24g2usb pico2w is an open-source printed circuit board by joypad-ai, from the joypad-ai/joypad-os repository on GitHub, published under the Apache-2.0 licence. It is a 2-layer board of 21 × 33 mm with 5 parts on 14 nets, routed with 24 tracks and 8 vias.

Its parts include 2 capacitors, 2 connectors and 1 IC. It belongs with the radio and wireless boards and the RP2350 boards of this library.

README

hardware/24g2usb_rp2350zero/README.md

24g2usb_rp2350zero carrier

Carrier PCB for the 24g2usb app: holds an nRF24L01+ mini SMD module and receives a Waveshare RP2350-Zero on female header sockets. Board: 18.5 x 26.0mm (the Zero's own footprint, plus a comfortable margin), 2-layer, 1.6mm FR4, 1oz copper.

Not yet fabricated or tested. This board is DRC-clean and its netlist is asserted against the firmware's wiring table, but no physical board has been built from these files. Treat it as a first spin: do the fit-check print and the module pad-order check below before ordering.

Everything here is generated from ../generate.py (--variant rp2350zero) -- edit the tables in that file and regenerate rather than hand-editing the .kicad_pcb. See its module docstring for the routing method and why it looks the way it does.

No KiCad GUI step is required before ordering. make gerbers zip produces a gerber/drill zip ready to upload as-is -- see "Ordering" below.

Mounting orientation -- read before soldering anything

The RP2350-Zero plugs in from above: female sockets soldered to this carrier's top face, Zero's male header pins pointing down into them. The carrier can also go above the Zero instead -- solder male header pins into J1 pointing down out of the carrier's bottom face, and plug those into a Zero that has female sockets fitted. Both ways put the module's antenna on the carrier's top face; mounting the carrier above additionally gives the antenna clear air above it with nothing overhead.

Never flip the board over to mate it. J1's two columns are not left-right symmetric (5V/GND/ 3V3/GPxx on one side, GP0-GP8 on the other) -- mating flipped swaps them and puts 3V3 across the SPI lines. Both faces are marked for this: "USB-C END" and the pin-1 marker (a square pad) are present on both the top and bottom face, so whichever face you solder a header to, orientation is never a guess. Through-hole pads are on *.Cu and *.Mask (both sides), so a socket or a header solders cleanly from either face.

BOM

See fab/bom.csv. Headline parts:

RefPartNotes
U1nRF24L01+ "Mini SMD" module, 1.27mm pitch, 12x18mm bodyHand-solder -- JLCPCB stocks none of these
J12x9 2.54mm female header, 15.24mm row spacingCut two 1x9 strips, or one 2x9 if you have it
C110uF 0805Bulk decoupling, right at the module's VCC/GND pads
C2100nF 0805HF decoupling, right at the module's VCC/GND pads

No RP2350-Zero on the BOM -- it's a separate board you already have, plugged into J1. This board has no breakout header for the Zero's unused pins and no mounting holes -- see "Known limitations."

Fab order settings (JLCPCB or similar)

  • 2 layers, 1.6mm thickness, 1oz copper, green soldermask, white silkscreen (defaults are fine)
  • Min track/space 0.3mm/0.2mm (signal), 0.9mm GND -- inside every fab's standard capability
  • Upload fab/24g2usb_rp2350zero-gerbers.zip (Gerber + Excellon drill, RS-274X)
  • This is a bare PCB order. JLCPCB has no nRF24 module in its assembly catalogue -- do not select PCBA/assembly for U1

Ordering

  1. make -C hardware/24g2usb_rp2350zero all (or generate drc gerbers zip render individually) regenerates the board, checks it, and produces everything in fab/ -- no GUI step needed.
  2. Print fab/24g2usb_rp2350zero-top-1to1.pdf at 100% scale (disable "fit to page" / "scale to fit" in your PDF viewer's print dialog) and lay your actual RP2350-Zero and nRF24 module on it -- the one check the software genuinely can't do for you. The print includes the module's TRUE 12x18mm body (on the fabrication-reference layer, not silkscreen -- see "Why the module outline isn't on silkscreen" below), including the antenna overhang past the board edge. Confirm J1's pad spacing matches the Zero's header pins, and that the module you have is really a single row of 8 pads at 1.27mm pitch -- seller listings for "mini nRF24L01+ SMD" modules aren't fully standardized, and this is the one mistake DRC can't catch.
  3. Check the module's pad ORDER. The board expects +3.3V, GND, CE, CSN, SCK, MOSI, MISO, IRQ along the row, VCC at the silkscreen-marked end. This is verified against the vendor dimension drawing for the common 12x18mm module (Sunrom model 3962, https://www.sunrom.com/p/rf-module-2-4ghz-nrf24l01-smd -- 12x18mm, 1.27mm pitch, first pad 1.6mm from the edge), which is what this footprint was built from. These modules are NOT standardised between sellers, though, and carry no silkscreen on the pad row, so if yours came from elsewhere, probe for continuity between each pad and any bare ground on the module (crystal can, or the ground fill around the antenna): exactly one pad should beep, and it must be the second from the +3.3V end. If GND appears at the far end of the row instead, that module needs a different footprint. A swapped VCC/GND kills the module on first power-up.
  4. Upload fab/24g2usb_rp2350zero-gerbers.zip to your fab of choice as a bare (non-assembled) 2-layer board.

Assembly order

  1. Module first (U1) -- hardest part to align, easiest to rework before anything else is in the way. Tack one corner pad, check alignment against the printed fit-check, then solder the rest.
  2. C1, C2 -- right next to U1's VCC/GND pads.
  3. J1 socket -- last, since it's the tallest part and the easiest to bump while soldering the others.
  4. Solder male headers to your RP2350-Zero (if not already fitted) and plug it into J1.

3V3, not 5V

The module's VCC pad is fed from the Zero's 3V3 pin, never 5V -- nRF24 modules are not 5V tolerant on their supply. This is called out on the silkscreen next to the module. If you're hand-wiring anything extra, don't cross it.

Why the module outline isn't on silkscreen

The nRF24 module's antenna genuinely overhangs the board edge on this carrier (by design -- see "Verification performed" below for the exact figure) with no copper underneath it. A full-length silkscreen outline of the module's true 12x18mm body would have to cross Edge.Cuts to show that overhang, and KiCad's DRC flags silk that crosses the board edge (silk_edge_clearance). Rather than ship that DRC note, the true body outline is drawn on F.Fab instead -- a fabrication reference layer, not printed ink, so it isn't DRC-constrained against the edge -- and the Makefile's 1:1 PDF/SVG exports include F.Fab specifically so the antenna overhang is still visible and checkable when you print it. Silkscreen itself just carries the pad labels, reference designators, and orientation markers; the pad copper marks the module's row on the physical board.

Verification performed

  • kicad-cli pcb drc --severity-all --exit-code-violations: 0 violations, 0 unconnected items, 0 schematic-parity issues.
  • Netlist assertion in generate.py passes: J1 and U1's pad-to-net mapping is checked against the wiring table from docs/apps/24g2usb.md / rf24g_host.h before any file is written.
  • Renders (fab/*.png, fab/*.svg) and the 1:1 PDF inspected: pads land on the expected nets, nothing routed under the module's antenna keepout, silkscreen legible, C1/C2 sit right next to U1's VCC/GND pads, board outline a plain rectangle, bottom face clean (no components, nothing obstructing the header holes). The module's antenna overhangs the board edge by about 7.75mm with no copper anywhere under it, confirmed both from the F.Fab outline in the 1:1 print and from the (automatically DRC-checked) antenna keepout zone.
  • Gerber round-trip: unzipped fab/24g2usb_rp2350zero-gerbers.zip and confirmed F.Cu, B.Cu, F.Silkscreen, B.Silkscreen, F.Mask, B.Mask, Edge.Cuts, the Excellon drill file, and the job file are all present, and that F.Cu/B.Cu actually contain the designed copper (0.3mm signal traces, 0.9mm GND traces, and the SMD/THT pad apertures) rather than an empty or pour-only layer.

Known limitations

  • No GPIO breakout header and no M2 mounting holes. An earlier revision of this board planned both, but at 18.5mm wide there wasn't room for either without conflicting with J1's own pads or routing -- see generate.py's comments near J1_POS/mounting-hole for the specific numbers. The board relies on J1's own socket for mechanical support.
  • Ground is carried by explicit 0.9mm-wide tracks, not a copper pour. kicad-cli's headless zone filler segfaults in this Docker toolchain even for a single trivial zone (confirmed, not assumed), so a pour would ship silently unfilled in the gerbers -- what the fab builds wouldn't match the design. Routing GND as an explicit track sidesteps the problem entirely rather than requiring a manual GUI fill-and-reexport step before every order.

Parts

5
QtyValueFootprintReferences
1joypad:nRF24L01_Mini_SMD_8P127U1
1joypad:Pico_Socket_1x5J3
1joypad:Pico_Socket_1x11J1
1100nFjoypad:C_0805_HandC2
110uFjoypad:C_0805_HandC1

More from joypad-ai/joypad-os

1
  • 2 layers18.5 × 26 mm24g2usb rp2350zero, the printed circuit board in 3D

    24g2usb rp2350zero

    joypad-ai/joypad-os

    Universal controller firmware for building adapters, dongles, and custom controllers.

    4 parts1.7kApache-2.0

Similar boards

  • 2 layers98 × 27 mmXy limit, the printed circuit board in 3D

    Xy limit

    opulo-inc/lumenpnp

    The LumenPnP is an open source pick and place machine.

    5 parts3.7k
  • 2 layers53.2 × 59.6 mmA10 OLinuXino Lime Rev B SHIELD TEMPLATE, the printed circuit board in 3D

    A10 OLinuXino Lime Rev B SHIELD TEMPLATE

    OLIMEX/OLINUXINO

    OLINUXINO is Open Source / Open Hardware, low cost from EUR 24 Linux Industrial grade Single Board Computer capable to operate -25+85C

    5 parts1.5k
  • 2 layers30 × 11 mmMain control board servo tester, the printed circuit board in 3D

    Main control board servo tester

    jamro/tiny-engineer

    A small desktop robot that brings an AI coding assistant to life, physically acting out when it reads files, thinks, writes code, and finishes work.

    5 parts1.1k
  • 2 layers78.8 × 35.3 mmKiCadTest, the printed circuit board in 3D

    KiCadTest

    hackclub/OnBoard

    💡 Join 1,000 teenagers and make your first PCB with a $100 grant!

    5 parts915
  • 2 layers50 × 23 mmMiniCircuits LTCC, the printed circuit board in 3D

    MiniCircuits LTCC

    VanceVagell/kv4p-ht

    Open source handheld ham radio project KV4P-HT

    5 parts828GPL-3.0
  • 2 layers20.3 × 15.2 mmL0 light sensor, the printed circuit board in 3D

    L0 light sensor

    Luos-io/luos_engine

    Open-source and real-time orchestrator for cyber-physical-systems, to easily design, test and deploy embedded applications and digital twins.

    5 parts546MIT

Questions

How big is the 24g2usb pico2w PCB?

It measures 21 × 33 mm and has 2 copper layers, 1.6 mm thick.

What parts does the 24g2usb pico2w use?

5 parts. The full list of its parts is on this page, with links to each part's symbol and footprint where PCBKit's library has them.

Where can I download the 24g2usb pico2w KiCad files?

From the joypad-ai/joypad-os repository on GitHub, at the commit this page was made from: the board is hardware/24g2usb_pico2w/24g2usb_pico2w.kicad_pcb. PCBKit opens the board in the browser, with nothing to install.

Can I use the 24g2usb pico2w design in my own project?

Its repository publishes it under the Apache-2.0 licence: you may reuse it on that licence's terms (keep the author's notice, and for a copyleft licence share your changes alike).