STM32L4Q5CGT AudioSpectrumAnalyzer

STM32 Audio Spectrum Analyzer - Custom PCB

This repository contains a small KiCad board (4 layers) for an audio spectrum analyzer. The board has an STM32L4Q5CGT6, an I2S microphone, a pin header for a Waveshare 2inch LCD Module (ST7789) and USB-C power.

The top side of the board in the KiCad 9.0 3D viewer, with all 3D models loaded.

This project uses an STM32L4Q5CGT6 microcontroller (MCU) to decrease the dimensions of the board. This MCU also has almost the same functions as most STM32 performance-line MCUs from ST that are applicable to this project. The initial prototype used a Nucleo-F767ZI board (refer to Related projects).

The board has these functions:

• It receives power and USB data through the USB-C receptacle.
• It reads audio from an ICS-43434 I2S microphone on the board.
• It controls the LCD module with SPI.

Note: This repository contains only project files (schematic Revision A, date 2026-03-31). It does not contain fabrication outputs, assembly data, test results or firmware for this board.

Features

• STM32L4Q5CGT6: Arm Cortex-M4, a maximum of 120 MHz, 1024 KB flash, 320 KB RAM, LQFP-48 package
• USB-C for 5 V power and USB 2.0 full-speed data, with ESD protection
• SPX3819 3.3 V LDO (500 mA) that supplies one +3V3 rail for all the parts on the board
• ICS-43434 MEMS microphone (I2S, 24-bit) on the board, connected to the SAI2 pins
• 1x8 pin header for a Waveshare 2inch LCD Module (ST7789) on SPI1
• Tag-Connect TC2030 footprint for SWD
• BOOT0 and RESET switches

Hardware

Primary parts

The schematic contains the name of the manufacturer, the MPN and the LCSC part number of each BOM part.

Pinout

The power pins are:

• U3 pin 1 and J2 pin 1 are +3V3.
• U3 pin 2 and J2 pin 5 are GND.
• On the microphone, pin 5 is VDD (+3V3) and pin 3 is GND. LR (pin 2) connects to GND.

The schematic gives only the interface names (SPI or SAI), not the peripheral names. The peripheral names in parentheses in the table are from the KiCad STM32L4Q5CGTx symbol.

Board

• 94.5 x 39.7 mm, with 1 mm rounded corners and four M3 mounting holes
• 4 layers: a top layer for signals, two inner GND planes, and a bottom layer for signals and a +3V3 pour
• Approximately 1.6 mm thick, with a HAL lead-free finish, a green solder mask and a white silkscreen
• The microphone is on the bottom side. All other parts are on the top side.

Circuit

• Power path. VBUS from the USB-C receptacle goes through a 2.2 µH series inductor (L1) into the SPX3819 LDO. Each side of L1 has a 2.2 µF capacitor. The LDO is on when USB power is available, because its EN pin connects to its input. One +3V3 rail supplies power to all items on the board: VDD, VDDA, VDDUSB, the Waveshare 2inch LCD Module and the microphone. VBAT also connects to +3V3, and the board has no battery for VBAT.
• USB. 5.1 kΩ pull-down resistors on CC1 and CC2 identify the board as a USB sink. D+ and D- go through the USBLC6-2SC6 to PA12 and PA11. The SBU pins have no connection.
• Clock. A 16 MHz crystal with C0G load capacitors (10 pF) connects to PH0/PH1. The crystal footprint has a front-copper keep-out area. This area prevents copper pour below the crystal. The board has no 32.768 kHz LSE crystal (PC14/PC15 have no connection).
• Microphone. The ICS-43434 is on the bottom side. Its footprint has a 0.5 mm hole through the board for the acoustic port of the microphone. WS, SCK and SD connect to PB12, PB13 and PB15.
• Display. The board has a pin header footprint for the Waveshare 2inch LCD Module. This LCD module was available before the project, and it connects directly to the pin header. The board has a silkscreen outline with the label "2inch LCD Module". The board also has four 3.2 mm holes for the mounting holes of the LCD module. The LCD module is on the left two-thirds of the board, and all other parts are on the right third.
• BOOT0 and RESET. S1 connects BOOT0 (PH3) to +3V3. When S1 is open, a 10 kΩ resistor keeps BOOT0 low. S2 connects NRST to GND. Each of the two lines has a 100 nF filter capacitor.

How to start

1. Install KiCad 10.0 or a higher version.

   Note: The project files are in the KiCad 10 format. KiCad 9 and previous versions cannot open these files.

2. Clone the repository:

   git clone https://github.com/OscarBazylewich/STM32_Audio_Spectrum_Analyzer_CustomPCB.git

3. Open STM32L4Q5CGT-AudioSpectrumAnalyzer.kicad_pro in KiCad.

   Note: The project files contain the symbols and the footprints. Thus, KiCad opens the project without other libraries.

4. If you want the full 3D view (View > 3D Viewer in the PCB Editor), install the JLCPCB KiCad Library with the Plugin and Content Manager.

   Note: KiCad uses the ${KICAD8_3RD_PARTY} path variable to find the 3D models for X1, S1, S2, L1 and C1.

   If KiCad does not show the 3D models of these parts, do these steps:

   1. Open Preferences > Configure Paths.
   2. If the list does not contain KICAD8_3RD_PARTY, add a path variable with this name.
   3. Set ${KICAD8_3RD_PARTY} to the folder that contains 3dmodels/com_github_CDFER_JLCPCB-Kicad-Library.

5. In the Schematic Editor, do the ERC.

6. In the PCB Editor, do the DRC.

7. In the PCB Editor, go to File > Fabrication Outputs > Gerbers.

8. Set an output folder, for example gerbers/.

   Note: The output folder in the saved plot settings is the project folder. If you do not set an output folder, KiCad writes the output files to the project folder.

9. Select the copper, mask, paste, silkscreen and Edge.Cuts layers.

10. Click Plot.

11. Click Generate Drill Files....

12. In the Generate Drill Files dialog, click Generate.

As an alternative to steps 7 to 12, use these commands in the repository folder:

kicad-cli pcb export gerbers --output gerbers/ STM32L4Q5CGT-AudioSpectrumAnalyzer.kicad_pcb
kicad-cli pcb export drill --output gerbers/ STM32L4Q5CGT-AudioSpectrumAnalyzer.kicad_pcb

Repository structure

.
├── STM32L4Q5CGT-AudioSpectrumAnalyzer.kicad_pro   # KiCad 10 project: design rules, net classes, BOM fields
├── STM32L4Q5CGT-AudioSpectrumAnalyzer.kicad_sch   # Schematic on one sheet (Revision A)
├── STM32L4Q5CGT-AudioSpectrumAnalyzer.kicad_pcb   # 4-layer PCB layout, 94.5 x 39.7 mm
├── .gitattributes                                  # Lets GitHub count the KiCad files in its language statistics
├── LICENSE                                         # GNU GPL v3.0
└── README.md

3D renders

The KiCad 9.0 renders include all 3D models, but the board corners are not rounded. The KiCad 10.0 renders do not include all 3D models (the 3D models of X1, S1, S2, L1 and C1 are missing). But these renders show the added GND pour on layers 1 and 4, and the rounded corners of the board outline in this repository.

KiCad 9.0: top side	KiCad 9.0: bottom side
KiCad 10.0: top side	KiCad 10.0: bottom side

Related projects

• STM32_Audio_Spectrum_Analyzer_ST7789_and_INMP441: This project is the initial prototype and its firmware. It uses a Nucleo-F767ZI board, an ST7789 display and an INMP441 microphone.

Credits

• Oscar Bazylewich made this KiCad project.
• The footprints and 3D models for X1, S1, S2, L1 and C1 are from the JLCPCB KiCad Library of CDFER. The symbols for X1, S1 and S2 are also from this library.
• The symbol and the outline of the Waveshare 2inch LCD Module are from a custom library.
• All other symbols, footprints and 3D models are from the standard KiCad libraries.

License

The license of this project is the GNU General Public License v3.0. Refer to LICENSE.