The coating you put over the circuit pattern that leaves the metal exposed where you want to join components to the board is another make-or-break aspect of PCB design. While the geometry of the packages continues to shrink, the laws of physics do not change. Molten solder will still find a way to migrate. Capillary action will pull it down a via until the solder joint is starved leaving an insufficient solder joint. A narrow enough gap is easy to bridge with just a little vibration from the conveyor system at the right moment. A thin sliver of mask will fail to adhere where it's intended.
Image Source: Wikimedia Commons
...The Laws of Physics Do Not Change
Back in the day, I ran a Receiving Inspection lab, and when a new lot of boards came in, we had to run several tests. We had an expensive machine that could measure the gold thickness of the connector fingers. It was based on some sort of radioactive isotope so it had to be calibrated every other week to keep up with the half-life of the material inside the box. Another machine had a pair of probes in a pincer orientation with their pointed tips facing each other. The PCB was placed between the pincers and aligned over a via. It would clamp down on the hole and could electrically measure the copper thickness of the via wall. Science! Back then, nobody tented the vias. Not sure how they measure the copper thickness nowadays.
So, what sort of high tech gizmo was used to determine the adhesion of the mask to the board? A pressure-sensitive adhesive elastomer–otherwise known as Scotch tape–was stuck to the board and then ripped away. Check the tape under good lighting and magnification for any signs of green mask, white ink or copper colored copper. That's called the tape-test. A solder mask sliver that is less than 100 microns in width stands a decent chance of failure.
There were some other instruments in the lab; the Mitutoyo pin and feeler gauge sets in the beautiful teak wood boxes, and the optical comparator that could pass for a Sci-Fi prop were among my favorites. There was a big granite block that was really, really flat and a light table that was quite light. Add in a microscope and a bevy of measuring tools along with mylar 1:1 artwork for each board to round out the non-destructive testing. With all of that going on, the number one reason to generate a discrepancy report was the tape test. So, make sure you're leaving enough mask behind to stick where it's needed.
Hobbyists can buy little ketchup bottles of soldermask to squirt on as a full board solution or in the form of a pen for touch-up jobs. Either way, it's smelly and messy. This is the same stuff the pros use, but they screen it on in a process called LPI for Liquid Photo Imaging. Dry film is a more advanced process where you start with a sheet of mask and a printed image of your desired solder openings. After the same curing and developing steps, you end up with professional-looking results. On the extreme end, there is LDI or Laser Direct Imaging which cuts out the organic steps and alignment variation producing an amazingly accurate deposition. Each of these is an order of magnitude more expensive than the one before.
LDI technology can also be used to ablate mask that should not have been applied in the first place. This type of rework can save a board from the waste pile. The result is as fantastic as if it was meant to be, and definitely a step up from trying to remove it with an Exacto-knife. Micron Laser Technology has an excellent slideshow that gives you some idea of the power of organized and energized photons.
I interviewed dozens of candidates for CAD PCB Designer while at Google. One of the first questions I would ask was, “describe the pad-stack that would be used for a 0.4 mm pitch BGA.” If you take the 100 microns away from the solder dam, that leaves an opening diameter of 0.3 mm so that should be the maximum solder mask opening. IPC also recommends 100 microns of expansion from the metal layer so that would put the maximum pad size at 200 microns or 0.2 mm. You'd like a little more than that for the via in pad, so this is where the current IPC values break down.
After consulting with COMPEQ out of Taiwan, Ibiden of Japan and a few other top-tier outfits, we compromised by enlarging the mask by 75 microns instead of 100. so the final numbers are a 225 micron pad with a 300 micron opening in the mask.
A fair number of candidates went for a soldermask defined land for this geometry where the numbers were more-or-less reversed. A larger metal pad that is mask defined allows some extra wiggle room for the u-via-in-pad can open up the fan-out which can be critical on these tight packages. The wider solder mask dam doesn't hurt when some punk-rock receiving inspector goes at it with the tape; just sayin'. So that was an acceptable answer as well and currently the only way to approach pitches below 0.4 mm.
The next part of the discussion will be about the advantages and disadvantages of Solder Mask Defined (SMD) and Non-Solder-Mask Defined (NSMD) lands. That was the follow-up question to the first. The questions have a two-fold purpose. One, to test the candidates' knowledge (obviously) and two, so I could find out what the other engineers were doing with these fine-pitch devices that become more common every day. There was something in it for me then, and now, there’s something in it for you, too.
About the Author
John Burkhert Jr is a career PCB Designer experienced in Military, Telecom, Consumer Hardware and lately, the Automotive industry. Originally, an RF specialist -- compelled to flip the bit now and then to fill the need for high-speed digital design. John enjoys playing bass and racing bikes when he's not writing about or performing PCB layout. You can find John on LinkedIn.More Content by John Burkhert