Openrz67-nrf is an open-source printed circuit board by mhellevang, from the mhellevang/openrz67-trigger repository on GitHub, published under the MIT licence. It is a 2-layer board of 29.5 × 29 mm with 15 parts on 44 nets, routed with 66 tracks and 13 vias.
It is built around the E73-2G4M08S1F, TLP172AM(E and CL31A107MQHNNNE, with the AO3401A, B3U-1000P and MY-2032-16 among its other parts. Its parts include 3 capacitors, 3 resistors, 3 ICs, 2 connectors and 1 diode. It belongs with the radio and wireless boards and the ESP32 and RISC-V boards of this library.
KiCad 10 project for the coin-cell trigger: 29.5 × 29 mm, 2 layers, Ebyte E73-2G4M08S1F
(nRF54L15) module, CR2032 clip on the back, two TLP172AM PhotoMOS relays, JST SH 1.0 mm
side-entry camera connector, a second SH connector for SWD, one button, one LED, a P-MOSFET against a reversed cell. No regulator, no charger, no power
switch. Concept stage, not fabricated.
The schematic and the board are generated: tools/design.py holds parts, placement,
nets and every track, and the two generators write the KiCad files from it. Edit the model
and run tools/regen.sh; do not edit the .kicad_sch / .kicad_pcb by hand, the next
run overwrites them.
File
What
tools/design.py
the design: parts with LCSC numbers, positions, nets, tracks, vias, keepout
tools/gen_sch.py
writes openrz67-nrf.kicad_sch: one symbol per part, a global label on every used pin, a no-connect on every unused one
runs both generators, then exports everything in out/ and runs DRC (with schematic parity) and ERC
tools/fetch_3d.sh
downloads STEP+WRL models for every LCSC part in the BOM into openrz67-nrf.3dshapes/
tools/module_3d.py
box model of the E73 module (none on LCSC or from Ebyte): uv run tools/module_3d.py
tools/export_step.sh
board STEP to out/openrz67-nrf.step (gitignored); fetches missing part models first
openrz67-nrf.3dshapes/
3D models; .wrl committed (renders), .step gitignored except the module's
openrz67-nrf.kicad_sym, openrz67-nrf.pretty/
project libraries: LCSC/EasyEDA imports via easyeda2kicad and KiCad's R
out/
generated: Gerber+drill zip, position file, BOM with LCSC numbers, schematic PDF, top/bottom renders, DRC/ERC reports
Regenerate
sh
tools/regen.sh
Close KiCad first. Needs kicad-cli and KiCad's bundled python (for pcbnew); override with
KICAD_CLI=… KICAD_PY=…. It exits non-zero on any DRC/ERC error or unconnected pad.
Circuit
The cell (VBAT) feeds the module through Q1, an AO3401A P-MOSFET with its drain on the
clip, source on VDD and gate on GND. The right way round the body diode conducts until the
channel turns on (under 85 mΩ at VGS = −2.5 V, about 1 mV at 15 mA). A cell put in upside
down leaves it off, so VDD never goes negative. The module has one supply pad (9, 1.8–3.6 V
per Ebyte; the nRF54L15 itself starts at 1.75 V) and both crystals inside. 100 µF sits at the clip terminal, ahead of Q1 (a ceramic, a reversed cell does not harm it),
100 nF right at module pad 9 (C3, ground straight to pad 10) and 100 nF at Q1/SWD (C2).
Each PhotoMOS LED is driven from a GPIO through 220 Ω: about 4 mA at 2.7 V with the worst-case
LED forward voltage, the TLP172AM needs up to 3 mA. The status LED has 1 kΩ (about 1 mA).
With a fresh cell both relays and the LED draw about 14 mA, inside Nordic's recommended 15 mA
sustained total for all GPIOs.
The PhotoMOS outputs go to the camera connector; camera ground (CAM_GND)
is a separate net from the cell's GND. J1 has the camera port's pin order, so the camera
cable is wired straight through. Pigtail wire colours vary; go by pin position, pin 1 is next
to the white dot.
nRF54L15
Module pad
Function
P1.04
7
button to GND, internal pull-up, wake from System OFF
P2.00
18
status LED through 1 kΩ
P2.04
27
S1 PhotoMOS LED through 220 Ω
P2.05
28
S2 PhotoMOS LED through 220 Ω
SWCLK / SWDIO
11 / 12
J2 pins 3 / 4
nRESET
19
not brought out; reset over SWD
The button has to be on P0 or P1: P2 cannot wake the chip from System OFF. The three outputs run
at high drive (S0H1) so the PhotoMOS LEDs get their 5 mA. The left pad column faces the board
edge; VDD (pad 9) and the button (pad 7) leave it on two tracks between the module and the edge.
Connectors:
Ref
Pin
Signal
J1 camera, SH 1.0 mm (Qwiic/STEMMA QT cable)
1
not connected (camera 6 V)
2
camera ground
3
S1
4
S2
J2 SWD, SH 1.0 mm (Qwiic cable to the probe)
1
GND
2
VDD. With the cell out, the probe's 3.3 V powers the board here. Never with the cell in: it would charge the CR2032
3
SWCLK
4
SWDIO
Design rules
Clearance 0.127 mm, min track 0.127, default track 0.20 (signals 0.16, power 0.25), via
0.45/0.25, hole-to-track 0.175, hole-to-hole 0.30, copper-to-edge 0.30, mask expansion
0.051. JLCPCB silkscreen minimums (1.0 mm text, 0.15 mm line). A rule area over the
module antenna (x 0–15, y 0–5.3) keeps copper, tracks and vias off both layers.
Accepted warnings
DRC and ERC have 0 errors. The warnings left in the reports:
Check
Count
What
ERC endpoint_off_grid
17
Pins of the imported symbols are not on the 1.27 mm grid. Connectivity is by label; verified by the schematic-parity DRC.
silk_over_copper
11
The holder footprint's own silkscreen crosses its centre pad. Fab clips it.
Mechanical
Outline 29.5 × 29 mm, R0.8 corners, no mounting holes. All parts on top except the cell clip
on the back. Module antenna end is flush with the top edge (y = 0); both SH connectors sit along the
bottom edge with their mouths facing it (y = 29), SWD left of camera (the SWD cable is a
lid-off job, no wall opening); the button sits bottom-left, the LED between the two connectors.
Part
Height over the board
CR2032 clip BT1 (back)
3.75 mm, the cell under it; cell centre (13.5, 18), slides in from either long side
J1 camera and J2 SWD connectors
2.9 mm, body 6.0 × 4.3 each
Module U1
2.4 mm (Ebyte drawing)
BT1 is only the positive clip (MYOUNG drawing: "TERMINAL(+)"). The cell's negative face
rests on the Ø10 mm bare pad in the middle of the back. It has no paste, so the cell rests on
the pad's finish, not on a solder dome with flux on it. On the back a copper-free ring 7.5 to 10.2 mm from the cell centre lies
under the cell's rim, where the + can wraps over the edge; inside the ring only GND copper,
the same potential as the cell face resting on it. Ebyte's manual gives no antenna keepout figure; the rule area covers the
PCB antenna (the module's top 5.2 mm) plus 2 mm to its right. The module's 3D model is a plain box from
tools/module_3d.py: blue PCB with the antenna, grey shield.
A modern remake of the Bare Conductive Touch Board: 12 capacitive touch electrodes, MP3/WAV/MIDI audio, and now WiFi, Bluetooth LE, USB-C, a proper LiPo power path, a fuel gauge, line-in, MIDI out, Qwiic and an RGB LED.
Kestrel H7: STM32H743 FPV flight controller with ICM-20602 + BMI088, MS5611, 16 MB blackbox, 5 V and switchable 10 V BECs.
114 partsCERN-OHL-S-2.0
Questions
How big is the Openrz67-nrf PCB?
It measures 29.5 × 29 mm and has 2 copper layers, 1.6 mm thick.
What parts does the Openrz67-nrf use?
15 parts, built around the E73-2G4M08S1F, TLP172AM(E, CL31A107MQHNNNE and AO3401A. 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 Openrz67-nrf KiCad files?
From the mhellevang/openrz67-trigger repository on GitHub, at the commit this page was made from: the board is nrf/kicad/openrz67-nrf.kicad_pcb and its schematic nrf/kicad/openrz67-nrf.kicad_sch. PCBKit opens the board in the browser, with nothing to install.
Can I use the Openrz67-nrf design in my own project?
Its repository publishes it under the MIT licence: you may reuse it on that licence's terms (keep the author's notice, and for a copyleft licence share your changes alike).