4 layers66 × 60 mm
MainFlightComputer
RockSat-X/RSXVT2026
Our experiment aims to evaluate the use of optical navigation with Commercial-off-the-Shelf (COTS) products for use in spaceflight applications.
72 parts3MIT
2 layers20.3 × 10.2 mm
Lsm6dsv32x breakout
godmar/imuboard-claudeA minimal breakout for the ST LSM6DSV32X 6-axis IMU (±32 g accel, ±4000 dps gyro). The circuit follows the mode 1 connection diagram in ST's datasheet (DS13511, Figure 28, section 7.1).
- Size
- 20.3 × 10.2 mm
- Copper layers
- 2
- Thickness
- 1.6 mm
- Parts
- 11
- Nets
- 11
- Pads
- 38
- Tracks, vias
- 49, 7
- Pours
- 4
- Routed
- Yes
- KiCad
- KiCad 9.0 (file 20241229)
- Created
- 27 Sep 2026
- Updated
- 27 Sep 2026
Overview
Lsm6dsv32x breakout is an open-source printed circuit board by godmar, from the godmar/imuboard-claude repository on GitHub. It is a 2-layer board of 20.3 × 10.2 mm with 11 parts on 11 nets, routed with 49 tracks and 7 vias.
It is built around the LSM6DSV32X. Its parts include 3 capacitors, 3 resistors, 1 IC and 1 connector. It belongs with the interfaces and adapters boards of this library.
Main components
1README
README.mdLSM6DSV32X Breakout
A minimal breakout for the ST LSM6DSV32X 6-axis IMU (±32 g accel, ±4000 dps gyro). The circuit follows the mode 1 connection diagram in ST's datasheet (DS13511, Figure 28, section 7.1).
| Board size | 20.32 × 10.2 mm, 2 layers, 1.6 mm FR4. The width is set by the 8-pin header; the height meets JLCPCB's 10 × 10 mm minimum for assembly. |
| Mounting | Two M2 holes (2.2 mm, non-plated) in the top corners, 15.72 mm apart, 1.9 mm from the top edge. There is no copper within 2 mm of each hole, so a screw head or washer can't short anything. |
| Supply | 3.3 V only. VDD and VDDIO are tied together; there is no regulator or level shifter. |
| Interface | I²C / I3C (default) or SPI (3/4-wire) |
| I²C address | 0x6B (SA0 pulled up by R3). Drive SDO low for 0x6A. |
| Parts | All SMD on top (0402 passives). The header is inserted from the bottom, so its plastic spacer sits under the board. |
Header pinout (J1, 2.54 mm, pin 1 = square pad, left when viewed from the top)
| Pin | 1 | 2 | 3 | 4 | 5 | 6 | 7 | 8 |
|---|---|---|---|---|---|---|---|---|
| Signal | 3V3 | GND | INT2 | CS | SCL / SPC | SDA / SDI | SDO / SA0 | INT1 |
The order follows the ring of IMU pads, so every signal is routed on the top layer without crossings. The pin names are printed on the back silkscreen.
Circuit notes
- C1 / C2: 100 nF ceramic on VDDIO and VDD, placed next to the supply pins (datasheet Table 2 note 2, section 7.1).
- C3: 4.7 µF footprint on 3V3; may help if the board is fed through long wires or from a noisy robot supply.
- R1 / R2: 10 k pull-ups on SCL / SDA (Rpu = 10 kΩ per Figure 28), enabled through JP1, a solder jumper that is bridged by default. Cut the trace between its pads to remove the pull-ups, for example when the bus already has pull-ups or when using SPI.
- R3: 10 k pull-up on SDO/SA0. The SA0 pin has no internal pull-up by default, so without R3 the I²C address would be undefined. In SPI mode SDO actively drives the line, so R3 does no harm.
- CS has an internal pull-up, so the part starts in I²C/I3C mode. Pull CS low to use SPI.
- SDx/SCx (pins 2/3) are tied to GND because the analog hub, Qvar and sensor hub are not used. OCS_Aux/SDO_Aux (pins 10/11) are left unconnected. Both follow the datasheet's pin table.
- Axes: U1 is rotated 180° on the board. The front silkscreen arrow shows +X pointing left and +Y pointing toward the header; +Z points out of the top face.
Files
| File | Contents |
|---|---|
lsm6dsv32x_breakout.kicad_pro/.kicad_sch/.kicad_pcb | KiCad 9 project |
imuboard.kicad_sym, sym-lib-table | Project symbol library (LSM6DSV32X symbol) |
fab/lsm6dsv32x_breakout_gerbers.zip | Gerbers + Excellon drill files, ready to upload |
fab/*_bom.csv, fab/*_pos_top.csv | BOM and top-side pick-and-place file (origin: bottom-left corner) |
fab/*_bom_jlcpcb.xlsx, fab/*_cpl_jlcpcb.xlsx (+ .csv) | The same in JLCPCB's assembly upload format, matching their sample files (SMD parts only; J1 is fitted by hand) |
fab/*_schematic.pdf, fab/*_assembly_top.pdf | Printable schematic and assembly drawing |
fab/erc.rpt, fab/drc.rpt | Check reports (0 ERC, 0 DRC, 0 unconnected, 0 schematic-parity issues) |
tools/ | Generator scripts that produce the files above |
The design is generated from scripts. tools/design.py holds the netlist,
tools/gen_schematic.py writes the schematic, and tools/gen_pcb.py does placement,
routing, the GND pours on both layers, and the silkscreen. To rebuild everything, including
the fab outputs and the checks:
./tools/make_fab.shYou can also edit the .kicad_sch / .kicad_pcb files directly in KiCad. Regenerating
overwrites those edits.
Fabrication rules used
- Clearance 0.15 mm (the LGA's 0.5 mm pitch pads are 0.15 mm apart)
- Tracks 0.2 mm for signals, 0.3 mm for 3V3
- Vias 0.5 mm diameter / 0.3 mm drill, tented
- Copper to board edge 0.25 mm
- Copper keepout of 2 mm radius around each mounting hole
These are within standard JLCPCB/PCBWay 2-layer capabilities. The LGA-14 needs stencil and reflow (or hot air) assembly.
The library footprints' silkscreen was moved to the Fab layers because the board is too dense for it. For the same reason the project ignores the "footprint differs from library" DRC check.
Parts
11| Qty | Value | Footprint | References |
|---|---|---|---|
| 3 | 10k | Resistor_SMD:R_0402_1005Metric | R1, R2, R3 |
| 2 | 100nF | Capacitor_SMD:C_0402_1005Metric | C1, C2 |
| 2 | MountingHole_M2 | MountingHole:MountingHole_2.2mm_M2 | H1, H2 |
| 1 | 4.7uF | Capacitor_SMD:C_0402_1005Metric | C3 |
| 1 | Conn_01x08 | Connector_PinHeader_2.54mm:PinHeader_1x08_P2.54mm_Vertical | J1 |
| 1 | I2C_PU | Jumper:SolderJumper-2_P1.3mm_Bridged_RoundedPad1.0x1.5mm | JP1 |
| 1 | LSM6DSV32X | Package_LGA:LGA-14_3x2.5mm_P0.5mm_LayoutBorder3x4y | U1 |
Similar boards
- 4 layers25 × 74 mm
PTR mini pcb
PTR-projects/PTR_mini_hardware
Welcome to the KPPTR-hardware repository! This repository contains the design files for the hardware components used in the KPPTR project.
140 parts1MIT - 4 layers30 × 28 mm
Rebot ctrl
Matheus3007/pcb-lab
PCBs designed entirely as code: Python circuits + KiCad 10 + Freerouting, checked, rendered and ordered assembled from JLCPCB
58 partsMIT - 4 layers26 × 56 mm
PTR micro pcb
PTR-projects/PTR_micro_hardware
Welcome to the KPPTR-hardware repository! This repository contains the design files for the hardware components used in the KPPTR project.
115 partsMIT - 4 layers48.9 × 52.1 mm
Waterloo rocketry canhw processor
punkfab/pcb-corpus
235 real KiCad boards from open-source hardware repositories, prepared as a placement and routing benchmark
80 parts1 - 2 layers60 × 30 mm
Controller
google/mozc-devices
Circuit diagrams and firmware source code for Gboard DIY keyboards
11 parts3kApache-2.0 - 2 layers103 × 30.5 mm
- 2 layers26 × 30 mm
Expansion Card
FrameworkComputer/ExpansionCards
Reference designs and documentation to create Expansion Cards for the Framework Laptop
11 parts1.1kCC-BY-4.0
Questions
How big is the Lsm6dsv32x breakout PCB?
It measures 20.3 × 10.2 mm and has 2 copper layers, 1.6 mm thick.
What parts does the Lsm6dsv32x breakout use?
11 parts, built around the LSM6DSV32X. 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 Lsm6dsv32x breakout KiCad files?
From the godmar/imuboard-claude repository on GitHub, at the commit this page was made from: the board is lsm6dsv32x_breakout.kicad_pcb and its schematic lsm6dsv32x_breakout.kicad_sch. PCBKit opens the board in the browser, with nothing to install.
Can I use the Lsm6dsv32x breakout design in my own project?
Its repository states no licence, so its author keeps all rights: ask godmar before reusing the design.