sparkfun / lilypad_protosnap_plus Goto Github PK

Re-name nets that have no connection to match pin mux matrix (also, include pin mux matrix in docs)

(1) 32u4 package used is not currently in the Sparkfun-Libraries (don't forget prod-ID)

(2) RGB LED package used is not currently in the Sparkfun-Libraries

NOTE: I see that the packages live in the "newlilypadparts" lbr in the hardware folder, but I'm not sure when the parts actually get added to the official SFE libraries. If the parts normally get merged to the outward facing Eagle libraries after this point than ignore (1) and (2).

(3) the Buzzer GND signal in the schematic does not use a GND symbol

(4) BOM and design discrepancies:

• Sparkle page needs product name changed to match new name
• 32u4 needs prod-ID
• one 10K needs to be subtracted from the Sparkle BOM
• one 1K needs to be added to the Sparkle BOM

(5) Should the bottom left of the board be on (0, 0) to avoid issues with non-pay Eagle use? (i guess not really a thing anymore)

(6) Is it worth getting rid of some of the orphans in the design? It just looks kind of funny in parts (non necessary fix)

(7) the D2 trace has an unnecessary right angle. I missed this on v01

(8) Do the traces on the Buzzer need to be at an angle not divisible by 45? (non necessary fix)

(9) I don't think we will ever need fiducials on the bottom of this design, but because it's on the design checklist if figured I would include it. (non necessary fix)

This reads ~7 but is analog, should read ~A7

(1) Sink 1 and Sink 2 nets do not have FLAG label (this looks intentional, but thought it was worth mentioning)

(2) Because this design has changed so drastically from the original 328 based lilypad dev. board, I think it seems more appropriate to call this v01

(3) BOM ISSUES: Remove 1 CAP-12416, Add 1 CAP-12417

(4) 32u4 currently named U$5, should be U5

(5) RGB LED currently named U$6, should have diode naming convention

(6) Routing, sizing, labeling, and spacing issues/ideas:

----The 3.3V trace above R3 goes from 12 mil to 10 mil, not sure if this is intentional.

----D2 trace below R7 on the bottom has a 90 degree angle, the 3.3V trace that goes to a via by the 3.3V pedal isn't used (no bSTOP on via) thus is unnecessary.

---- D+ and D- traces could be straightened out a bit (may help with signal integrity)

---- R3 could be scooted to the right so that the 3.3V trace enters and exits the R3 pad but can be straight, this would also allow for the same on the "RESET trace, you could then scoot the "RESET" label over to be centered with the button.

---- There are quite a few instances of traces entering pads at angles, some are necessary due to spacing limitations, and some seem to be unnecessary. I don't see any instances that are terminal to building or function, but I thought it was worth mentioning as it is a point in the design checklit.

----"CHG" label could be scooted to the left to be centered with the LED

(7) 32u4 FP and tCREAM: The 32u4 FP in this design is different from the FP on the currently live 32u4 boards. The FP on the live boards omits the center pad entirely, reduces the tCREAM apertures on the outer pads to 75% of the pad size, and has pads that have a rounded inner side that matches that of the pads on the 32u4 chip. The FP on the live designs yields low amounts of rework assuming accurate PnP placement.

QUESTIONS:

(1) What is the "4" silk under the white LEDs referencing?

(2) Was it intentional to leave the SF flame off of all the boards? As it stands, the only SF logo is on the frame

Move away from trace, expand bridge slightly