Content originally posted in LPCWare by Pacman on Sun Sep 22 14:02:13 MST 2013
Well.. I think it looks quite pretty and I like the size, but I do have some comments/suggestions.
I've only looked at the PNG pictures (I don't use Eagle).
[list=1]
[*] If this is made for hand-soldering, it's a very good idea to have the traces connect to the side of the pad which is far away from the component. If not doing this, you'll experience that pads just fall off as soon as you give the PCB too much heat or you do rework using a soldering iron.
[*] I don't like 90° turns. try eliminating as many of those as you can, so you get 45° turns.
[*] Adding a ground-plane doesn't cost extra, and it's more environment friendly (less etching acid needed, less copper down the drain). I know it's only a very, very small adapter, but it might reduce RF noise a little.
[*] Try making your traces head for the center of the pins/pads. (look at the 3V3 via in the middle/center and the GND pin in the top/center)
[*] I believe you could increase the trace width slightly; this might lower the PCB cost.
[*] Avoid 'pockets', especially when traces are thin. Pockets make it easier for acid to 'hide' under the soldermask and slowly ruining the PCB. (No, it's not very likely to happen ws the PCBs are usually washed quite well, but it's good layout practice).
[*] It's possible it'll be very, very difficult to read the silk screen. I tried zooming it to 'actual size' and as I believe that most manufacturers will have a 10 mil silk screen, you might just get a lot of white dots. 'ISP, Reset' and 'CLK' will most likely be readable, though. C1, C3, R1, R2 could easily have larger font size. Try keeping font-size 35 mil (0.9mm) or larger.
[*] Where did C2 go ? :)
[*] Try keeping traces as far from eachother as possible. (for instance, the two top/left traces on the bottom side does not need to get so close to eachother and GND gets very close to Rst. P00 gets very close to the corner of P14). I haven't checked all, so best bet is that you should try checking one pin at a time, going through all pins and traces. It may help to think of the signals as enemies that don't like eachother - keep them as far apart as you can. ;)
[*] Always start with a prototype run of low quantities.
[*] If your PCB is NSMD, pads tend to be torn off quite easily by a soldering iron. If it's SMD (Solder Mask Defined), the solder mask that overlaps the pad makes the pad stronger, thus it's more likely to stay on the PCB. I recommend SMD for hobbyists and breadboard adapters. NSMD should usually be used if you're working with BGA, but it's not always the case. Sometimes you might have to mix the two.
[/list]
Most important: Thicker traces, connect traces on the side of the pads facing away from the component.
Those are all just suggestions; I think the PCB would work as it is. :)