Skip to the content
2 layers48 × 41.8 mmMoskvich ecu, the printed circuit board in 3D

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

8

README

hardware/README.md

ECU 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).

FileWhat it is
schematic.svgOne-sheet schematic (open in any browser)
pcb_top.svg, pcb_bottom.svgBoard previews (both copper layers, courtyards, cut-out)
moskvich_ecu.kicad_schEditable 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_proMinimal KiCad project so the schematic and PCB open together
moskvich_ecu.kicad_pcbThe PCB, KiCad 7 format (footprints embedded, tracks, vias, GND pours, outline + cut-out)
bom.csv, netlist.csvParts list and net list
gen/pcbgen.pyGenerator: parts, placement, auto-router, design-rule check, KiCad/SVG/BOM export
gen/gen_schematic.pyDraws schematic.svg (the readable picture)
gen/gen_kicad_sch.pyWrites moskvich_ecu.kicad_sch and verifies it against the PCB netlist

Regenerate everything (needs numpy scipy shapely):

bash
python hardware/gen/pcbgen.py && python hardware/gen/gen_schematic.py && python hardware/gen/gen_kicad_sch.py

Status — 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.svg is 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.

text
   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

ItemNotes
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).
L1Any 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.
F1An 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 / R142.2 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 orderPad 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 antennaI 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 connectorJ2.2 +5 V, J2.3 signal, J2.4 GND. GM-style sensors are usually A = ground, B = signal, C = 5 V — check yours.

Bring-up

  1. 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.
  2. Fit U3 and the module, flash, join Moskvich-ECU. LED: blue blip = stopped, yellow = cranking, green = petrol, cyan = LPG, violet = simulator / OTA.
  3. 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.
  4. Hold the command high on purpose (firmware stopped, jumper 3.3 V → GPIO6): the CD74HCT221 output must drop after ≈ 16–23 ms.
  5. 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
QtyValueFootprintReferences
6100nFC_0603C2, C6, C7, C8, C9, C11
410kR_0603R2, R11, R13, R16
322kR_0603R3, R7, R9
3BZT52C3V6D_SOD-123D4, D5, D6
3M2.5MountingHole_2.7_M2.5H1, H2, H3
2100RR_0603R10, R15
2100kR_0603R6, R8
215kR_0603R12, R14
222uF 10VC_0805C3, C4
10.5A 32V fuseFuse_1206F1
110nFC_0603C5
110uF 50VC_1210C1
11N4148WD_SOD-123D3
11kR_0603R5
11k 0.25WR_1206R1
12.2uF 25V X7RC_0805C10
14.7kR_0603R4
14.7uHL_4x4L1
1AP63205WU-7SOT-23-6U2
1BC847BSOT-23Q2
1CD74HCT221M96SOIC-16_3.9x9.9mm_P1.27mmU3
1ESP32-C3-ZeroESP32-C3-Zero_2x9_SocketU1
1ISL9V3040P3TO-220_LayDown_CutoutQ1
1PowerTerminalBlock_P3.50_1x04J1
1SMBJ24AD_SMBD2
1SS34D_SMAD1
1SensorsTerminalBlock_P3.50_1x04J2

Similar boards

  • 2 layers31.2 × 35.8 mmIgniter, the printed circuit board in 3D

    Igniter

    jephilp/22RE_Igniter

    Drop-in replacement for 22RE igniter modules.

    45 parts1GPL-3.0
  • 4 layers159.6 × 161 mmShack interface, the printed circuit board in 3D

    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 mmICM, the printed circuit board in 3D

    ICM

    OpenLogicEFI/Hardware

    Hardware is based off an open source project called Speeduino by Josh Stewart.

    9 parts19
  • 2 layers120.4 × 99.9 mmDP1600iAuxTop, the printed circuit board in 3D

    DP1600iAuxTop

    Hocus-Pocus/Speeduino-DP1600i-

    73 parts1
  • 2 layers202.6 × 66 mmWafel eval board, the printed circuit board in 3D

    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 mmKline l9637d, the printed circuit board in 3D

    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 mmMinimood, the printed circuit board in 3D

    Minimood

    heolfief/minimood

    [WIP] STM32F4 based audio synthesizer

    142 parts2GPL-3.0
  • 2 layers65 × 76 mmRaspi HAT, the printed circuit board in 3D

    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.