I’ve created a 4 layer PCB with a BMS IC (BQ76925) and a Buck IC (LMZM23601). My plan is to connect an 11.1V LiPo battery to the board, and then output a bucked down 3.3V and 11.1V from screw terminals (which will go to another board with an STM32). I also am outputting the analog and digital outputs from the BMS (I2C etc) to my STM board.
The 4 layers are - SIG, GND (called PACK- here), PWR (11.1V), SIG.
My biggest fear is that I haven’t isolated my digital and analog components enough.
This is also the first PCB I’ve ever made, so I’d love to get some feedback from the community.
This forum is primarily aimed at helping KiCad users with KiCad specific questions, there are other more general electronics forums that are better suited to this kind of question.
We generally let this kind of post run for a little while . . . but don’t be too surprised if it gets closed when you aren’t expecting it to.
Apart from the trace carrying my bucked down 3.3V, I kept the trace width as KiCad’s default (0.2mm) as I assumed from the BMS datasheet that the pins are fairly low current - would you recommend increasing the trace width anyway (if space allows)?
Also, are sense resistor traces essentially expected to accommodate the same amount of current as the actual battery output? The 11.1V from my battery is supposed to provide up to 10A (if all four of my motors stalled at once), so would this mean my trace between my Sense components should also handle 10A?
My standard for signal tracks is 0.25mm and for VCC is 1mm. Near ICs with 0.4mm pitch I use 0.2mm tracks but in small distance from IC I change them into 0.25mm.
I see - I made a mistake in my sense resistor connections. From the example layout in the datasheet, it looks like the sense resistor is connected to Battery- and Pack-;
I’ve connected the PACK- end of the sense resistor using the PACK- ground plane
For the Battery- end of the sense resistor, I calculated a minimum track width of 7.19mm to allow 10A of current.
High-current design isn’t trivial.
If you have 4 layers, use them all.
If you only have two layers, use both of them.
You also might need to specify thicker copper. I use 2oz copper in these cases.
You might be better served with a copper “zone”, instead of a fat trace. Also - make sure you calculate the power being dissipated in your sense resistors.
I see, I quickly put together a copper zone for Battery-. It’s on the top layer (which also has a bigger copper zone that’s Pack-)
If I were to instead move this Battery- zone to another layer (say the GND/Pack- layer), I’m assuming I’d have to connect the pads with Via’s, and thus find Via’s big enough to accommodate 10A?
I think you should double-up on the zone. Use both top and bottom layers to carry all that current. Add some stitching vias near the sense resistor to allow current to flow from the top layer to the bottom.
Changing thread to rope will be part of the answer!
As for track width, I like to make the tracks almost as wide as the pads to which they are connected unless there is not enough space. Unless you are at high voltage or maybe controlled impedance, there is generally no disadvantage to wide tracks. They have slightly less stray inductance and they are more mechanically rugged.
This is a view of a recent 2 layer board which I designed.
Tracks for terminal blocks and connector should be on the BOTTOM layer, unless the connectors are surface mountable. You can not solder a pad if it is UNDERNEATH a connector. That is unless you are using plated through holes under the connectors.
I’ve realized I made a big mistake - the ground for this circuit should’ve been BAT-, not PACK-. So I’ve updated the schematic and layout to reflect this. And instead of a smaller, special zone for BAT-, I’m doing that for PACK- (and the sense resistors that are still connected to PACK-).
Additionally, I made the traces thicker (0.4mm) to match the pads, as I have ample room.
Apologies for my naivety, but aren’t the terminal block/connector pads plated through holes (ie can be connected through any layer)? I assumed it’d be like any other THT component
yes they are plated, so it will work.
However it still a good idea to connect them from the bottom layer. In case your footprint is wrong (wrong hole size) you can increase the hole size (so you loose the plating), but the boar can still work
