STM32 course

STM32 Course PCB — V0.1

A beginner-friendly introduction to STM32 hardware design and KiCad. This is a minimal black-pill-style board built around the STM32F103C8T6 (ARM Cortex-M3), designed while following Phil's Lab's free full tutorial:

KiCad 6 STM32 PCB Design Full Tutorial — Phil's Lab #65 A ~1h40m step-by-step walkthrough of an STM32-based PCB — schematic creation, two-layer layout and routing, through to manufacturing files.

This project is just a beginner intro to STM32 hardware design and KiCad — the design is intentionally kept simple (no ESD protection, no fancy features) while following good design practices taught in the course. It is a learning project, not production-ready hardware.

Features

• MCU: STMicroelectronics STM32F103C8T6 (Cortex-M3, 48-pin)
• Power supply: AMS1117-3.3 linear regulator, powered from USB (5V VBUS)
• USB: Micro-B connector, device-only USB-FS design
• Clock: 8 MHz crystal with load capacitors
• Debug/IO: SWD header, I2C bus with pull-ups
• 4x mounting holes

Course Overview

The video covers the complete PCB design workflow in three stages. This project follows it end to end:

1. Schematic

• STM32 microcontroller & decoupling — one 100nF cap per VDD/VBAT pin, based on ST recommendations
• Configuration pins — BOOT0 (run vs. bootloader mode) and NRST behavior
• Pin-out planning with STM32CubeIDE
• Crystal circuitry — load capacitor calculation from the crystal's CL spec
• USB — device-only design, D+ pull-up resistor per AN4879, differential pair routing
• Power supply & connectors — AMS1117-3.3 LDO, ferrite bead for the analog rail, USB Micro-B
• Electrical Rules Check (ERC) and annotation
• Footprint assignment

2. Layout

• PCB set-up — two-layer board stackup, track/via sizes, grid settings
• Placing the MCU with decoupling caps and crystal close by first
• USB and SWD layout
• Changing footprints, adding 3D models
• Switch & connector placement, power supply layout
• Mounting holes and board outline

3. Routing & Manufacturing

• Decoupling and crystal routing first (short traces)
• Signal routing, then power routing
• Finishing touches and Design Rules Check (DRC)
• Producing manufacturing files: BOM, CPL, Gerber, drill (e.g. for JLCPCB assembly)

Documentation

Schematic

PCB Layout

Both copper layers overlaid — top (F.Cu, red) and bottom (B.Cu, blue) shown together:

3D Render — Top View

Design Notes

These are the notes taken directly on the schematic during the design process:

Power Supply

• Capacitor values for the regulator were taken from the datasheet.
• A bulk capacitor is included as good design practice.
• The ferrite bead is a resistive load that dissipates heat at high frequencies.
• VBUS (USB power) is typically noisy; filtering could be added but is acceptable for this basic PCB.

Decoupling

• One decoupling capacitor per VDD and VBAT pin; 100nF selected based on ST recommendations.
• The analog supply (+3.3VA) is kept separate from the digital supply via a ferrite bead, with an additional decoupling capacitor for VDDA.

MCU Configuration

• BOOT0: pulled LOW → MCU executes code normally; pulled HIGH → MCU enters bootloader (can accept instructions over USB, UART, or I2C).
• NRST: pin is LOW when in reset. The MCU has an internal pull-up, so it can be left floating. A reset button could be added here, but a capacitor was used instead to keep NRST high and prevent accidental resets.
• VBAT: can be connected to an external battery for RTC usage, or simply tied to VCC.

Crystal Oscillator

• Load capacitance calculation: take the crystal's load capacitance (10pF), subtract stray capacitance (~3–5pF), multiply by 2 → CL = 2 × (CL0 − Ca) = 2 × (10pF − 5pF) = 10pF.
• Reference: ST oscillator design guide (AN2867)

USB

• The 1.5K resistor on D+ is based on application note AN4879 from ST — required for the STM32F1 series. The 1.5K value was also chosen because it's already used elsewhere in the design, reducing BOM size.
• This is a device-only USB design, so the cable shield is not connected to GND.
• No external ESD protection is included since this is an introductory tutorial project (some STM MCUs may have internal ESD protection — check the datasheet).
• USB differential pair routing: KiCad recognizes the pair by the + / - suffix in net labels.

I2C Pull-ups

• Standard pull-up value is 2.2K, values as low as 1K are acceptable. 1.5K was used here to reduce the BOM size.

Status

This repository contains the completed PCB (V0.1) following the full tutorial above.

Tools

• KiCad 10.x (the course itself uses KiCad 6, but the workflow is nearly identical)
• STM32CubeIDE for pin-out planning