Take a look at this footprint. We’re looking at the solder-side of a DB-25 connector footprint. Given all the SMT and HDI (high density interconnect) we see these days, this looks primitive; like it could be straight out of 1979 or something. But it is a recent PCB design. Some of those good old-standard parts still have a place in today’s world.
However, old or new, issues can still pop up. So, just what do you see wrong with this one? At least two issues are pretty obvious, and a third may be open to debate.
What’s wrong with this picture?
soldermask on pads
annular ring too small
traces too close which could cause exposed copper if we open up the soldermask
I’d love to see the traces buried in the board, but this is most likely a ‘quickie’ 2 or 4 layer board that doesn’t allow it.
1) uncovered via in the pattern is of concern.
I don’t see much else since our “selective solder” machine places these and solders them VERY effectively. I don’t care if traces are close to the pads, since my manufacture is VERY effective with soldermask coverage, and solder doesn’t wick to the traces.
I’m more concerned that my assembly drawing shows the correct side of the board for the connector mounting, and that my Pin 1 is in its proper place.
Been here, done this…
1. It looks like the soldermask is covering the pads.
2. I don’t see a square pad to denote which pin is pin 1.
Not sure on the third, but not sure why there is a via in the middle of the part.
more than three?
1) Soldermask on/covering pads.
2) needless traces too closely offset toward other pads.
3) teardropping always helps reliability with pads interfacing smaller traces, especially on external connectors.
4) is the via really needed between pads of the connector? I bet not, it could have been elsewhere.
5) no pin one indication, square pad.
Brad hit all the issues. Great job!
1. The solder mask is supposed to be 2 or 3 mils larger than the pad and definitely not cover the pad. There are no solder joints. This is a CAD library padstack construction error. After plugging and unplugging the mating connector a dozen times, this connector will come loose from the PCB.
2. The DRC trace to pad spacing rules seem to be smaller than the trace width. If the pad solder mask was swelled 3 mils it could have caused pad to trace solder bridging.
3. Avoid placing vias in-between rows of connector pins. The via is also directly under the connector and hopefully there are no metal parts in the connector that are near the via that will cause a short circuit.
4. I always use tear-drops on my through-hole trace to pad entries, especially connectors. Notice the drill hole in the via is offset toward the trace. A tear-drop would have reinforced the connection.
5. No Pin 1 marking. Normally Pin 1 is square on connectors to make it easy to identify in case there’s a problem. Also, all through-hole parts that have a danger of insertion inversion normally have a square Pin 1.
Any PCB fabrication shop with a front end CAM system would have caught all of these issues, but the PCB designer should have also been aware. Looks like these issues slipped by several people in the process.
Things look pretty well discussed above but may I add.
Some of the plane clearances around the pins have left gaps in the reference return for the signals: SI problem.
It is not easy to see that the pins are protruding far enough through the board so that 45° filets are produced. I don’t like what looks to be indents in the right side for the solder around the pins. Holes may be too big.
If those little white dots are solder balls, there are a couple located in the narrow clearances between traces and pads. I can’t see a lot of detail but there looks to be balls on soldered pads. No nitrogen environment, poor soldering temperature profile, out gassing, any of which may help with the pin soldering.
In our industry that connector would have to have mechanical support. It could not rely on the soldering of the pins.