Don't forget the decoupling cap near the SX1276.
Why choose a very flimsy 200mA regulator instead of a similarly sized, cheap-as-chips, copiously available but much more powerful AMS1117-3.3?
Common approach in microcontrollers is to pull them up internally in software. IDK if the FT232 offers this option. Anyway, I wouldn't worry about this. It's not a battery-run application so reducing current draw to the bare minimum isn't really necessary, and the floating FT232 pins likely won't do any harm otherwise.
They're just a text label; they don't actually do anything in the real world. But as said, there's not really a need to do anything with those floating pins. If your professor is being difficult about it for some weird reason nobody but him comprehends, throw in some 10k resistor arrays and use those to tie each unused pin to GND.
Not all changes are improvements, I'm afraid.
Place C4 close to one power pin, C5 close to another one, and C6 close to yet another one. Bunched together like you have them now it's not all that much different from just using a single, bigger capacitor.
I quite liked the fact that IN (USB) and OUT (antenna) connectors were on opposing sides of your board, earlier. Maybe you have a good reason for the current 90-degree arrangement.
Given how much space you have, the narrow spacings are kind of odd, but since pretty much anything is manufacturable these days, it's not necessarily a problem.
I'd space the test points a little wider; they're kind of inconvenient to access this way, especially if you want to monitor two adjacent ones at the same time.
Why use a very narrow track between the ferrite bead and your linear regulator? That's part of the greatest current path. Yet, it's a signal-width trace, for no particular reason. The USB data traces, on the other hand, are surprisingly heavy. Not wrong...just an odd choice.
In your place I'd make more effective use of the bottom layer. OK, you've got a nice, continuous ground plane now. But it'll still work well enough if you two nice, big supply lines (Vbus and 3.3V) across your board that you can tap into with vias. This leaves signal traces on the top side, which will then be even easier to route.
You have oodles of space on your board, and yet it looks cramped, doesn't it? That alone signals that there's room for improvement.
However...all the acidity aside, I'm sure it'll work in its current state, even if I'd do it differently. Decide how much you want to optimize, or at what point you're just going to send it out to get manufactured and then see how it goes. Usually with a new board, you have to go through one or two iterations before it does what you want, anyway.
oh, i get the capacitors placement now. Thank you for the feedback. I'm more on the programming side and didn't have any designing/layout course in my degree, so there are still a lot to be improved for my PCB layout skills
Ok, great to hear!
Like I said, the layout may not be the prettiest, but it'll get the job done most likely. At some point just decide to send it out and see how it goes. Then do some bug fixes and order a second board if needed.
