JLCPCB Vias in large SMD pads? - Page 1
Forum section: electronics / general

author: phil from seattle
author_rank: Super Contributor
timestamp: October 19, 2024, 04:39:12 pm
content: Looking for feedback on the JLCs ability to handle vias in SMD pads. I've used them a fair number of times and have generally avoided vias in pads but this design I am working on has a part that the manufacturer recommends vias in the pads. It's an RP2350B - lpf80 and the vias are in the large ground pad on the bottom. See the screenshot below..I've heard of solder paste leaking out vias during reflow and causing solder starvation. But, I have also heard it's an old problem and most manufacturers have solved the problem. Has anyone used vias like this with JLCPCB? Any cautions? As long as I am at it, any experience on this topic with other manufacturers?

author: wraper
author_rank: Unknown
timestamp: October 19, 2024, 04:42:39 pm
content: Tenting opposite side prevents most of solder leakage. You may need to apply a bit more solder paste for vias vs no vias or capped and plated vias.

author: wraper
author_rank: Unknown
timestamp: October 19, 2024, 04:45:58 pm
content: Also it looks like JLCPCB offers free proper via in padhttps://jlcpcb.com/blog/jlcpcb-free-via-in-pad

author: T3sl4co1l
author_rank: Super Contributor
timestamp: October 19, 2024, 04:48:18 pm
content: Paste doesn't leak out, it's not that fluid. But solder can wick in during reflow.Use small diameter (<= 0.3mm) and relatively few, to reduce the "wickability", and solder volume that can be consumed. Lead-free tends to wick less than leaded as well.DO NOT tent the backside: this traps flux in the barrel, which will bubble out during soldering, making voids very likely.Tim

author: tooki
author_rank: Super Contributor
timestamp: October 19, 2024, 04:58:35 pm
content: There’s no difficulty whatsoever for the PCB house to manufacture this. No vias in pads is simply good practice for most things. But they’re extremely common for ground pads on QFNs, DPAK, etc., especially to improve thermal conductivity.I don’t know why you’d think the “manufacturer” has any role in solving solder starvation: you determine the amount of paste by your paste stencil aperture design. If the issue is the solder paste flowing out before it actually melts, I mean… it still leaves behind enough. Starvation happens when the amount of paste applied is correct for the pad size, but didn’t take the vias into account, which will mop up a bit.(Yes, many PCB manufacturers, including JLCPCB, automatically reduce your apertures by default, since many PCB footprints inexplicably use apertures the same size as the pad, which is way too much paste with normal stencil thickness. You can ask them not to apply the reduction, and I’m actually not sure if they do that to custom pads like the ground pads in question.)There are other things you can do, too. One is to use tented vias on the opposite side, which means the solder mask goes over the via. On small vias, this will close them up most of the time. That stops solder from escaping.The luxury option is to use vias that are completely filled in and plated over (that is, the finished pad doesn’t even have any holes). This is called “via in pad plated over”:https://www.viasion.com/blog/understanding-via-in-pad-plated-over-vippo/But unless you need that on the same board for a BGA anyway, I wouldn’t bother with it for the stuff we’re talking about. I’ve done vias in ground pads many times, without giving it particular attention, and it’s been fine. The problem has usually been too much solder paste if anything, when using a different PCB manufacturer and forgetting to adjust for their different aperture reduction defaults.

author: tooki
author_rank: Super Contributor
timestamp: October 19, 2024, 04:59:50 pm
content: Quote from: T3sl4co1l on October 19, 2024, 04:48:18 pmIsn’t that why we divide the stencil apertures for large pads into quadrants with a gap, so flux and its vapors can escape?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: October 19, 2024, 05:56:24 pm
content: Nah that's so the mask and squeegee works properly; too wide an unsupported gap and the squeegee scoops down into it, thinning the deposit inconsistently (depends on pressure).Paste kinda melts and spreads out on the board and in the joint; paste-per-pad helps just a little bit (I mean, enough it's still worth doing), but you can do almost as well spreading paste across, say, TSSOP pads in a continuous bead. It migrates enough by spreading out and coalescing that it's not as particular as you might think. Look up some videos on reflow process, see how things move.Flux definitely wicks into the holes, and you'll see it bubbling out the bottom; solder itself not so much, but it's able to wick down, given enough time and activation.Tim

author: tooki
author_rank: Super Contributor
timestamp: October 19, 2024, 06:22:49 pm
content: Quote from: T3sl4co1l on October 19, 2024, 05:56:24 pmThat is another (arguably more important) reason, but gas venting is a reason for it.E.g.https://iconnect007.com/article/118546/smt-stencils-101-what-are-industrystandard-stencil-designs/118549/pcbsays:QuoteMore links:https://blueringstencils.com/wp-content/uploads/2019/09/Root-Cause-Stencil-Design-for-SMT-Component-Thermal-Lands_Paper.pdfhttps://www.circuitnet.com/experts/87782.html

author: langwadt
author_rank: Super Contributor
timestamp: October 19, 2024, 06:25:43 pm
content: Quote from: tooki on October 19, 2024, 04:58:35 pmI'd assume for the case that JLCPCB is not just making the PCB but also the assembly

author: thm_w
author_rank: Super Contributor
timestamp: October 21, 2024, 09:07:15 pm
content: Your footprint looks wrong to me, dimensions don't seem to match up to the datasheet:https://datasheets.raspberrypi.com/rp2350/rp2350-product-brief.pdfMaybe double check.

author: phil from seattle
author_rank: Super Contributor
timestamp: October 23, 2024, 04:38:22 pm
content: Quote from: thm_w on October 21, 2024, 09:07:15 pmI took that straight from the demo board that's part of the "Hardware design with RP2350" document from Raspberry PI Ltd. What specific issues are you referring to?

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: October 23, 2024, 06:08:21 pm
content: Quote from: tooki on October 19, 2024, 04:59:50 pmNo, it's to reduce the amount of paste on a large pad to stop the part floating up due to surface tension

author: thm_w
author_rank: Super Contributor
timestamp: October 23, 2024, 09:56:52 pm
content: Quote from: phil from seattle on October 23, 2024, 04:38:22 pmIgnore me, was looking at the wrong package (not QFN80).

author: wraper
author_rank: Unknown
timestamp: October 24, 2024, 06:11:56 pm
content: Quote from: mikeselectricstuff on October 23, 2024, 06:08:21 pmIt's helpful for several reasons. Reduces the amount of paste, lets gasses escape thus reduces voiding, prevents chip tilting. One benefit of doing this does not make other benefits disappear from existence.

author: tooki
author_rank: Super Contributor
timestamp: October 24, 2024, 08:30:24 pm
content: Quote from: mikeselectricstuff on October 23, 2024, 06:08:21 pmOne can simply reduce the aperture (without dividing it) to accomplish that alone.My understanding is that the "window pane" design is primarily to vent gas and prevent squeegee scooping on large parts.

author: wraper
author_rank: Unknown
timestamp: October 25, 2024, 08:34:05 am
content: Quote from: tooki on October 24, 2024, 08:30:24 pmThere is another benefit of doing this. You don't want to make too large openings in the stencil as it may cause squeegee push below the stencil surface and leave thinner paste layer in the middle of large opening.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: October 25, 2024, 10:21:44 am
content: Is that not what "scooping" implies?Tim

author: tooki
author_rank: Super Contributor
timestamp: October 25, 2024, 11:01:44 am
content: Quote from: wraper on October 25, 2024, 08:34:05 amThat is what “squeegee scooping” means.

author: wraper
author_rank: Unknown
timestamp: October 25, 2024, 11:26:45 am
content: ^somehow missed second part of the sentence.

author: tooki
author_rank: Super Contributor
timestamp: October 25, 2024, 04:16:53 pm
content: Quote from: wraper on October 25, 2024, 11:26:45 amSorry… what?!? What did I miss?Your entire sentence simply explains what squeegee scooping is.What exactly is it you think you’re saying that T3sl4co1l and I did not already cover? Squeegee scooping = the squeegee pushing into large stencil openings, causing the paste to be scooped out, leaving insufficient solder paste.

author: wraper
author_rank: Unknown
timestamp: October 25, 2024, 04:19:32 pm
content: I meant I missed, not you.

author: tooki
author_rank: Super Contributor
timestamp: October 25, 2024, 04:43:29 pm
content: Ah. Names or pronouns are useful things.