Rocket power board

[Pdada1]

No description provided.

[StarlightDescender]

Assuming this is good to review despite the PR still being marked as a draft?

1. There's a lot of stuff on the root page, and the subsheets are basically empty. I think you could have your buck, battery charge circuitry, and current sensing on the same sheet? In general there's some messy stuff that would benefit from being tidied up, both for aesthetics but also readability.
2. You should note the fuse current, and on that note I think 6.3A is too high? my napkin calculation says that 4A is sufficient - 2A max through the gecko on both the 5V and 12V lines, and the battery current draw due to the 5V is at most (2A * (5V/12V) * 1/e) = 0.92A (assuming an efficiency of 90%).
3. On the 5V enable, I'm not sure why you're using the Drain-Source voltage to size R14/15? Should you not be using the Gate-Source Threshold voltage to calculate the divider such that V(HIGH) across the divider gives a voltage just above VGSth?
4. Your P-MOSFET has an insufficient Continuous Body Diode Forward Current (1.5A) - from the buck and the gecko we can output up to 2A, is there a reason we're limiting it here?
5. Is there a reason you don't have a low-pass RC filter on the INA2180? You should also make a note of the gain of the INA.
6. Rather than add a solder jumper to the CAN termination resistor, you could mark it as DNP and only add it if you do actually need it.

[ManavToor]

Please organize your schematic better, it is very difficult to read.

[StarlightDescender]

1. Sorry I wasn't clear, I meant that you should put a differential low pass filter on the inputs to the INA.
   nvm im trolling, yes the low pass filter should be right at the ADC pin
2. How did you size the fuse? What math/current draw/data has been referenced?
3. Current sense resistors not sized still?
4. Some of your footprint links are broken - There's a footprint from tutorial board, as well as several from other projects and some from folders in your downloads folder. These should all be in the project specific footprint library, and should be referenced with a relative filepath, rather than an absolute filepath.

[StarlightDescender]

Still some weird schematic stuff - ex. lipo voltage from power subsheet goes to VCC on main sheet which only connects to 12V sense in on power subsheet?

1. Why is R8 so small? if 2A max this gives you a V range from 0 to 2V - try to use most of the voltage range (for the PIC, 0-5V)
2. I was thinking about this more - we also want current sense for the 12V rail to rocket, and battery charging current
3. Not sure how I missed this one, but the buck converter wants 3 1uF input capacitors.
   

Layout:
4. C13 and 14 are getting kind of far from the 12V input - probably best to do a 2x2 array of capacitors, if that makes sense?
5. You can move R1 and R2 closer to the buck
If you haven't already, read 9.4 of the buck datasheet, and also AN-1149

[StarlightDescender]

1. No datasheet for U7 ;-;

2. Either source a 455R resistor or adjust your value slightly - I just looked and 455R isnt a value that can be found easily. Also, this is for exactly 2A, which is the same current draw that would kill the buck - maybe set it for 1.9A or even 1.8A? Something like 475R exists and gives a shutdown current of 1.9A

3. You're not using the error output of the efuse?

4. Excellent google sheet, only concern is your estimate of input capacitance? From what I'm understanding, you're saying camera board capacitance is 22uF, estimating all of the boards in total as 3 camera boards worth of capacitance, and then putting a FOS on that? Can you elaborate a bit more on that one?

Layout:
5. Overall nice work on the buck layout/routing, there's a few daisychained traces (R1/R2, for example) and a few things I'd question (is there a reason you're running the GND pad from R2 all the way to the GND fill of C13? Is it necessary to split the GND planes?) but very good work!

[Tessa-P]

• no pdf in folder :(

• programming connector has wires running inconsistent lengths under label (this doesn't matter)

• FLT should have overline
  

• Note calls out R2 but resistor has since been renamed
  

• add datasheet for can transciever (i hate google)

• Your source impedence on your battery voltage sense line is too high, datasheet says max 10kR
  
  

• fill out title block and put it in your portfolio 👀

In general looks good :)

[StarlightDescender]

Overall looks decent! A few notes before routing:

1. Theres a bunch of stuff that's pretty cramped? I'm looking at the F.silkscreen layer and there's a lot of overlap, partially because stuff is just so close together. Also there's a lot of parts that are slightly offset from each other, which doesnt look very nice.
2. The GND pour for the oscillator should be separated from the general GND pour on both sides, except for one trace.
3. A few things that look like they'll be interesting to route - the far side of the e-fuse (the side farther from the MCU)
4. When you get to it, connectors should line up with the board edge, and the mounting holes should be square

Resolved

[StarlightDescender]

1. Fix DRC
   
2. Take a look at fig 2-3 (pg 15) of the datasheet for oscillator layout - you should copy this layout.
3. center-to-center distance between the mounting holes should be some multiple of 0.5in, also rounded pcb corners please
4. Connectors (screw terminal and gecko connector) should be right on the board edge
5. in general you have some parts that are almost aligned but not quite? the board looks nicer if you can align components so they're all facing the same way (and so silkscreens are also all in one direction)
6. How did you calculate the spacing for the via fence on the oscillator?

[StarlightDescender]

1. totally missed this, please revert your changes to both RA and charging on the pad, and also tidy up the symbols/footprints (delete stuff you arent using - ex. don't need the L and M SOT-23-THIN footprints)
2. Is there a reason you have CAN TX and RX on non-adjacent pins?
3. Lots of places where you have components really smushed together - this wont be very fun to solder. You have lots of space in other places, maybe there's a way to take advantage of that?
   
   
   
4. Why run the CAN traces through two vias each?
   
5. There's some silkscreens that will get covered by components - L1, U4, and a few others.
6. we cant have parts with thermal pads on both sides? currently we reflow one side, and then we try to reflow the other and then the first side melts and falls off which isnt great
7. thermal pads should probably get thicccc traces so they can effectively dissipate heat. Something like 0.05in or so

[Joe-Joe-Joe-Joe]

Spreadsheet is good. I wish every board designer did this
Schematic:
5V

1. Does FLT need an external pullup? Can the PIC internal GPIO pullup source enough current? This is the only reference I could find and it says "no"
   
   
2. schematic note for what this does?
   
3. This is kind of really broad but have you considered transient protection/reverse polarity protection? Most importantly is downstream, we don't want to reverse-voltage the 5V bus
   
   main
4. There is a builtin function for DNPs that makes it more obvious
   
   12V
5. Pullup for FLT - as above, schematic note for OVCSEL - as above
6. Why do you use 0.01uF for Cin if datasheet recommends 0.1uF?
7. Your schottky diode for the charge line is rated to 1A average fwd current. But your fuse is 5A to the battery (also consider that when charging you are also powering the entire bus. So the minimum current over the diode is (battery max charge current + 5V buck max input draw + 12V (2A since RILM is 475))
8. Why is F1 a chip fuse instead of a replaceable clip fuse (I think there is a standard littlefuse holder we use elsewhere?)
9. L1 is 42mR typ but Webench calls for 19mR
   

PCB:

1. Building on the charge current concerns above - are you exceeding the max current on a single gecko pin for the charge line?
   
2. standard hole spacing I believe is in increments of 0.5"
   
3. Dangling trace
   
4. I'm not going to check all your power trace sizes. But note that your cross-sectional area across this pour where it constricts is less than the width of the actual trace into the pin. You can almost certainly eke out a bit more space on the top-right of the gecko mounting hole
   
5. Bend osc traces in a "Y" shape rather than 90 deg
   
6. As Ash mentioned, try to spread components more evenly
7. Your edge cut is not straight
   
8. Minor nit, rn your buck gnd plane goes through your pad. you can move C12 and R2 to give yourself a larger path
   
9. You can move this to the side to match and not overlap ss
   
10. Can move C13 upward to bridge pours directly, then add more GND vias below
    
11. Nit silkscreen labels should be oriented the same way and not overlap vias
    

thats enough for now