Forums

Hi Anubhav! Hopefully someone will chime in here pretty quick. I'll ping discord.

Hi Anubhav,

I really like the design, very cool and I like the artwork. Looking at the design in tracespace I noticed you have component part numbers in the drill file, I'm not sure if this expected but I didn't on my design. Not sure if this will cause a problem or just get ignored. Another thing which again may be fine is the spacing between R4 - R12, might be a little tricky to hand solder, but someone with more experience hand soldering SMD components can probably comment.

You have way too many files in your gerbers, I think your board houses will confuse them, this is all you need:
F.Silks
F.Mask
F.Cu
B.Cu
B.Mask
B.Silks
Edge.Cuts which contains the board outline.
In1.Cu and In2.Cu are also needed for 4 layer designs.
NCDrill (1 or 2 files)
This guide explains it more:
https://docs.oshpark.com/design-tools/kicad/generating-kicad-gerbers/

Good looking board, just a couple of notes
J1 - if soldered it will make the pico not lay flat
LCD Screen silk has REF** in it, you can click edit and make sure the ref des isn't showing
FPC Connector - I hop you are good at soldering, that looks like a nightmare!, also your ground connections seem a little weird, the top and bottom ground are only connecting to the pour on one side (the right side has a sliver opening between them) and I'd remove the vertical trace, you have enough of a ground connection left and right and that will just add thermal mass
There's lots of places where you have a "T" connection on top of a via (like R27/R28, that is not recommended because a wandering drill can disconnect one side, better would be a "T" on the trace, you can also do the pad its going to but those can pull up with heat and force so if you are reworking you could break the connection, better to "T" on the trace
You might be able to get rid of some of your traces by making a power plane (3.3V or 5V) on your front copper
A couple of places you have your via pretty close to the pad, like SWDIO and GP6, if you have vias that are open (instead of tented) you could get solder thieving down them, I'd move them a little bit away so you have guaranteed solder mask coverage between the pin and the via
USB C - this is tricky to solder as well but do-able, I'd just triple check your pinout as you won't be able to program the Pico without that header or a modified cable because the clearance from your board to the Picos onboard USB

Very creative design! Love the QR code (I'm just glad it wasn't a link to https://rr.noordstar.me/mantakeeb-dc7df7fd).

Some things I noted:

• On the files, you included the Fab, Courtyard, Eco1, Eco2, and Drawing layers, which you don't need to do when you submit to the PCB manufacturer (usually).
• R4-R12 might be a little bit close to each other if you plan on hand soldering. If you haven't already, I'd suggest you print out a paper doll: https://discord.com/channels/897249680306618368/916892368534392852/919292113567481896
• The R19, R31, R33, R35, R37 silkscreen probably won't print (or will be partial) since there's a hole there...suggest you move the designator to a different location.
• C2 and the GP27 silkscreen are on top of each other. Just move C2 to the left side.
• R3 looks like there might be an extra paste pad. I don't think this would affect the manufacturing of the PCB, but would impact solder paste stencil if you were to have one of those made.
• Just want to confirm R23-R28 won't interfere with whatever you have there...I'm not sure what the outline is for.
• Is the cutout for a display? If so, are you using an FPC connector or soldering directly to the board? If you are using a connector, I ended up changing my connector from a Molex with 0.4mm leads to an Amphenol with 1.0mm leads to make it easier to solder. It's still going to be a challenge and I think I might use solder paste and a heatgun.