I recently had a PCB made overseas, just for a one-off prototype. I spent a few hours examining the boards so I thought I’d share my findings.
This is not a review, I do not intend to name the manufacturer, because this is a one-off examination; my results here could be different a second time around, or different to someone else using the same manufacturer. I chose a 4-layer board, and the results could be different for a 2-layer board using an alternate production line for instance, and so on. It wouldn't be fair to promote or criticize a PCB manufacturer by naming-and-shaming them on this sample of one single design.
This is merely a short blog post showing just some of the things that could be worth examining. It is up to users of PCB services to determine if the manufacturing tolerances are sufficient for a particular design or not. What follows is really not an exhaustive set of findings, just a few things of interest primarily examining the solder mask and the silkscreen quality (some things like vias were not examined beyond confirming that they do provide electrical contact).
From these results and previous experience a tentative summary would be that it is likely that if designs use large parts then virtually any low cost PCB manufacturer could be used. As designs get smaller then tolerances need to be tighter.
The solder mask is a (usually) green coloured layer on top of the copper although the examples here use a blue solder mask. Solder does not stick to this layer. Where there are copper pads, there is no solder mask; it is known as a solder mask opening.
Usually the aim is to have a solder mask opening slightly larger than the copper pad for components (it is known as a non-solder mask defined pad). An example is shown here of a non-solder mask defined pad. The copper layer is the conductor (it can be timed or covered with some other conductor; this example uses gold). The immediate area around it is the underlying board. The dark blue area is the solder mask. This design is unusual that the solder mask opening is so large, ordinarily it is much smaller (it happens to be a mark for optical recognition, not actually a pad for electrical reasons, but it nicely shows the solder mask so I used this photo). What should be noted is that often the solder mask layer is not exactly aligned with the copper layer. While this isn’t a problem for large features, it could cause issues for smaller pads as will be seen later.
The pad here is 1mm diameter (the small ticks on these photos are 0.1mm apart).
The photo below shows a more realistic pad arrangement; the two rectangular pads are for an 0402-sized surface mount resistor. The pads are 0.07x0.09mm in size and the mask opening is a further 0.1mm on each side. However because the solder mask layer is not perfectly aligned, the opening is greater on the bottom and right side of the pads, and does not extend beyond the copper pads on the top and left sides of each pad. It is a minor issue and should cause no difficulty when the parts are soldered to the board.
The photo below shows a more serious issue.
It can be seen that the solder mask layer has slipped so much that there are just very narrow slivers of it between the pads. The slivers are so narrow that they are actually broken up in places. The reason this could be a more serious issues is that the solder mask opening acts as a barrier during reflow. If the solder mask is so narrow that it has broken in some places, then there is a greater risk of short circuits when the board has had the solder paste and components applied and the board is heated and the solder melts. The soldered board will need a lot more inspection and possibly rework as a result. Perhaps a possible solution for a future board with the same manufacturer would be to try to reduce the solder mask opening by 0.05mm or so, in an effort to reduce the break-up of the narrow solder mask. It wouldn't help with the slippage of course.
The photo below shows a QFN package; the offset of the solder mask shouldn’t hopefully cause any problems.
For comparison, this is what it should have looked like according to the Gerber file:
Shaped holes (Milled)
For some components, a shaped hole is needed. The photo here shows such a hole; this was intended for a micro-USB connector. An oval shape was expected but it can be seen that the left side of the hole isn’t as straightly cut as the right side. I think this might be due to milling bit wander, because the other side of the PCB (the solder side of the PCB) had the hole looking slightly better than the photographed side (the component side of the PCB). Perhaps the hole is milled from the solder side of the board (this is just a guess).
However, the hole quality is not bad at all. It should cause no problem for the micro-USB connector.
This is what the EAGLE layout looked like for such a shaped hole:
The diagonal hatch and the circle in the middle of it is cosmetic, just for documentation purposes. The cyan shape defines the milled edge, and was drawn with a near-zero width (0.01mm). The overall red shape is a 'polygon' and the 'smd' pad is the tall rectangle to the right of the cyan shape. The other side of the board has a 'polygon' too.
The text and component markings were done in white on this PCB. The text shown here was done at a fairly small 32mil height setting in EAGLE with the ratio setting (which controls the thickness of the text) at 8%. It might look ugly at this zoom level but it is readable and doesn’t look so bad when looking at the PCB using the naked eye. I think text smaller than 32mil would have been difficult to read on this PCB though. 40mil and higher is very clear to read.
By appropriate sizing of solder mask openings and text sizes it is possible to get good results, acceptable for prototyping in many circumstances. As pads get smaller the slipped solder mask can become an issue. As pads get closer to each other very narrow solder mask can break up which could cause difficulties during soldering.
Text may need to be larger than 0.8mm height for legibility with some low cost PCB manufacturers.