Solder mask expansion - Page 1
Forum section: electronics / general

author: ahbushnell
author_rank: Frequent Contributor
timestamp: May 22, 2019, 11:55:41 pm
content: What drives setting the solder mask expansion. What are recommended values?ThanksAndy

author: ajb
author_rank: Super Contributor
timestamp: May 23, 2019, 03:33:01 am
content: It's primarily driven by the mask to copper alignment accuracy. Actually, it's the accuracy of the solder mask edges relative to the copper, because you have to account for any expansion or retraction of the mask during the application process in addition to alignment error (offset/rotation). The important thing is that the solder mask should never be allowed to wind up on a pad, so your mask expansion should be at least equal to the maximum mask edge error that your fab can guarantee. Looking at OSH Park as a convenient example, theystatea mask accuracy of 3mil/0.762mm, so your expansion should be at least 3mil but preferably a bit more.The flip side of mask expansion is that if you set it too high you risk losing mask between adjacent pads. Your fab should also specify a minimum solder mask web/sliver, so if the spacing between adjacent pads is less than twice the mask expansion plus the minimum web, you won't get any solder mask between those pads. Using OSH Park again, their minimum web is 4mil, so with <3+3+4mil between pads the mask between will be eliminated. This may or may not be a problem, in my experience most assemblers don't seem to be bothered by not having mask between IC pads, because they should have their processes dialed in well enough that it's not an issue, but you can negotiate your pad and expansion dimensions a bit to maintain the web if that's important to you. Losing solder mask between pads on chip components, on the other hand, or really anything else, would be asking for trouble.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: May 23, 2019, 04:15:46 am
content: To extend that a bit further -- typically you want to do NSMD (non solder mask defined) pads. This is a pad of copper, with traces or spokes connecting to it, fully cleared by solder mask. A solder fillet forms between the outline of said blob, and the component pin. Some solder/fillet will wick up the traces/spokes.(Related topic: pad thermal relief balance. You don't want to have too many / too wide traces connecting to one pad, and not to the other, say of small chips (<0805). This is a tombstoning risk factor.)Sometimes, you have SMD (solder mask defined) pads. This usually arises when you are so hard-pressed for thermal or current handling, that you pour copper partly or entirely over the pad, and therefore the fillet forms up to the edge of the mask.Because the copper and mask have that 3 mil uncertainty between them, you definitely don't want to mix SMD/NSMD pads on a single part! Keep this in mind next time you're laying out a power device.Say you have a TSSOP regulator or MOSFET, with direct thermal pours -- this is a good place to use SMD pads.For the most part, even when power handling is key, spokes arefine. Run the numbers yourself! Take the thermal conductivity of copper, foil thickness, spoke dimensions, and solve for Rth. It's not much! Really only significant when a huge source of power is available, like asoldering iron tip!The better fabs are okay with 2.5 mil mask expansion, and webs down to 3 mil. I normally use rules of 2.5 or 3 mil expansion, and 3.7 mil minimum web. This allows for a 0.5mm pitch part to still have full mask between pads. You may need to shave pad widths slightly to get this to work -- it's perfectly acceptable to reduce pad width, by about 0.03 mm (an IPC-7351 side fillet), which may be what's missing to get you a reliable footprint.0.4mm pitch, and fine pitch BGA (less than 0.7mm or so?) tend to be difficult though, and in that case you may find a more accurate mask is required. LDI (laser direct imaging) has tighter tolerances, making this feasible.Incidentally, if you ever do a BGA, do yourself a favor and fully tent the vias on the solder side!Of course for fine pitch BGA more than a row deep, you're pretty much forced into HDI (with via in pad, but the vias are solid filled in an HDI process, so it doesn't matter).Tim

author: ahbushnell
author_rank: Frequent Contributor
timestamp: May 23, 2019, 01:39:28 pm
content: Great information. Just what I was looking for.ThanksAndy