SparkFun Forums

[n1ist]

A few quick notes...

Schematic:

- Missing bypass caps on processor (one on Avcc. one or two on Vcc, placed right next to the chip)
- Recommend standard pinout on ISP header
- Recommend adding ground to headers that don't have it
- Add headers for other I/O? ADC6 and ADC7 are only ADC, not GPIO
- Stylistic - it's better not to have 4-way junctions on a schematic; makes it easy to miss one where the traces should connect but don't or vice versa. Better to do two 3-way junctions instead

PCB:
- Footprint for USB connector should have the outer mounting pads extending past the left and right edge of the connector and should have vias tying the pads to the board for mechanical strength. Too easy to rip the connector off the board without them. Same for the LIPO connector.
- There's very little clearance between the LIPO connector ahd the 4-pin header; will you be able to get the plug in? Does the plug fit flush to the board? Mught be better to rotate the connector 90 degrees clockwise.
- Check clearance betwen trace connecting C2 and C3; looks like it comes very close to the other pad of the caps
- Is the resonator footprint on the right side of the board? It's blue on the topside picture, and shows up on the bottom side, shorting to the trace from R7 to D1
- PWR and VCC traces look quite thin. Should be wide for lower impedance.
- Any restrictions about via, pour, or traces beneath the radio? At least tent the vias on the bottom side so as not to short out to vias or pads on the bottom of the radio PCB

/mike

[mattmunee]

Mike,
Thank you so much for the detailed response. This was the type of feedback I was hoping to receive. It will take a little while for me to digest and implement your suggestions, but I'll post a revised design ASAP!

[davep238]

-Addtional notes-
Schematic:
- You have several pins that have a net associated with them, but don't connect to anything. (i.e. D4). This shows up as an ERC error: "Only one pin on net D4".
- Fix your ERC errors, or at least, approve them.
- ADC6 & 7 are inputs, but aren't connected to anything. Should they be grounded, pulled up, pulled down, etc? This also generates an ERC error.
- some of the text (i.e. "SPI programming Pins") runs into other text or parts.
Board:
- you have tStop errors for the "IO" connector because the silk screen overlaps the stop mask. The only way to fix this is to fix the library part. While in the schematic editor, run the ULP "exp-lbrs". This will produce libraries that only contain parts that are used on your design. Once the library is fixed, in the board editor, click on Library->Update (choosing the newly created libraries).
- I don't see the point of silk "D9" that's below the "ARD" LED. There isn't a D9 in the schematic.
- You don't always need to connect to SMD parts at the corner of pads. For example, if you make a straight trace run between R4 and the "ARD" LED, then the ground plane would flow between U2/"CHRG" and R4/ARD"
- traces should not come out of connector pads at an angle. A trace should only come out of the long end of the pad, or out of the side of the pad. Angled traces would be OK if the pads were round, instead of oval.
- the silk for U3 has unneeded lines near pins 10, 20, & 30. Fix this in the library.
- the antenna pad should be labeled with silk (i.e. ANT)
- the radio's VDD pad is so close to pin 1 of the IO connector that it would be easy to short out.
- the "-" symbol for the LIP connector overlaps a pad of C8. Move C8. C8 may be in the way of the connector or the cable from the battery.
- I don't see an outline for U1, so I don't know if there is enough space between U1 and other parts.
- The "CHG" and "B+" silk is too close together.
BTW
- contrary to another poster, I see that the resonator is on the top layer and is not interfering with any other part.
- I find it helpful to print out the board actual size and then lay parts on the paper to see if everything fits right.

[mattmunee]

Thanks for all the help, everyone. I implemented *most* of the suggestions, and I just ordered parts and boards, so I'll give it a go soon. One pressing question that I have from this is concerning the "45-degree rule". Is that still a hard-and-fast rule these days? Also, on a related note, that is why I tried to come off the pads at the corners, to eliminate all the 90-degree copper intersections. How is a 90-degree bend in a trace different from a 90-degree trace/pad intersection? Isn't there still potential for acid traps? Anyone have a solid reference for good practices for PCB design (with explanations)?

[davep238]

The concern that 90 degree bends and 90 degree junctions caused acid traps may have been true in the old days, but they are no longer a concern. Go ahead and use them.