Skip to the content
4 layers66.7 × 66.2 mmSTM32G474 Dev v3, the printed circuit board in 3D

4-layer STM32G474RE dev board (Nucleo-64 headers, USB-C, CAN-FD, STDC14) designed in KiCad 9: schematic, PCB layout, Gerbers & BOM

Size
66.7 × 66.2 mm
Copper layers
4
Thickness
1.6 mm
Parts
77
Nets
102
Pads
395
Tracks, vias
1,315, 387
Pours
4
Routed
Yes
KiCad
KiCad 10.0 (file 20260206)
Created
3 Oct 2026
Updated
23 Oct 2026

Overview

STM32G474 Dev v3 is an open-source printed circuit board by Rennaafi, from the Rennaafi/stm32g474-dev-board repository on GitHub, published under the MIT licence. It is a 4-layer board of 66.7 × 66.2 mm with 77 parts on 102 nets, routed with 1,315 tracks and 387 vias.

It is built around the MCP2562FD-E/SN, AP2112K-3.3 and USBLC6-2SC6, with the NUP2105L among its other parts. Its parts include 20 capacitors, 12 connectors, 10 resistors, 4 ICs and 4 diodes. It belongs with the microcontroller boards boards and the STM32 boards of this library.

Main components

4

README

README.md

STM32G474 Development Board (Nucleo-64 style, with USB-C and CAN-FD)

A 4-layer STM32G474RE (LQFP-64) development board designed in KiCad 9 and finalised in KiCad 10. It follows the NUCLEO-64 header layout (ST morpho CN7/CN10 plus Arduino Uno R3 headers) and adds a native USB-C port, a CAN-FD transceiver, an STDC14 debug connector and four corner mounting holes. There is no on-board ST-LINK; debugging uses an external STLINK-V3 on the STDC14 connector.

3D render, top

Status: schematic and layout are complete (ERC 0 errors · 0 unconnected · 4 DRC errors, all vendor-footprint hole clearance in the USB-C connector, see waivers.md). The slides from the KCCI PCB Design final presentation are in docs/presentation/. See Known limitations and Before ordering.

Features

  • MCU: STM32G474RE, LQFP-64, 170 MHz Cortex-M4F. HSE 16 MHz crystal, LSE 32.768 kHz crystal.
  • Headers: the MCU I/O pins reach the NUCLEO-64 morpho headers (CN7, CN10, 2x19 each) and the Arduino Uno R3 headers (CN5, CN6, CN8, CN9).
  • USB: native USB-C (USB 2.0 full speed) on PA11/PA12 with a USBLC6-2SC6 ESD protector. DFU works over this port (BOOT0 header).
  • CAN-FD: MCP2562FD transceiver on FDCAN2 (PB12 = RX, PB13 = TX), NUP2105L bus ESD protection, optional 120 ohm termination (solder jumper), 3-pin bus header J6. Needs +5 V (USB or the 5 V input).
  • Debug: STDC14 connector for STLINK-V3 (SWD + virtual COM port on PA2/PA3), plus a 1x6 SWD header.
  • Power: USB-C 5 V -> PTC fuse -> Schottky -> AP2112K-3.3 LDO. Ferrite-bead-filtered VDDA. IDD measurement jumper JP6 in the MCU supply.
  • User I/O: user LED, user button (PC13), reset button, power LED, test points (+5V, 3V3, VDDA, GND), GND probe hooks.
  • Mechanical: 66.75 x 66.25 mm, 77 parts (76 on top), 387 vias, 103 nets, four M3 plated corner holes tied to GND, rounded corners (R4).
  • Stack-up: 4 layers, signal / GND / GND / signal, 1.6 mm (JLC04161H-7628 values set in the board file).

Schematic

Schematic

The CAN-FD block:

CAN-FD block

Cropped views of each section (as used in the presentation) are in Media/schematic/:

Power input + ESDLDO
USB-C power input and ESDAP2112K LDO
MCUHSE / LSE crystals
MCUHSE
CAN-FDSWD + STDC14 debug
CAN-FDDebug

PCB Layout

Top and bottom (the bottom silkscreen carries the pin names of the headers):

TopBottom
PCB topPCB bottom

Floorplan (both signal layers) and the four layers on their own:

Floorplan

L1 signal + partsL2 GND
L1L2
L3 GNDL4 signal
L3L4

Isolation jumpers (solder bridges)

JumperDefaultPurpose
JP62-pin header (fit a jumper)IDD measurement: the MCU supply runs through it; remove the jumper and insert an ammeter to measure current
JP7bridgedBOOT0 pull-down; cut it to use D15/SCL (set nSWBOOT0 = 0 first)
JP9bridgeduser LED on D13/SCK; cut to unload that pin
JP10 / JP11bridgedUSB D-/D+ stubs on the PA11/PA12 morpho pins; cut to remove the stubs
JP12 / JP13bridgedCAN RXD/TXD on PB12/PB13; cut to get those morpho pins back
JP14open120 ohm CAN termination; bridge only on the two end nodes of a bus

Design notes

  • Stack-up. L1 signals + parts, L2 GND, L3 GND, L4 signals. Each signal layer sits next to a solid GND plane. There is no VDD plane: VDD is a trace tree (about 93 mm on L1 and 111 mm on L4, 19 vias) joining the MCU supply pins, their 100 nF caps (each placed at its pin), the bulk cap, the VDDA ferrite and the CN7 VDD pins. The MCU draws well under 100 mA, so this is electrically fine, but it is longer than ideal.
  • Return paths. 222 GND vias (return vias beside signal vias, plus edge stitching about every 4 mm). Of 165 non-GND vias, 82 have a GND via within 1 mm, 54 within 2 mm, 22 within 3 mm and 7 farther away; those 7 are CAN-area and +5 V vias added after the stitching pass (see limitations).
  • USB pair. Routed on L1 over the L2 GND plane, w 0.30 mm / gap 0.22 mm, 45-degree bends only. Total routed length D+ is 38.5 mm and D- is 35.1 mm (3.4 mm mismatch, irrelevant at 12 Mbps). Estimated differential impedance about 91 ohm (Hammerstad-Jensen single-ended + IPC-2141 coupling for JLC04161H-7628, 0.2104 mm prepreg, Er 4.4; range 87-93 ohm). scripts/zdiff.py reproduces the estimate. It is a closed-form estimate, not a field solver result.
  • Crystals. HSE and LSE are routed on L1 only, with no vias, short runs, and load capacitors at the crystal.
  • CAN-FD. CANH is 17.1 mm and CANL is 21.9 mm. The pair is not tightly coupled; at CAN bit times that is irrelevant, but it is not a controlled-impedance pair. PB12/PB13 reach the transceiver over long routes (about 50 mm and 70 mm), so set both GPIOs to low or medium speed in firmware.
  • Mounting holes. M3 plated pads tied to GND, centred 4 mm from each corner, with the corner arcs concentric to the holes.

Known limitations

  • VDD tree is long (one link loops around the top of the board) because the direct L4 corridors were already occupied.
  • Return vias: not every signal via has a GND via within 1 mm. The 7 vias farther than 3 mm are CAN-area and +5 V vias placed after the stitching pass.
  • CAN-FD block is spread out in the lower-right corner because that was the only free space; the pair is not tightly coupled.
  • Impedance was estimated, not confirmed in the fab's calculator.
  • DRC: 4 errors and 40 warnings under KiCad 10.0.6. The 4 errors are hole_clearance between the GND shield pads of the GCT USB4105 footprint and its own locating peg (0.194 mm against the 0.25 mm board rule). Warnings are silkscreen and library-link items. 0 unconnected items. See docs/reports/waivers.md.

Before ordering

  1. Run the fab's impedance calculator for the USB pair on JLC04161H-7628 and compare with about 91 ohm.
  2. Open every Gerber layer in a viewer (GerbView or the fab's own). Check L2 and L3 on their own, the outline (four arcs) and the drill file (four 3.2 mm holes).
  3. Verify the pinouts of U5 (MCP2562FD) and D4 (NUP2105L) against the datasheet of the exact parts you buy.
  4. Confirm the FDCAN2 pin mapping (PB12 = FDCAN2_RX, PB13 = FDCAN2_TX, AF9) in the STM32G474 datasheet.
  5. Check the BOOT0 / nSWBOOT0 option bytes (RM0440) if you use JP7.
  6. BOM/BOM.csv has no manufacturer part numbers, and BOM/CPL.csv rotations may need the fab's preview correction (SOIC-8, SOT-23, USB-C).
  7. Fit female 2x19 sockets on CN7/CN10. The footprint uses the male-pin pad pattern so the pin numbers match the Nucleo.

Versus the NUCLEO-G474RE

AreaNUCLEO-G474REThis board
USBMCU USB not brought to a connector on the boardNative USB-C on PA11/PA12 with ESD protection and DFU
CANFDCAN available on the MCU, no transceiverMCP2562FD transceiver, ESD protection, termination option, on FDCAN2
DebugOn-board ST-LINKSTDC14 connector for an external STLINK-V3
Layoutn/a4-layer S/GND/GND/S, GND-referenced signal layers, USB pair routed for about 90 ohm
FlexibilitySolder bridgesIsolation jumpers for BOOT0, LED, USB stubs and CAN pins
Mechanicsn/aFour corner M3 plated holes, rounded corners; morpho and Arduino headers kept

Repository Structure

text
.
├── STM32G474_Dev_v3.kicad_pro    # KiCad project
├── STM32G474_Dev_v3.kicad_sch    # Schematic
├── STM32G474_Dev_v3.kicad_pcb    # PCB layout (KiCad 10 file format)
├── Gerber/                       # Gerbers, drill files, job file (+ upload-ready zip)
├── BOM/                          # BOM.csv and CPL.csv (pick-and-place)
├── Media/                        # Renders, schematic images, per-layer views
├── docs/presentation/            # Final presentation slides (PDF)
├── docs/reports/                 # ERC and DRC reports, notes on the DRC results
└── scripts/zdiff.py              # USB pair impedance estimate

Notes on the files

  • A few parts use a personal KCCI symbol/footprint library (STM32G474RE, crystals, buttons, ferrite, polyfuse, Schottky). Those symbols and footprints are embedded in the schematic and board, so the project opens and checks cleanly without the library; the library itself is not included.
  • The board file references standard KiCad 3D models (${KICAD9_3DMODEL_DIR}); the 3D render in Media/ was made with local models.
  • The PCB file is saved in the KiCad 10 format and needs KiCad 10 to open. Designed in KiCad 9.0.7, final checks and the Gerber export with KiCad 10.0.6.
  • The Gerbers are the final export (the silkscreen carries the header pin names and the author's name and handle).

Parts

77
QtyValueFootprintReferences
11100nCapacitor_SMD:C_0603_1608MetricC3, C4, C5, C6, C8, C10, C12, C17, C18, C22, C23
6BridgedJumper:SolderJumper-2_P1.3mm_Bridged_RoundedPad1.0x1.5mmJP7, JP9, JP10, JP11, JP12, JP13
4MountingHole_PadMountingHole:MountingHole_3.2mm_M3_Pad_ViaH1, H2, H3, H4
4SolderJumper_2_OpenJumper:SolderJumper-2_P1.3mm_Open_Pad1.0x1.5mmJP1, JP2, JP3, JP4
310kResistor_SMD:R_0603_1608MetricR4, R6, R12
31kResistor_SMD:R_0603_1608MetricR3, R5, R7
210uCapacitor_SMD:C_0603_1608MetricC1, C2
212pCapacitor_SMD:C_0603_1608MetricC13, C14
21uCapacitor_SMD:C_0603_1608MetricC9, C11
25k1Resistor_SMD:R_0603_1608MetricR1, R2
25p1Capacitor_SMD:C_0603_1608MetricC15, C16
2Conn_02x19_Odd_EvenConnector_PinSocket_2.54mm:PinSocket_2x19_P2.54mm_VerticalCN7, CN10
2GND_HOOKConnector_PinHeader_2.54mm:PinHeader_1x02_P2.54mm_VerticalJ3, J4
2Green_LEDLED_SMD:LED_0603_1608MetricD2, D3
1+3V3TestPoint:TestPoint_Pad_D1.5mmTP2
1+5VTestPoint:TestPoint_Pad_D1.5mmTP1
1100Resistor_SMD:R_0603_1608MetricR11
1120Resistor_SMD:R_0805_2012MetricR13
14.7uCapacitor_SMD:C_0603_1608MetricC7
1500mKCCI:PolyFuse_1206_3216MetricF1
1600KCCI:BLM18PG121SN1DFB1
1AP2112K-3.3Package_TO_SOT_SMD:SOT-23-5U2
1ARD_ANALOGConnector_PinSocket_2.54mm:PinSocket_1x06_P2.54mm_VerticalCN8
1ARD_D0-D7Connector_PinSocket_2.54mm:PinSocket_1x08_P2.54mm_VerticalCN9
1ARD_D8-D15Connector_PinSocket_2.54mm:PinSocket_1x10_P2.54mm_VerticalCN5
1ARD_POWERConnector_PinSocket_2.54mm:PinSocket_1x08_P2.54mm_VerticalCN6
1BOOT0Connector_PinHeader_2.54mm:PinHeader_1x02_P2.54mm_VerticalJP5
1CANConnector_PinHeader_2.54mm:PinHeader_1x03_P2.54mm_VerticalJ6
1Conn_01x06_PinConnector_PinHeader_2.54mm:PinHeader_1x06_P2.54mm_VerticalJ2
1Crystal 16 MhzKCCI:TSX-3225Y1
1Crystal 32.768 KhzKCCI:TSX-3225Y2
1D_SchottkyKCCI:Schottky Diode_B5819W-TP_SOD3716X135ND1
1GNDTestPoint:TestPoint_Pad_D1.5mmTP4
1IDDConnector_PinHeader_2.54mm:PinHeader_1x02_P2.54mm_VerticalJP6
1MCP2562FD-E/SNPackage_SO:SOIC-8_3.9x4.9mm_P1.27mmU5
1NUP2105LPackage_TO_SOT_SMD:SOT-23D4
1RESETKCCI:button_434133025816SW2
1STDC14Connector_PinHeader_1.27mm:PinHeader_2x07_P1.27mm_Vertical_SMDJ5
1STM32G474RETxKCCI:STM32G474REU1
1TermJumper:SolderJumper-2_P1.3mm_Open_RoundedPad1.0x1.5mmJP14
1USBLC6-2SC6Package_TO_SOT_SMD:SOT-23-6U3
1USB_C_USB2.0Connector_USB:USB_C_Receptacle_GCT_USB4105-xx-A_16P_TopMnt_HorizontalJ1
1VDDATestPoint:TestPoint_Pad_D1.5mmTP3
1~KCCI:button_434133025816SW1

Similar boards

  • 2 layers120 × 64 mmSensor module, the printed circuit board in 3D

    Sensor module

    HasiKe/Hayabusa

    Eigenbau-Motorsteuerung und Umbauprojekte für die Suzuki Hayabusa der ersten Generation (1999–2007).

    138 parts
  • 8 layersFoc control, the printed circuit board in 3D

    Foc control

    sujaygouda123/foc-control

    BLDC field-oriented-control board for a humanoid robot actuator. KiCad 10, Ø80 mm, 8 layers, 1.6 mm.

    104 parts
  • 4 layers65 × 56.5 mmCANopy, the printed circuit board in 3D

    CANopy

    taciturnaxolotl/CANopy

    can hat design for raspberry pis

    42 parts1
  • 4 layers94 × 72.8 mmMain board v2, the printed circuit board in 3D

    Main board v2

    BlueJayRacing/22xt_kicad

    As a summary, you should be using KiCad Version 9.0. All project will be modular, and you should be storing all your step files, symbols, & footprints within the created folders.

    163 parts
  • 4 layers250 × 90 mmVCU V2, the printed circuit board in 3D

    VCU V2

    shutianx180/mk12-vcu-pcb

    366 parts
  • 2 layers50 × 40 mmSTM32 CAN USB, the printed circuit board in 3D

    STM32 CAN USB

    mihircn/stm32-usb-can-fd-adapter

    STM32G0B1-based USB-to-CAN FD adapter designed in KiCad.

    31 parts1
  • 2 layers125.3 × 55.3 mmStm32 can lin, the printed circuit board in 3D

    Stm32 can lin

    trnila/stm32_can_lin

    Set nSWBOOT0 to 0 using STM32CubeProgrammer for the first time, then connect the debugger and flash the device:

    103 parts
  • 2 layers48.5 × 34.6 mmAxiom thermocouple, the printed circuit board in 3D

    Axiom thermocouple

    robotical/axiom-thermocouple

    Thermocouple amp + microcontroller and JST SH / axiom magnetic connectors

    64 partsGPL-3.0

Questions

How big is the STM32G474 Dev v3 PCB?

It measures 66.7 × 66.2 mm and has 4 copper layers, 1.6 mm thick.

What parts does the STM32G474 Dev v3 use?

77 parts, built around the MCP2562FD-E/SN, AP2112K-3.3, USBLC6-2SC6 and NUP2105L. 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 STM32G474 Dev v3 KiCad files?

From the Rennaafi/stm32g474-dev-board repository on GitHub, at the commit this page was made from: the board is STM32G474_Dev_v3.kicad_pcb and its schematic STM32G474_Dev_v3.kicad_sch. PCBKit opens the board in the browser, with nothing to install.

Can I use the STM32G474 Dev v3 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).