solder mask bridge between QFN pads, how important? - Page 1
Forum section: electronics / general

author: thinkfat
author_rank: Unknown
timestamp: May 08, 2019, 09:04:45 pm
content: I just got back some prototype PCBs from JLC and I noticed that they took out the solder mask between the pads of a QFN-40, 0.4mm pitch footprint.I asked for the reason and they said their minimum solder mask bridge is 10mil (0,254mm). This constraint is not listed in their manufacturing capabilities, btw.How important is it actually to have solder mask between the pads? For the prototypes and hand-soldering it didn't appear to be an issue, the PCB works as expected, would it be more critical for an actual PCBA run?BR,Matthias

author: DerekG
author_rank: Frequent Contributor
timestamp: May 08, 2019, 10:43:50 pm
content: It is fairly usual.They are assuming you are using a thin solder paste screen & having no mask between the pins will help the QFN sit hard against the board if there are any small placement misalignments.So ................. use minimum solder paste to do the job to avoid shorted pins.

author: mrpackethead
author_rank: Super Contributor
timestamp: May 09, 2019, 01:23:46 am
content: The real purpose of solder mask is not for stopping solder bridges. Solder will bridge across mask, if you have too much anyway, particually at fine pitches. Its to stop solder from wicking down tracks.. if you hav eever used a board with no solder mask ( prob dip parts ) you will know will know that you can put the solder on any old bit of copper.. For wave soldering this would have been horrific.At 0.4mm pitch your stenciling will need to be resoanbly good.

author: thinkfat
author_rank: Unknown
timestamp: May 09, 2019, 11:45:16 am
content: Quote from: mrpackethead on May 09, 2019, 01:23:46 amThat makes a lot of sense. Yes, I've seen that effect on vias place too close to pads so that there wasn't a solder mask dam in between. On reflowing the solder was wicked away by the via and the pad ran dry.Thanks a bunch!

author: AndyC_772
author_rank: Super Contributor
timestamp: May 09, 2019, 12:28:34 pm
content: Removing solder mask from between the pins of any fine pitch (0.5mm or thereabouts) device is completely normal.The greater risk is that, if you have very thin webs of solder mask between pins, they'll flake off and can end up on the pads, preventing a good solder joint from being made.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: May 09, 2019, 12:50:10 pm
content: Yeah, if you want industrial-grade soldering, get an industrial-grade fab.To be fair, 0.5mm is the limit for most (LPI) soldermask. To do better usually requires laser (LDI), so, special equipment and a custom run.Also, to be fair, 10 mils is a preposterously loose limit. That's barely good enough for SOIC, and won't even do TSSOP. Typical is 4 mils. JLC must be the only big proto-oriented Chinese fab that's that bad?For low quantities, you're probably in need of rework anyway (whether due to solder or assy defects, or component changes), so the potentially poorer soldering from missing mask isn't a big impact.Tim

author: nctnico
author_rank: Super Contributor
timestamp: May 09, 2019, 04:21:33 pm
content: In my experience the footprint specifications of 0.4mm QFNs are too optimistic. Assemblers have asked me to keep at least 0.2mm between the pads which results in 0.2mm wide pads for 0.4mm QFNs. With these geometries bridging is no longer an issue for the assemblers I have dealth with.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: May 09, 2019, 07:04:44 pm
content: What footprint specs? IPC says 0.2mm pad width is fine.Tim

author: nctnico
author_rank: Super Contributor
timestamp: May 09, 2019, 08:56:37 pm
content: The manufacturer's.

author: thinkfat
author_rank: Unknown
timestamp: May 09, 2019, 09:07:08 pm
content: Quote from: T3sl4co1l on May 09, 2019, 12:50:10 pmI think the wording was that they require 10 mil between the pads, it's not the minimum webbing. I have on the same PCB another QFN package with 0.5mm pitch, the pad distance is around 10mil and they kept the solder mask in between the pads just fine.

author: mrpackethead
author_rank: Super Contributor
timestamp: May 09, 2019, 10:36:29 pm
content: JLCPCB does .15mm ( 6mil ).. .254 is odd.

author: asmi
author_rank: Super Contributor
timestamp: May 10, 2019, 01:57:16 pm
content: Quote from: blueskull on May 09, 2019, 10:43:20 pmNot too thin for some:This is 0.4 mm pitch QFN (FT601), the board was manufactured by OurPCB.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: May 10, 2019, 07:40:25 pm
content: I can see what looks like breaks in the soldermask. This particular example may not have lifted webs, but it's very likely that another board in the batch does!Not that that's necessarily a killer either, but it's still a source of possible defects and subsequent rework.Tim

author: asmi
author_rank: Super Contributor
timestamp: May 10, 2019, 08:55:03 pm
content: Quote from: T3sl4co1l on May 10, 2019, 07:40:25 pmNo, there are no breaks on any of boards - I manually inspected them all under stereo microscope. I've manufactured three batches of boards with them, and none of them had a single solder stop break in either 0.4 mm QFNs or 0804 4-resistor networks. Not saying it's going to be that way for every future boards, but so far it's been perfect.It probably helps that they are not aiming to be the cheapest manufacturer, instead putting more emphasis on price-to-quality ratio, and so far they delivered. See my threadhere- there are more photos there, as well as some feedback from others.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: May 11, 2019, 07:42:09 am
content: Quote from: asmi on May 10, 2019, 08:55:03 pmAh, that does indeed sound good, and alignment in the other photos looks excellent.Tim