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…
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.
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 directory
Purpose
OpenDongle-CH570.kicad_pro
KiCad 10 project and design-rule settings
OpenDongle-CH570.kicad_sch
Schematic
OpenDongle-CH570.kicad_pcb
PCB layout
lib/OpenDongle.kicad_sym
Project-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-table
Portable 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.
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:
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:
Parameter
Requirement
Layer count
2 copper layers
Finished board size
16.4 mm x 10.0 mm
Finished thickness
0.8 mm nominal (35 um + 0.73 mm core + 35 um)
Material
FR-4
Copper
1 oz / 35 um outer copper
Surface finish
ENIG recommended; hard gold on the USB contacts is preferred for high insertion-cycle production
Minimum finished drill
0.20 mm
Minimum track/space used
0.15 mm track, 0.127 mm design-rule clearance minimum
Soldermask
Both sides; no soldermask over the USB contacts or antenna conductor
Additional requirements and checks:
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.
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.
Verify the board USB contact fits in several Type-A receptacles before a production run.
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.
References
Qty
Value / part
Package
Suggested LCSC part
Notes
U1
1
WCH CH570Q
DFN-10, 3 mm x 3 mm, exposed pad
C49260680
Confirm pin-1 orientation and exposed-pad soldering
Y1
1
32 MHz crystal
2016, 4 pad
C37635332
8 pF load, +/-10 ppm tolerance, 40 ohm maximum ESR
R1
1
1.5 kOhm, 1%
0603
C22843
Required V5-to-VDD33 connection
C1, C3
2
2.2 uF
0603
C23630
X5R or better, 10 V minimum; suggested part is 16 V
C2, C4
2
100 nF
0603
C14663
X7R 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.
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…
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.