Skip to the content
2 layers16.4 × 10 mmOpenDongle CH570, the printed circuit board in 3D

OpenDongle CH570 is a compact USB Type-A 2.4 GHz receiver built around the WCH CH570Q RISC-V wireless MCU. The PCB is 16.4 mm x 10.0 mm and uses a PCB-edge USB connector and an independently created, WCH-informed 2.4…

Size
16.4 × 10 mm
Copper layers
2
Thickness
0.84 mm
Parts
9
Nets
11
Pads
35
Tracks, vias
34, 22
Pours
2
Routed
Yes
KiCad
KiCad 10.0 (file 20260206)
Created
12 Jul 2026
Updated
25 Oct 2026

Overview

OpenDongle CH570 is an open-source printed circuit board by openkeyboard-org, from the openkeyboard-org/OpenDongle repository on GitHub. It is a 2-layer board of 16.4 × 10 mm with 9 parts on 11 nets, routed with 34 tracks and 22 vias.

It is built around the CH570Q. Its parts include 4 capacitors, 1 resistor, 1 IC, 1 connector and 1 crystal.

Main components

1

README

hardware/CH570/README.md

OpenDongle CH570

OpenDongle CH570 is a compact USB Type-A 2.4 GHz receiver built around the WCH CH570Q RISC-V wireless MCU. The PCB is 16.4 mm x 10.0 mm and uses a PCB-edge USB connector and an independently created, WCH-informed 2.4 GHz PCB antenna.

Design files

File or directoryPurpose
OpenDongle-CH570.kicad_proKiCad 10 project and design-rule settings
OpenDongle-CH570.kicad_schSchematic
OpenDongle-CH570.kicad_pcbPCB layout
lib/OpenDongle.kicad_symProject-owned CH570Q and four-pin PCB USB symbols
lib/OpenDongle.pretty/Project-owned USB edge connector and independently created, WCH-informed antenna footprints
sym-lib-table, fp-lib-tablePortable project-local library configuration
fab/Exported outputs: schematic PDF and gerber/NC drill set (see Fabrication outputs)

Open the project with KiCad 10 or later. The library tables use ${KIPRJMOD} paths, so the project resolves every symbol and footprint from this directory and does not depend on global KiCad configuration. Nothing needs to be added to your global symbol or footprint library tables.

Electrical design notes

  • USB VBUS supplies the CH570Q V5 pin (pin 2) directly. There is no external regulator; the CH570 regulates 3.3 V internally.
  • R1 is the 1.5 kOhm connection required by WCH between V5 and the internally regulated VDD33/VIO33 rail (pin 1) for direct 5 V operation.
  • Both V5 and VDD33/VIO33 have 2.2 uF bulk and 100 nF high-frequency decoupling: C1/C2 on V5, C3/C4 on VDD33.
  • Y1 is a 32 MHz, 8 pF-load crystal on XI/XO (pins 9 and 8). The CH570 provides programmable internal crystal load capacitance, so external load capacitors are not fitted.
  • The RF output (ANT, pin 10) connects directly to the independently created, WCH-informed PCB antenna, as recommended by the CH570 datasheet.
  • USB data connects to the CH570Q native USB pins: D+ to PA1/UDP (pin 4) and D- to PA0/UDM (pin 3).
  • GND reaches the CH570Q through the exposed pad (pin 11).
  • The three unused GPIOs (pins 5, 6, 7) carry no-connect flags.
  • AE2 and J1 represent copper footprints fabricated as part of the PCB. They are excluded from the assembly BOM and position file at both the symbol level (in_bom no, in_pos_files no) and the footprint level (exclude_from_bom, exclude_from_pos_files), so they do not appear in the Fabrication Toolkit output as unsourceable line items.

See the WCH CH572/CH570 datasheet for the power, oscillator, RF, USB, and package requirements.

Design verification

This design passes both checks cleanly with KiCad 10:

sh
kicad-cli sch erc --severity-all OpenDongle-CH570.kicad_sch     # 0 errors, 0 warnings
kicad-cli pcb drc --severity-all --schematic-parity OpenDongle-CH570.kicad_pcb   # 0 violations, 0 parity issues

Fabrication outputs

fab/ holds the exported outputs: the schematic as PDF, and the gerber/NC drill set under fab/gerbers/. The KiCad sources remain the design of record — regenerate the exports with KiCad 10 whenever the schematic or layout changes:

sh
kicad-cli sch export pdf -o fab/OpenDongle-CH570-schematic.pdf OpenDongle-CH570.kicad_sch
kicad-cli pcb export gerbers -o fab/gerbers/ \
    -l F.Cu,B.Cu,F.Paste,B.Paste,F.Silkscreen,B.Silkscreen,F.Mask,B.Mask,Edge.Cuts \
    --no-protel-ext --check-zones OpenDongle-CH570.kicad_pcb
kicad-cli pcb export drill -o fab/gerbers/ --excellon-separate-th \
    --generate-map --map-format gerberx2 OpenDongle-CH570.kicad_pcb

Anyone ordering from these files must still pass the stackup and antenna requirements below to the fabricator; the gerbers alone do not carry them. (JLC-oriented assembly outputs from the Fabrication Toolkit plugin go to production/, which stays untracked.)

Fabrication requirements

The antenna geometry and USB connector make the board construction part of the electrical and mechanical design. Use these settings unless a revised PCB has been validated:

ParameterRequirement
Layer count2 copper layers
Finished board size16.4 mm x 10.0 mm
Finished thickness0.8 mm nominal (35 um + 0.73 mm core + 35 um)
MaterialFR-4
Copper1 oz / 35 um outer copper
Surface finishENIG recommended; hard gold on the USB contacts is preferred for high insertion-cycle production
Minimum finished drill0.20 mm
Minimum track/space used0.15 mm track, 0.127 mm design-rule clearance minimum
SoldermaskBoth sides; no soldermask over the USB contacts or antenna conductor

Additional requirements and checks:

  1. Preserve the antenna copper, ground keepout, board thickness, and via fence exactly. The antenna is designed for 0.8 mm FR-4; a different thickness detunes it. Do not allow the fabricator to add serial numbers, tooling features, or anything else in the antenna region.
  2. Keep the board outline and USB contact geometry at 1:1 scale. If an edge bevel is requested, confirm that the fabricator supports it on a 0.8 mm board without shortening or damaging the USB contacts.
  3. Verify the board USB contact fits in several Type-A receptacles before a production run.
  4. The enclosure and carrier must not place metal or conductive material over the antenna region.

USB receiver shell

This USB receiver shell has been verified to fit and work well with the PCB. Other shells designed for the same PCB dimensions and specification should also work, but their fit has not been verified.

Suggested BOM

The listed LCSC/JLCPCB numbers are suggested assembly parts, not sole-source requirements. Substitutes should match the value, package, dielectric/tolerance, voltage rating, and crystal parameters.

ReferencesQtyValue / partPackageSuggested LCSC partNotes
U11WCH CH570QDFN-10, 3 mm x 3 mm, exposed padC49260680Confirm pin-1 orientation and exposed-pad soldering
Y1132 MHz crystal2016, 4 padC376353328 pF load, +/-10 ppm tolerance, 40 ohm maximum ESR
R111.5 kOhm, 1%0603C22843Required V5-to-VDD33 connection
C1, C322.2 uF0603C23630X5R or better, 10 V minimum; suggested part is 16 V
C2, C42100 nF0603C14663X7R or better, 10 V minimum

AE2 (PCB antenna) and J1 (PCB USB connector) are fabricated as PCB copper and are not assembly parts.

Source attribution

  • The 0.8 mm FR-4 antenna was independently created, informed by the WCH reference antenna published in the openwch schematic/PCB library; no WCH CAD or artwork file was copied, imported, converted, or traced.
  • The PCB USB connector footprint is derived from the USB armory hardware design.

License

This hardware design, including the independently created antenna implementation described in ../NOTICE, is licensed under the CERN Open Hardware Licence Version 2 - Weakly Reciprocal. See LICENSE.

Parts

9
QtyValueFootprintReferences
2100nFCapacitor_SMD:C_0603_1608MetricC2, C4
22.2µFCapacitor_SMD:C_0603_1608MetricC1, C3
11.5kResistor_SMD:R_0603_1608MetricR1
132MHzCrystal:Crystal_SMD_2016-4Pin_2.0x1.6mmY1
1CH570QPackage_DFN_QFN:DFN-10-1EP_3x3mm_P0.5mm_EP1.7x2.5mmU1
1PCB AntennaOpenDongle:ANT-F-2-2.4G-0.8MM-FR4-WCHAE2
1PCB USBOpenDongle:usb-PCBJ1

More from openkeyboard-org/OpenDongle

1
  • 2 layers16.3 × 9.9 mmOpenDongle CH592, the printed circuit board in 3D

    OpenDongle CH592

    openkeyboard-org/OpenDongle

    OpenDongle CH570 is a compact USB Type-A 2.4 GHz receiver built around the WCH CH570Q RISC-V wireless MCU. The PCB is 16.4 mm x 10.0 mm and uses a PCB-edge USB connector and an independently created, WCH-informed 2.4…

    9 parts4

Similar boards

  • 2 layers53 × 73.5 mmCh32v305-radioset, the printed circuit board in 3D

    Ch32v305-radioset

    cnlohr/cnhardware

    My dumping grounds for all my kicad projects and random hardware bringup.

    71 parts114
  • 2 layers34.6 × 10.9 mmCh570funprog, the printed circuit board in 3D

    Ch570funprog

    cnlohr/ch570funprog

    CH570-based RISC-V Programmer

    25 parts6MIT
  • 2 layers103 × 30.5 mmTS Back Endcap, the printed circuit board in 3D

    TS Back Endcap

    EEVengers/ThunderScope

    ThunderScope GitHub Repo

    9 parts1.3kMIT
  • 2 layers31.8 × 47.6 mmNGC 38 connector, the printed circuit board in 3D

    NGC 38 connector

    rusefi/rusefi

    rusefi - GPL internal combustion engine control unit

    9 parts1.2k
  • 2 layers24 × 27.3 mmExpansion Card Retrofit, the printed circuit board in 3D

    Expansion Card Retrofit

    FrameworkComputer/ExpansionCards

    Reference designs and documentation to create Expansion Cards for the Framework Laptop

    9 parts1.1kCC-BY-4.0
  • 2 layers15.6 × 17.3 mmSKR Mini TFT Thermistor Board, the printed circuit board in 3D

    SKR Mini TFT Thermistor Board

    VoronDesign/Voron-Hardware

    Cool Hardware designed by the Voron Design group

    9 parts1.1kGPL-3.0
  • 2 layers39.1 × 49.5 mmLearnoliver, the printed circuit board in 3D

    Learnoliver

    hackclub/OnBoard

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

    9 parts915
  • 2 layers17.4 × 16.9 mmToolhead, the printed circuit board in 3D

    Toolhead

    tanaes/whopping_Voron_mods

    9 parts787GPL-3.0

Questions

How big is the OpenDongle CH570 PCB?

It measures 16.4 × 10 mm and has 2 copper layers, 0.84 mm thick.

What parts does the OpenDongle CH570 use?

9 parts, built around the CH570Q. 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 OpenDongle CH570 KiCad files?

From the openkeyboard-org/OpenDongle repository on GitHub, at the commit this page was made from: the board is hardware/CH570/OpenDongle-CH570.kicad_pcb and its schematic hardware/CH570/OpenDongle-CH570.kicad_sch. PCBKit opens the board in the browser, with nothing to install.

Can I use the OpenDongle CH570 design in my own project?

Its repository states no licence, so its author keeps all rights: ask openkeyboard-org before reusing the design.