That’s a quite bad example, with hardly any effort to
I mean, 4 long dogbones all jumping over the same track…
It’s obviously just quickly thrown together, but it will work, especially for hobby stuff and when EMC compliance is not such a big issue. There always is some compromise between speed and effort.
It’s just not a good example.
I’m seeing $8 US for 5 pieces, 100mm x 100mm board right now from our favorite low end provider.
Well, I halfway expected to get some beating for that. 
OK, rerouted power traces to the top, and have 4 short signal traces breaking the GND plane, and I separated the tracks.
Nice!
I’d probably move R1-R3 a bit further apart. Might be easier accessible with tweezers or for soldering. Not a big deal though.
I would be tempted to rotated J4 90deg anticlockwise , if possible.
D1 could move up and thus freeing some routing
It’s now in the area were there is not much more to improve.
Serpentine tracks may be slightly better then one wire hopping dogbones. Moving the resistors apart may make it a bit easier to fit your tweezers in between. Further benefits will be small.
And as Piotr already wrote, Half the advise given here is also not very important for a PCB as simple as this, but more in a general sense of:
From a manufacturing standpoint, running traces between through-hole connectors is best avoided.
Since those connectors will be wave-soldered, any mis-alignment in the solder mask runs the risk of solder-bridging.
But, 99% of the comments about this design fall into the category of “turd polishing.” At some point you just have to shoot the designer and go to production.
Meh, solder masks have not been misaligned that much for 40 years or so, unless you can find some really atrocious PCB manurefacturer. But both the pad size and soldermask have their own Gerber layers and a clearance between these can be set in the board setup.
Apart from this being a hobby project, and this PCB is not even fit for wave soldering because the THT connectors are mounted from both sides. Some of the youtube video’s about selective soldering look nice though.
Yeah, not only does rotating them save space, the traces are much easier to manage! Thanks for the suggestion.
And Piotr, I remembered I have an extra +3V3 at pin 17.
3Dogs, I’m a software developer. Polishing turds is part of my job description.
Thanks everyone for helping me with my first design.
Now that looks alot better
OK, then…
One more stylistic suggestion - don’t have traces leave SMT pads at anything but a 90° angle. And, try to leave from the center of the pad. There’s a reason (other than looks) why this should be done - SMT parts are pulled into the correct position by the surface tension of the molten solder. Having traces that are asymmetrical might be enough to pull the part out of position.
It’s called “tombstoning”, and indeed it’s a real thing. Asymmetry in the pad connections can result in a difference in which the pads reach the temperature at which the solder melts, and if the difference is too big, then the molten solder on one pad can pull an SMT part (mostly resistors and capacitors) upright.
Thanks everybody. I learned a lot from people with far more experience by reading every post in this thread.
And the suggestions keep flowing in! Thanks, that’ll be an easy one to fix.
I am really impressed at the quality and volume of the critique I’ve gotten in just two days. Thank you all for being so willing to share your experience!
Never heard of this one before (but then I don’t do high volume layouts myself). Can you elaborate a bit?
Traces are covered with solder mask, so the effect could only be uneven heating.
I would have expected tombstoning to be an effect of wrong pad/stencil geometry, one example here Perfect 0402 Footprint — Worthington Assembly Inc.
Not sure how relevant this is though:
If you are in the high volume (1M/year) business, assembly and layout people will know already and your company part library is tuned for high yield.
If you just make runs of 100 PCBAs, I’d say you have other more important issues.
Many of these rules are hold-overs from the early days of SMT manufacturing, but they are still worth following.
I have seen issues with LQFP parts where asymmetrical pads caused the part to be pulled out of alignment. But, these days, having the trace exit the pad in the center and at 90° is more of a style issue.
Putting vias right next to a small resistor or capacitor pad can cause solder starvation, though.
Still an issue with poor designs.
If one padis part of a zone (no thermal relief ) and the other has a single 8th track and IF the part was say an 0603, it’s almost guaranteed to tombstone during reflow
Eg
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
