This page is meant to provide a list of things that should be checked when reviewing the schematic for a PCB. It is the designer’s responsibility to check for ALL of the things below themselves, then assign others to review their schematic.

Part Reviews

Schematic Sheet Reviews

Microcontroller.SchDoc (@Logan Hartford)

• Personally, I am not a fan of using nets like this

I think it is always more clear when you make connections with a wire rather than just a net. Using too many nets like this is usually an indication that the schematic symbol hasn’t been customized for this application. If it were me, I would move the pins around on the symbol such that it would be possible to neatly make wire connections for all of the connections in the schematic.

• Most of you’re ports don’t have I/O type selected, set each one to input/output/I/O as determined by the design

• I see 6 power input pins on the microcontroller and 11 decoupling caps. I assume one of those if for the 3V3 on the debugging port. What the rest are used for is not immediately clear to me.

• Having the decoupling caps off the side like that is fine when where they are supposed to go is obvious, in the cases where it’s not obvious its best to put the caps next to the pins they are decoupling for clarity.

These are the decoupling caps for the whole BMS, I included one per component that draws power. Should I split it up by adding a decoupling cap section for each page?

• Like I said, it’s more clear when the caps are placed close to the pin which they are intended to decouple. This isn’t a major issue but I think doing it this way helps avoid errors. It makes it a lot more intuitive to check if the decoupling is good. The way it is now, I have to go to every sheet, count all the power pins and then return to this sheet and make sure they match. Rather than just checking to see if each power pin has an associated decoupling cap. Some people will debate whether or not you should do this so I would make your own decision.

BMSRev3.SchDoc (@Farris Matar)

Comments:

• You need a power connector (i.e. screw terminal) for VBAT power, currently VBAT doesn’t come from anywhere on your board

• Change the battery connector pinout to match that of the TATTU battery we are using (picture taken from datasheet). I believe the only discrepancy is you are missing the B12 connection, which should connect to the CV12 pin on the IC

  • The B- in this diagram would be Cell 0 in your schematic, which connects to GND correctly, just an FYI

• The MOSFET you chose requires a pretty high Vgs (5V min.), but with the signal from the STM32 you’ll only be able to achieve a Vgs of 3.3V. Select a different MOSFET, with a lower minimum Vgs

• You’ll also need to add the balancing part for the top cell (the FET connected to BA16 and resistor leading to CV15. Note that there’s no current limiting resistor on CV12). Refer to the example from the datasheet above, where CV16 would be CV12 in your schematic since we’re using a 12 cell battery

• EN needs to be driven high in order to enable the IC. Connect the other end of the switch to 3.3V

• “LDON” pin should be named “LDOIN”

• VA is the IC’s internal 5V LDO output, do not tie this pin to VBAT, it should instead be connected to a 5V power port and to a 1uF capacitor to GND. However, since your board doesn’t use 5V anywhere, you should connect it to LDOIN to disable the LDO

• VP requires a 0.1uF capacitor to GND, as mentioned in datasheet

• In your buzzer circuit, the buzzer is rated for a 30mA supply. Therefore, add a resistor between 3.3V and the buzzer to limit the current to 30mA or slightly less

BatteryBalancingRev3.SchDoc (@Rishith Bomman)

Appears fine to me, but I also don’t know too much about battery balancing

change Cell 12S to net instead of port

The balancing comes from sample schematic on MAX14921 datasheet (12 cell instead of 16).

Display.SchDoc (@Ari Wasch)

• change IC? to U for both displays.

• Also add a unique number for the IC, ex: U6 or U7. (tools → annotate → annotate schematic)

• annotate this as well:

• Change names of B_1, C_1, D_1, A_1 to something that makes more sense. change A_2, B_2, C_2, D_2 to A B C D

• Label where you got your resistor measurements from.

  • 3.3V-2.1V/20mA = 60ohms. not a big difference but where did you get 62?

Looking at availability on digikey, there are no 60Ohm. Some 60.4 but they are not the standard type of resistor so went up to 62 rather than down to 59.

Power.SchDoc (@Logan Hartford)

• This is pedantic, but I’d like to see the connections on L1 routed like how I have modified them on the left, vs how they are on the right.

• This is my personal preference, but I’m not a fan of routing power with wires in the schematic. Ports are cheap, use them. This is also a better reflection of how the power will look in layout since you don’t typically route GND.

• This is not a suitable use for a signal port, a power port should be used instead like the one you have to 3V3.

• The capacitor and inductor are not set up correctly.

  • For the capacitor, you want to display the voltage rating and the capacitance

  • For the inductor you should display the saturation current and inductance

  • ^ Still not done

  • We don’t care about displaying the part numbers for passive components

• Please include a link to the calculation you used to make the inductor and output capacitor selection

Webench:

• The example application schematic includes a Schottky diode going from GND to the left side of the inductor which is absent from your design. Where is the current return pathway when the regulator has disconnected the output from VBAT? I don’t think the regulator will function without the diode, let me know if I’m missing something.

CAN.SchDoc (@Wolfgang Windholtz (Deactivated) )

• CAN TRANSCEIVER IS OUT OF STOCK

  • Team wide problem. a new CAN transceiver needs to be speced

Generic Schematic Reviews

Net Naming (@Farris Matar)

Comments:

• Remove the AGND net name everywhere in your schematic, replace with a GND port when necessary. AGND is just connected to GND, and the AGND net name will just rename the GND net to AGND in your layout file, which might get confusing

  • As a general rule, never put net names on wires that connect to a power port

• Make VBAT a power port instead of a regular port

• Could use net names on the LED driver outputs

• “CS” port should be renamed to “CS_n” as it is active low

Wiring and Connections (@Wolfgang Windholtz (Deactivated) )

Comments:

• I made general comments in a doc. Some are repeats of others.

• Need to check pinout with Cubemx

https://docs.google.com/presentation/d/1j2JOP5_mvNR77QduVfKEUzUqP0qxYE0P82QO_lafwXU/edit?usp=sharing

Component Labels (@Logan Hartford )

Design-for-Test (@Ari Wasch )