Sgm modem is an open-source printed circuit board by ebixs, from the ebixs/smart-gas-meter-iot repository on GitHub. It is a 4-layer board of 75 × 50 mm with 57 parts on 38 nets, routed with 367 tracks and 354 vias.
It is built around the ESD224DQAR, DMG2302U and MMBT3904, with the M2.5 among its other parts. Its parts include 16 capacitors, 16 resistors, 6 transistors, 4 connectors and 2 ICs.
Status: v0.1-draft — engineering draft, NOT fabrication ready. The schematic follows the Quectel EC200U Series
Hardware Design V1.0; the PCB is a 4-layer layout study. The EC200U footprint is provisional: its pad geometry and
the pad that carries each pin number are placeholders built from the partial dimensions in the hardware design guide.
It must be replaced by Quectel's EC200U Series Footprint & Part file, and the board re-placed and re-routed, before
any layout review or order. Bench-only: MODEM_VIN comes from a current-limited 3.8 V supply. Never connect any of
this to a live gas meter, gas line, valve, mains or field wiring.
The board plugs onto the carrier board's modem header J6 (carrier v0.2, hardware/kicad/) with a socket J1
on its underside, pin for pin: 1 MODEM_VIN · 2 GND · 3 MODEM_TXD · 4 MODEM_RXD · 5 MODEM_EN · 6 MODEM_RESET · 7 MODEM_STATUS · 8 GND (3.3 V logic). It is the "replaceable modem board" of the hardware decisions.
What is here
Path
Purpose
design_modem_v01.py
Single source of truth: every part, value, footprint and pin → net assignment (same Part API as the carrier's design_v02.py)
tools/generate_schematic.py
Writes the schematic, project file and project-local libraries; reuses the carrier's sheet writer unchanged; generates the EC200U symbol and the provisional footprint
Project-local symbols, footprints and STEP models (nickname SGMM)
pcb_layout_modem_v01.py
Placement table (75 × 50 mm, 4 layers)
tools/build_pcb.py
Builds the board with KiCad's pcbnew module, fans ground and VBAT pads out to their planes, autoroutes with Freerouting, stitches the ground pours and writes a DRC report
sgm_modem.kicad_pcb
The routed layout study
check_netlist_matches_design.py
Netlist vs. design, pin by pin, plus J1 pin-out = carrier J6
tests/
Design invariants (no 3V3 on the modem, open-collector PWRKEY/RESET_N, every 1.8 V output shifted, …)
exports/
Schematic PDF, netlist, DRC report, layer artwork
Circuit (from the EC200U hardware design guide)
VBAT — MODEM_VIN (3.3–4.3 V, 3.8 V nominal, up to 2 A bursts) feeds VBAT_RF (57, 58) and VBAT_BB (59, 60).
Two 100 µF low-ESR tantalum capacitors, a 100 nF / 33 pF / 10 pF MLCC set at each pin pair, and a TVS diode with
≥ 4.7 V stand-off (to be selected). On the PCB the whole inner layer In2 is the VBAT plane (the guide asks for
≥ 2–2.5 mm VBAT traces). J2 is an optional direct VBAT input, not fitted: never run it in parallel with carrier J7.
PWRKEY / RESET_N — open-collector MMBT3904 drivers (4.7 kΩ base resistor, 47 kΩ base pull-down) from
MODEM_EN / MODEM_RESET. The carrier's 100 kΩ pull-downs keep the module off while the ESP32 boots.
Switching on or off needs PWRKEY low for ≥ 2 s.
Level shifting — the module's UART and STATUS are 1.8 V. Three N-MOSFET shifters with their gates on
VDD_EXT (the module's own 1.8 V output, 2.2 µF) and 10 kΩ pull-ups on the 1.8 V side. Candidate FET:
Diodes DMG2302U (VGS(th) ≤ 1.0 V); a BSS138 is marginal with a 1.8 V gate.
(U)SIM — JAE SF53S006VCBR2000 micro-SIM, 0 Ω series resistors, 33 pF on each line, 10 kΩ pull-up on DATA,
100 nF on USIM_VDD and a TI ESD224 array (0.5 pF; the guide's limit is 15 pF).
Antenna — ANT_MAIN on a short 50 Ω line (net class RF, 0.35 mm over the In1 ground plane — confirm with the
fabricator's stack-up) to a Hirose u.FL, with a π network (0 Ω + two not-mounted shunts).
Network LED — NET_STATUS drives a green LED through a transistor, about 1.8 mA from VBAT.
Bench access — test pads for the module USB (VBUS, D+, D−) and the 1.8 V debug UART; solder jumper JP1 with
4.7 kΩ to VDD_EXT forces USB download mode when closed before power-up (open by default).
Review items (open)
Footprint: replace the provisional EC200U footprint with Quectel's file; then re-place and re-route.
MCU-side pull-ups: J6 carries no 3.3 V rail, so MODEM_RXD and MODEM_STATUS rely on the ESP32's internal
pull-ups (firmware must enable them). Alternative: add 3V3 to the next carrier revision's modem header.
TVS selection for VBAT, exact MPNs for the tantalum capacitors and the MOSFETs.
Header current: one 2.54 mm pin carries MODEM_VIN bursts of up to 2 A; check the socket rating or use J2.
RF line width against the real stack-up; tune the π network with the chosen antenna.
Verification (2026-10-26, KiCad 7.0.11 here; CI repeats ERC/DRC with KiCad 9)
Check
Result
Netlist vs. design (check_netlist_matches_design.py)
The board's exploded 3D model is in hardware/visualization/boards/modem.html, and the schematic can be explored
net by net in hardware/visualization/schematic/index.html.
It measures 75 × 50 mm and has 4 copper layers, 1.6 mm thick.
What parts does the Sgm modem use?
57 parts, built around the ESD224DQAR, DMG2302U, MMBT3904 and M2.5. 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 Sgm modem KiCad files?
From the ebixs/smart-gas-meter-iot repository on GitHub, at the commit this page was made from: the board is hardware/kicad-modem/sgm_modem.kicad_pcb and its schematic hardware/kicad-modem/sgm_modem.kicad_sch. PCBKit opens the board in the browser, with nothing to install.
Can I use the Sgm modem design in my own project?
Its repository states no licence, so its author keeps all rights: ask ebixs before reusing the design.