

Moskvich ecu
Programmable ignition ECU for Moskvich 412/2140 (ESP32-C3, web tuner)
- Size
- 48 × 41.8 mm
- Copper layers
- 2
- Thickness
- 1.6 mm
- Parts
- 45
- Nets
- 24
- Pads
- 127
- Tracks, vias
- 502, 47
- Pours
- 2
- Routed
- Yes
- KiCad
- KiCad 7 (file 20221018)
- Created
- 26 Oct 2026
- Updated
- 26 Oct 2026
Overview
Moskvich ecu is an open-source printed circuit board by pachobg2, from the pachobg2/moskvich_ignition repository on GitHub. It is a 2-layer board of 48 × 41.8 mm with 45 parts on 24 nets, routed with 502 tracks and 47 vias.
It is built around the ISL9V3040P3, CD74HCT221M96 and BZT52C3V6, with the M2.5, 1N4148W and BC847B among its other parts. Its parts include 16 resistors, 11 capacitors, 6 diodes, 3 ICs and 2 transistors. It belongs with the ESP32 and RISC-V boards of this library.
Main components
8ISL9V3040P3
TO-220-40℃~+175℃@(Tj) 1.3V@1mA 1.6V@6A,4V 150W 17nC 21A 4.8us 430V 700ns TO-220 IGBT Transistors / Modules ROHSonsemiIGBT Transistors / ModulesCD74HCT221M96
SOIC-16-55℃~+125℃ 18ns 2 4.5V~5.5V 4mA 4mA 74HCT Monostable Reset input、Adjustable pulse width、Dual edge triggering Schmitt trigger SOIC-16 Monostable Multivibrators ROHSTexas InstrumentsMonostable MultivibratorsBZT52C3V6
SOD-123Zener DiodeshongjiachengM2.5
-0.45mm 2.5mm 2mm 5mm DIN934 Hex M2.5X0.45 Nickel plated Silver white - Hexagonal nutsShuntianHex Nut1N4148W
SOD-123150mA 1A 1V@50mA 1uA@75V 400mW 4ns 75V Independent SOD-123 Switching Diodes ROHSSTMicroelectronicsSwitching DiodesBC847B
SOT-23-65℃~+150℃ 1 NPN 100MHz 100mA 200 200mV 250mW 45V 5uA 6V NPN SOT-23 Bipolar (BJT) ROHSNexperiaBipolar (BJT)SMBJ24A
DO-214AA(SMB)-55℃~+150℃ 15.4A 24V 26.7V 38.9V 5uA 600W TVS Unidirectional DO-214AA(SMB) ESD and Surge Protection (TVS/ESD) ROHSGOODWORKESD And Surge Protection (TVS/ESD)SS34
SMA(DO-214AC)-55℃~+125℃ 3A 40V 500uA@40V 550mV@3A Independent SMA(DO-214AC) Schottky Diodes ROHSMDDSchottky Diodes
README
hardware/README.mdECU hardware — schematic, PCB, BOM (rev B, SMD)
A small two-sided board: SMD passives and ICs (0603 / 0805 / 1206 / 1210, SOT-23, SOIC-16, SMA/SMB), an SMD buck regulator for the 5 V rail, an ESP32-C3-Zero on pin sockets, 3.5 mm screw terminals, and the ignition IGBT lying in a cut-out so the case floor cools it. 48 × 41.8 mm (about a third of the through-hole rev A).
| File | What it is |
|---|---|
schematic.svg | One-sheet schematic (open in any browser) |
pcb_top.svg, pcb_bottom.svg | Board previews (both copper layers, courtyards, cut-out) |
moskvich_ecu.kicad_sch | Editable schematic, KiCad 7 format (every pin has a net label; no hand-routed wires). Its netlist is checked identical to the PCB's. |
moskvich_ecu.kicad_pro | Minimal KiCad project so the schematic and PCB open together |
moskvich_ecu.kicad_pcb | The PCB, KiCad 7 format (footprints embedded, tracks, vias, GND pours, outline + cut-out) |
bom.csv, netlist.csv | Parts list and net list |
gen/pcbgen.py | Generator: parts, placement, auto-router, design-rule check, KiCad/SVG/BOM export |
gen/gen_schematic.py | Draws schematic.svg (the readable picture) |
gen/gen_kicad_sch.py | Writes moskvich_ecu.kicad_sch and verifies it against the PCB netlist |
Regenerate everything (needs numpy scipy shapely):
python hardware/gen/pcbgen.py && python hardware/gen/gen_schematic.py && python hardware/gen/gen_kicad_sch.pyStatus — read this. The board was generated and checked by my own script: copper clearance ≥ 0.2 mm (≥ 0.7 mm around the coil net), every net connected, nothing within 0.5 mm of the edge or inside the cut-out, no footprint overlaps, no hole collisions. The file parses in a KiCad-format library. It has not been opened in KiCad, run through KiCad's DRC, or built. The footprints are generic IPC-style land patterns I defined, not manufacturer drawings. Before ordering: open it in KiCad ≥ 7, press B to fill the zones, run Inspect → Design Rules Checker, and compare every footprint with the datasheet of the exact part you buy (especially the inductor, the fuse, the terminals and the module).
Opening it in KiCad or EasyEDA
- KiCad 7+: open
moskvich_ecu.kicad_pro. The schematic uses simple embedded symbols (boxes with named pins) and the footprint names of the PCB; reassign footprints/symbols to library parts as you like, then Update PCB from schematic. - EasyEDA: import the files through EasyEDA's KiCad import (File → Import; menu names differ between the Standard and Pro editions — I have not tried it here). Import the schematic and the PCB; if the editor complains, open them in KiCad first and re-export. Replace the generic footprints with EasyEDA/LCSC library parts (this also gives JLCPCB assembly part numbers).
- The schematic is a grouped parts-and-nets drawing: connections are carried by net labels, not long wires.
schematic.svgis the readable hand-arranged picture of the same circuit. - Neither file was opened in KiCad/EasyEDA by me; the script re-reads the schematic and checks every pin's net against the PCB netlist (42 symbols, 24 nets, no mismatches).
Circuit in one paragraph
Ignition-switched 12 V → 0.5 A fuse → SS34 Schottky (reverse polarity) → SMBJ24A TVS → 10 µF → AP63205 buck (3.8–32 V in, fixed 5 V, 2 A; L = 4.7 µH, 2 × 22 µF out, 100 nF boot — the datasheet's values) → 5 V. The points signal (J1.1) is pulled up through 1 kΩ (wetting current), divided and inverted by a BC847 into GPIO4. The LPG valve signal, the battery voltage and the MAP sensor each go through a divider with a 100 nF cap and a 3.6 V zener into ADC1 pins. The MCU's coil command (GPIO6) feeds a CD74HCT221 monostable that (a) turns the 3.3 V logic into a 5 V gate drive and (b) limits coil-on time in hardware (≈ 16–23 ms with the 15 kΩ / 2.2 µF network; the firmware limits it to 9 ms first), so a hung MCU can never leave the coil charged. It drives the ISL9V3040P3 ignition IGBT; its collector (the tab) is the coil negative (J1.4). Coil current never flows through the buck or the sensor grounds: it uses the 1.5 mm top-layer collector track and the GND pours / J1.3.
Board facts
- 48 × 41.8 mm, 2 layers, 1.6 mm, three M2.5 mounting holes. Origin = top-left corner, X right, Y down (as in KiCad).
- Rules used: tracks 0.2 mm (signal) / 0.4 mm (power) / 1.5 mm (collector), clearance 0.2 mm (0.7 mm around the collector net), vias 0.8 / 0.4 mm, GND pours on both layers. These are within normal 2-layer fab capabilities.
- Top side: module sockets, J1/J2, the IGBT pads, and the buck stage (U2, L1, C1–C4, C11, D1, D2, F1).
- Bottom side: everything else (dividers, points input, the CD74HCT221 and its resistors). The bottom parts sit in the 6 mm gap between the board and the case floor, so keep them ≤ 3 mm tall.
- Terminals: J2 (top right) = LPG signal, +5 V, MAP signal, GND. J1 (right) = points lead, +12 V, GND, coil −. The coil track and the GND pour handle the 4 A pulses; use ≥ 1 mm² wire on J1.3 / J1.4.
- The module's USB-C faces the top edge (2.2 mm from it).
Mounting the IGBT through the cut-out
The IGBT is cooled by the case floor, which acts as the heat sink.
box floor (aluminium) ───────────────────────────── z = 0
│ ┌ M3 screw into a tapped hole in the floor
tab ─┴─ insulating pad (silicone, 0.25 mm) + shoulder washer
TO-220 lies flat in the cut-out ───► leads bent UP through the 3 pads
PCB on 6 mm standoffs ───────────────────────────── z = 6- Cut-out: 18.0 × 13.0 mm window at x 3.64 … 21.64, y 27.79 … 40.79 (bottom-left of the board). The strip below it is only 1.0 mm wide — handle the board by the edges.
- Lead pads (Q1), 3.0 mm to the right of the window, 2.54 mm pitch, 1.0 mm drill: collector (24.64, 34.29), emitter (24.64, 31.75), gate (24.64, 36.83) — the part is rotated 180° compared with a part lying leads-left, so the gate is the lowest pad. The silkscreen outline shows the package.
- Tab hole ends up near (8.1, 34.3) (the board is the drilling template through the cut-out). Check against your real part before drilling the floor.
- Lead forming: leave ~4 mm flat from the package, bend up 90°, trim to just clear the board top.
- The tab is the coil negative (battery voltage plus spikes to ~400 V). Insulate it from the case: silicone pad + plastic shoulder washer under the screw head. Check with a multimeter that tab ↔ case is open before powering the board.
- Dissipation is ≈ 2–3 W at 6000 rpm (≈ 0.3 W at idle); the floor of a metal box is plenty. On a plastic box use a real heat sink bolted to the tab.
- Conformal-coat the board: the collector net sees ~400 V flyback spikes with only 0.7–0.8 mm clearance.
Parts and where the numbers come from
| Item | Notes |
|---|---|
| AP63205WU-7 (U2) | Pinout, 4.7 µH / 10 µF / 2 × 22 µF / 100 nF and "EN to VIN" are from the Diodes datasheet (DS41326). Abs. max VIN 35 V DC / 40 V for 400 ms — hence the SMBJ24A TVS (clamps ≈ 39 V). Fit enough ceramic capacitance after derating (X7R/X5R lose capacity with DC bias). |
| L1 | Any shielded 4.7 µH inductor, I_sat ≥ 2 A, DCR < 100 mΩ, about 4 × 4 mm. The land pattern is generic: adjust it to your part. |
| F1 | An SMD fuse (0.5 A, ≥ 32 V rating) or a PTC of the same 1206 size. Ordinary 1206 PTCs are often rated only 6–15 V: do not use those. |
| C10 / R14 | 2.2 µF X7R + 15 kΩ ⇒ guard time ≈ 0.7·R·C (CD74HCT221 datasheet), with the capacitor derated by its DC bias: 16–23 ms. If you change them keep it above the firmware's 9 ms and below ~25 ms. |
| ESP32-C3-Zero pad order | Pad numbers/GPIOs follow the Waveshare list (1 = 5V, 2 = GND, 3 = 3V3, 4–9 = IO0…IO5 down the left side, 10–18 = IO6, IO7, IO8, IO9, IO10, IO18, IO19, IO20, IO21 up the right side, USB at the top). Read the silkscreen on your module and measure the header row distance (15.24 mm assumed). |
| Module antenna | I did not leave a copper-free zone under the module (SMD parts and pours sit under its body); check where the antenna is on your revision and, if needed, move parts and add a keep-out there. |
| MAP sensor connector | J2.2 +5 V, J2.3 signal, J2.4 GND. GM-style sensors are usually A = ground, B = signal, C = 5 V — check yours. |
Bring-up
- Without the module, the CD74HCT221 and the IGBT: power from a bench supply (current limit 0.3 A). Check +5 V, check reverse polarity is blocked, check the TVS does not conduct at 14.4 V.
- Fit U3 and the module, flash, join
Moskvich-ECU. LED: blue blip = stopped, yellow = cranking, green = petrol, cyan = LPG, violet = simulator / OTA. - Tools → Bench simulator at 800 / 3000 / 6000 rpm with a 100 Ω resistor and LED, or a scope, instead of the coil on J1.4. Check one pulse per trigger and on-time = the dwell shown in the Live tab.
- Hold the command high on purpose (firmware stopped, jumper 3.3 V → GPIO6): the CD74HCT221 output must drop after ≈ 16–23 ms.
- Only then fit Q1, connect the coil and the distributor, and follow
docs/HARDWARE.md.
Not done / ideas
- No gerbers: export them from KiCad (File → Plot) after the DRC. Add a fab note and silk text.
- Hand-soldering: everything is 0603 or larger; the SOIC-16 and TSOT-23-6 need a fine tip and flux. Solder the buck IC and its caps first, then check the 5 V rail.
- A coil-current sense resistor and an IGBT over-current limit were left out to keep the build simple.
- Unused module pins on the left header (IO2, IO5) are unconnected — a coolant-temperature divider would use IO2 (ADC1).
Parts
45| Qty | Value | Footprint | References |
|---|---|---|---|
| 6 | 100nF | C_0603 | C2, C6, C7, C8, C9, C11 |
| 4 | 10k | R_0603 | R2, R11, R13, R16 |
| 3 | 22k | R_0603 | R3, R7, R9 |
| 3 | BZT52C3V6 | D_SOD-123 | D4, D5, D6 |
| 3 | M2.5 | MountingHole_2.7_M2.5 | H1, H2, H3 |
| 2 | 100R | R_0603 | R10, R15 |
| 2 | 100k | R_0603 | R6, R8 |
| 2 | 15k | R_0603 | R12, R14 |
| 2 | 22uF 10V | C_0805 | C3, C4 |
| 1 | 0.5A 32V fuse | Fuse_1206 | F1 |
| 1 | 10nF | C_0603 | C5 |
| 1 | 10uF 50V | C_1210 | C1 |
| 1 | 1N4148W | D_SOD-123 | D3 |
| 1 | 1k | R_0603 | R5 |
| 1 | 1k 0.25W | R_1206 | R1 |
| 1 | 2.2uF 25V X7R | C_0805 | C10 |
| 1 | 4.7k | R_0603 | R4 |
| 1 | 4.7uH | L_4x4 | L1 |
| 1 | AP63205WU-7 | SOT-23-6 | U2 |
| 1 | BC847B | SOT-23 | Q2 |
| 1 | CD74HCT221M96 | SOIC-16_3.9x9.9mm_P1.27mm | U3 |
| 1 | ESP32-C3-Zero | ESP32-C3-Zero_2x9_Socket | U1 |
| 1 | ISL9V3040P3 | TO-220_LayDown_Cutout | Q1 |
| 1 | Power | TerminalBlock_P3.50_1x04 | J1 |
| 1 | SMBJ24A | D_SMB | D2 |
| 1 | SS34 | D_SMA | D1 |
| 1 | Sensors | TerminalBlock_P3.50_1x04 | J2 |
Similar boards
- 2 layers31.2 × 35.8 mm

- 4 layers159.6 × 161 mm

Shack interface
PE1RGU/hf-antenna-switch
Remote HF antenna switch: 3 radios x 4 antennas (path to 8), outdoor relay unit with a hardware safety chain, controlled over Cat6 from a shack interface. KiCad 10, open hardware, designed together with an AI.
290 parts2CERN-OHL-S-2.0 - 2 layers54.1 × 27.4 mm

ICM
OpenLogicEFI/Hardware
Hardware is based off an open source project called Speeduino by Josh Stewart.
9 parts19 - 2 layers120.4 × 99.9 mm

- 2 layers202.6 × 66 mm

Wafel eval board
LVladymyr/WAFEL-Evaluation-Board
Evaluation board for TI BQ76952 multi-chemistry BMS IC
253 partsCERN-OHL-S-2.0 - 2 layers65 × 53 mm

Kline l9637d
quangvd917/ab125-kline
Bản mới của kline-l9637d: C3 SuperMini cắm thẳng lên mạch qua rào cái, không còn giắc J2. PCB một mặt, kích thước 70 × 38 mm, để tự làm. Firmware dùng env c3supermini như cũ, không phải sửa.
23 parts2 - 2 layers140 × 125 mm

- 2 layers65 × 76 mm

Raspi HAT
4rynv/VacDepoctrl
Open source firmware for a automation of vacuum systems controlled using Raspberry pi
36 parts1
Questions
How big is the Moskvich ecu PCB?
It measures 48 × 41.8 mm and has 2 copper layers, 1.6 mm thick.
What parts does the Moskvich ecu use?
45 parts, built around the ISL9V3040P3, CD74HCT221M96, BZT52C3V6 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 Moskvich ecu KiCad files?
From the pachobg2/moskvich_ignition repository on GitHub, at the commit this page was made from: the board is hardware/moskvich_ecu.kicad_pcb and its schematic hardware/moskvich_ecu.kicad_sch. PCBKit opens the board in the browser, with nothing to install.
Can I use the Moskvich ecu design in my own project?
Its repository states no licence, so its author keeps all rights: ask pachobg2 before reusing the design.