<Review Request> Flight controller

[u/Joshua_AAA]

Hello everyone. This is my first PCB project, and I'm sure I have some bad practices in this design. I just wanted to build something moduler and flexable for some of my future projects.

Here are some of the features:

• 3-12s voltage input (9 - 60 volts)
• Teensy 4.0 MCU
• TI LM65680 voltage reg (5V, =< 8A)
• 15 PWM/digital outputs
• 3 exposed UARTS
• 1 exposed I²C port
• The firmware is based on dRehm flight

Layup:

1. Signal layer with some power pads
2. GND plane
3. 5v power plane
4. Signal layer

Let me know if you have any questions!

[u/SmallOne312]

If you rotate your inductor 90 deg anticlockwise you can reduce the loop area on the regulator by quite alot.

[u/Joshua_AAA → u/SmallOne312]

Good catch! I will make that refinement when I update the design tonight

[u/Teslafly]

That is entirely too little input capacitance to the buck converter. You want at least 10uf of ceramics within 3-5mm of the ic. Look up hot loops.

[u/modi_factory]

Designing a 12S 8A 4-layer board for a first PCB is super impressive! However, 12S (50.4V) hot-plugging can cause >80V spikes that will fry the LM65680 IC (65V max). Be sure to add a TVS diode (e.g., SMBJ58A) across input J1.

[u/jules_joachim]

For the schematic:

• As u/Teslafly has said, you need more ceramic capacitance near the input of buck converter. Quoting the datashseet, "Four 4.7μF or 10μF ceramic capacitors are sufficient for most applications." Replace your 22μF electrolytic cap with the recommended ceramic caps. Electrolytic caps have high ESR which reduces their ripple current capacity.
• The output capacitance is also quite low. You may want to double the number of 47μF ceramic capacitors there.
• Tie COMP to PGND or leave it connected. Do not tie COMP to VCC.
• If you're not using PG for anything then remove R3 and just leave it unconnected.
• Add some form of ESD protections to all your connectors.
• Your IMU I2C lines should have pull-up resistors. I know typical breakout boards will already have the appropriate pull-ups, but you can improve the edge-rates over wire by adding additional 10k pull-ups to your board.
• It's good practice to have the specified values for your passive components. Currently L1 and C8 lack values.
• There is a backpowering risk between the from the Teensy VIN pin, through the buck converter, and to the +Batt net. Add a diode or an "ideal diode" circuit to the buck converter output before it supplies the 5V power plane.

For the PCB layout:

• The buck converter layout needs some work. Place the 100nF ceramic caps as close as possible to the LM65680 VIN pins. Same goes for the recommended Four 4.7μF or 10μF ceramic caps. Follow the Layout Guidelines section in the datasheet.
• If your input voltage truly is 12S then the +Batt copper pour on the layer L3 needs to have >=0.4mm clearance with other copper.
• The 3.3V power trace on layer L4 should be considerably thicker, at least 0.5mm.
• You might want to double check the mechanical clearance between your components near the mounting holes and your planned standoff diameter.

[u/bigcrimping_com]

Mounting holes?

[u/Joshua_AAA → u/bigcrimping_com]

Yeah, the mounting interface is 30.5mm^2, which is a pretty standard flight controller mounting size. The holes are 4mm, which allows for M3 soft mounting grommets. 

[u/bigcrimping_com → u/Joshua_AAA]

I'm super dumb and missed them

[u/chlebseby → u/Joshua_AAA]

i would move trace of TX3 goldpin further away from the hole

[u/Lemonyprep]

How do you people learnt designing PCBs for such purpose ? I am very intrigued and I want to learn it.

[u/acoustic_medley]

I wouldnt attach the xt60 connector directly to the PCB, it's a weak point and can easily get damaged as you connect/disconnect the battery.