-

[realbarisbasturk]

-

[thm_w]

Looks OK to me. You could add mounting holes, test points, LEDs, if wanted.

This could easily be done on a 2 layer board, but 4 layer works too.

[Jerrery]

Cool to see KiCad design - I ever been using it too. Suggest adding a TVS diode (e.g. SMAJ5.0A) at power input for ESD protection. Also the 3D shows tight connector spacing - might cause soldering issues, maybe adjust slightly~

[mariush]

It would be easier to  rotate the chips ....

rotate U1 counter-clockwise 90 degrees, and take the trace going to CS_BME, put a via between the chip and C1 (now on the left side), on the back side come down with the trace and use another via to bring the trace back on top and route it to the right to the pin header.

Same deal on the right, rotate clockwise 90 degrees this time, and do the same with that trace.

Consider leaving an empty pin (as key) to the left of MISO and duplicating  the CS_INT and CS_BMI and CS_BME to the right of  miso, mosi , clock   ... that would allow someone to use a 2 x 5 ribbon cable to connect the board to some other board

miso mosi clock   GND    3.3v
INT   BMi  BME   NC/GND NC/3.3v

The empty pin will allow you to insert a 2x5 plug without issues... if you leave a pin there you would not have the versatility, you'd have to desolder the single row header and swap with another double row header.

[PGPG]

For connector pads 1,2,3,4 you don't need your tracks + vias as they are automatically connected to right zones.
I think there is a way to force pad 1 getting thermal relief connection at 45°, but don't remember how to do it.

Clearances at zones around vias seems for me too big.
When I add zone I set 3 of parameters (don't remember names, don't have KiCad here) to 0.25 and one to 0.2.

[PGPG]

I thought adding multiple vias would help, I know they are not really necessary. If you suggest it actually hinders more than helps, I'll remove it.

I just wanted to tell that they are not necessary.
If you have several zones with the same net than adding some (many) vias to connect them together is rationale, but if each your zone is different net than it have no sense.
Your viases near these connector pads give really nothing. You can think of THT connector pad as of a via but much stronger than other vias because of big hole diameter and being filled with tin.

I used the default (whatever KiCad provides) but will look into it too before I finalize the PCB.

Default KiCad settings are very conservative hare. I may be using such parameters in 80s.
Whenever I add zone I change parameters to:
Clearance, Thermal relief gap and Theremal spoke with to 0.25mm and Minimum width to 0.2mm.
These are not very demanding parameters - I would used them also 20 years ago.

[PGPG]

One more think - how many layers your PCB have.
It looks that there are at least two zones (3V3 and GND) and they are not at top so probably 4 layers.

I use 2 layer PCBs until I don't have to use more layers.
Here is the example of my 2 layer PCB:
https://forum.kicad.info/t/approaching-pcb-track-routing-for-a-newbie/36302/8

I used top layer for supply and signal and whole bottom as GND.
I used there three 0Rs to jump with VCC over signal tracks without breaking GND continuity.
Top free space is also GND - all vias you see are GND.

[JOSDHO]

Nice job for a first PCB — the layout looks clean and organized. For a sensor breakout board like this, you might want to add a few extra test pads on the I²C lines and power rails so you can easily hook up a scope probe during debugging. It’s also handy to leave a couple of unpopulated resistor pads or jumpers in series with the signal lines, so you can insert pull-ups or current-limiting resistors later without having to cut traces.

If this board will be in an enclosure, think about adding mounting holes early — it saves a lot of headache later. Otherwise, your current 4-layer stackup is fine, but you could even simplify to 2-layer if cost is a concern since signal integrity here isn’t very demanding.

Looks like a solid starting point, good luck with the rest of your project!

[thm_w]

The diode is upside down.

Ferrite looks ok but I would put something larger than 100nF, maybe 1uF or 10uF, should be available in the same footprint.

[SYOM]

Great job on the PCB design! It’s great that you’re taking the modular approach and using an Arduino Portenta H7 for prototyping.

A few things to consider:

Power and Ground Planes: Make sure you’ve added solid power and ground planes to minimize noise and voltage drops, especially since you're connecting it to other sensors and components. In KiCad, you can use zones to define these.

Decoupling Capacitors: I noticed you might not have added decoupling capacitors for each power pin of the ICs. Adding 0.1 µF and 10 µF capacitors close to the power pins will help with filtering noise and voltage spikes.

TVS Diodes: I see you’re adding a TVS diode for ESD protection, which is excellent! Make sure the TVS diode’s clamping voltage is well within the voltage rating of your components to avoid any damage. The placement should also be close to the input pins to be effective.

The addition of a ferrite bead is also great for filtering high-frequency noise, but keep in mind it will add some resistance, so ensure it's in an area where it won’t impact power delivery significantly.

Looking forward to seeing the final version once you’ve implemented the feedback!