-
Notifications
You must be signed in to change notification settings - Fork 2
New issue
Have a question about this project? Sign up for a free GitHub account to open an issue and contact its maintainers and the community.
By clicking “Sign up for GitHub”, you agree to our terms of service and privacy statement. We’ll occasionally send you account related emails.
Already on GitHub? Sign in to your account
Rocket power board #93
base: main
Are you sure you want to change the base?
Conversation
Assuming this is good to review despite the PR still being marked as a draft?
|
Please organize your schematic better, it is very difficult to read. |
There was a problem hiding this comment.
Choose a reason for hiding this comment
The reason will be displayed to describe this comment to others. Learn more.
- 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 - How did you size the fuse? What math/current draw/data has been referenced?
- Current sense resistors not sized still?
- 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.
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?
Layout: |
There was a problem hiding this comment.
Choose a reason for hiding this comment
The reason will be displayed to describe this comment to others. Learn more.
-
No datasheet for U7 ;-;
-
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
-
You're not using the error output of the efuse?
-
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!
d965894
to
e6e50b5
Compare
There was a problem hiding this comment.
Choose a reason for hiding this comment
The reason will be displayed to describe this comment to others. Learn more.
Overall looks decent! A few notes before routing:
- 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.
- The GND pour for the oscillator should be separated from the general GND pour on both sides, except for one trace.
- 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)
- When you get to it, connectors should line up with the board edge, and the mounting holes should be square
There was a problem hiding this comment.
Choose a reason for hiding this comment
The reason will be displayed to describe this comment to others. Learn more.
- Fix DRC
- Take a look at fig 2-3 (pg 15) of the datasheet for oscillator layout - you should copy this layout.
- center-to-center distance between the mounting holes should be some multiple of 0.5in, also rounded pcb corners please
- Connectors (screw terminal and gecko connector) should be right on the board edge
- 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)
- How did you calculate the spacing for the via fence on the oscillator?
There was a problem hiding this comment.
Choose a reason for hiding this comment
The reason will be displayed to describe this comment to others. Learn more.
- 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)
- Is there a reason you have CAN TX and RX on non-adjacent pins?
- 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?
- Why run the CAN traces through two vias each?
- There's some silkscreens that will get covered by components - L1, U4, and a few others.
- 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
- thermal pads should probably get thicccc traces so they can effectively dissipate heat. Something like 0.05in or so
No description provided.