Via in pad - Page 1
Forum section: electronics / projects

author: OM222O
author_rank: Frequent Contributor
timestamp: July 25, 2020, 09:38:42 am
content: HiI've been using the "via in pad" pretty extensively for different things, such as: reinforcing the screw mounting holes, connecting signals or power / gnd to chips while using the underside as a bus, etc.So far I've had no issues with singal integrety, power issues,soldering components, or any other issues. Watching today's dave video about PCB layout practices made me wonder why he didn't recommend this method? Is there something wrong with them? It saves a ton of space when routing, especially on 4 layer boards where it basically eliminates all the power and ground routing.

author: voltsandjolts
author_rank: Unknown
timestamp: July 25, 2020, 09:44:39 am
content: Only downside I am aware of is that via in pad can suck molten solder away from the pad-component joint and reduce reliability.For manual soldering that doesn't apply, just add more solder.

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: July 25, 2020, 09:49:25 am
content: Quote from: OM222O on July 25, 2020, 09:38:42 amDave, contrary to popular belief sometimes, is not the end-all-be-all expert in this kind of stuff. (nor is anyone else here, and I'm definitely not an expert- I just wanted to point out that you will always find differing opinions and practices depending on who you ask)One problem you can get with via-in-pad, esp if you don't have plugged vias, is that on very small components, the amount of solder that wicks into the via can be significant and make the joint poor, or increase the likelyhood of tomb-stoning.In my experience via-in-pad can be useful for high-density, but I've only used it a few times on bigger pads mostly for cooling. I've also done it with screw-mounting, but I don't really consider that via-in-pad, because it's not a true pad I'm soldering a component to.One of the issues we do have on our high-density flip-chip components is that the presence of a via will actually influence the surface of the plated material, which can reduce our yield.

author: paul8f
author_rank: Regular Contributor
timestamp: July 25, 2020, 09:51:31 am
content: If that pad ever gets reworked, maybe there's a risk of the via going open cct?(Just my own opinion, I've no evidence of this happening!)I also agree with the other posters suggesting the wicking issue.

author: soFPG
author_rank: Frequent Contributor
timestamp: July 25, 2020, 09:58:32 am
content: What does Via-In-Pad mean? Just an un-tented via right where the BGA-ball is?

author: Siwastaja
author_rank: Super Contributor
timestamp: July 25, 2020, 10:18:24 am
content: For stray inductance, via-in-pad is preferable.For routing area usage, via-in-pad is preferable. You save a lot of space.It's all about solder sucking, really. Reliability issues are hard to assess if you are looking at one-off successes. 999 out of 1000 may be fine, then one fails.Thermal conductivity balancing can be problem as well. Same as using a large pour of copper on one of the pads. Can cause tombstoning.Laser drilled 0.1mm microvias are OK, they do not suck significant amounts of solder.If you have 0.2mm drill available at your fab you are using, that'susuallyOK as well, but maybe a bit iffy.Copper-filled holes are ultimate, but expensive. The pads look completely normal and flat. No solder sucking, and massively good electrical and thermal conductivity. They conduct a lot of heat during soldering, though, which you must take into account, balancing the pads.Via-in-pad is often specified in datasheets and used with large power components, with a lot of solder (large mask opening). Solder sucking doesn't matter when you have so much in excess. Still, use max. 0.3mm hole, IMHO.

author: Siwastaja
author_rank: Super Contributor
timestamp: July 25, 2020, 10:24:39 am
content: Quote from: soFPG on July 25, 2020, 09:58:32 amYes, or any other component lead/pad.Since the hole is completely open, and plated with the same plating as the pad, solderwillflow into the hole, more or less.

author: forrestc
author_rank: Unknown
timestamp: July 25, 2020, 10:37:46 am
content: Quote from: OM222O on July 25, 2020, 09:38:42 amAs others have said, it has to do with solder consumption. If you're hand-soldering it isn't a big deal.Generally if you have a via 'attached' to a pad in some way (i.e. not separated with enough solder mask), it will suck the solder off of the pad and into the via. In typical mass assembly you'll find that any 'via in pad' or 'via too close to pad' joints will end up with less solder and often will end up without sufficient solder for reliable joints. To avoid this you have to either use a very small via which doesn't need much (if any) solder, or get your assembly house to fill the vias during manufacturing. I.E. "plugged vias". Although I've never intentionally used one, I definitely have had situations where I didn't separate a via far enough from a pad and ended up with an assembly run where I had to rework most of the joints on that pad to ensure adequate solder coverage since all of the solder ended up in the via..So if you're getting something assembled and there is a choice to do so, you generally want to avoid this. However, there are quite a few situations where you really can't avoid it, so you have to resort to using them and dealing with the repercussions.

author: Unixon
author_rank: Frequent Contributor
timestamp: July 25, 2020, 11:22:09 am
content: HAL finished PCBs are also safe against solder sucking issues because vias are already filled with solder, but unfortunately HAL may be incompatible with BGA packages.

author: Siwastaja
author_rank: Super Contributor
timestamp: July 25, 2020, 11:27:34 am
content: Quote from: Unixon on July 25, 2020, 11:22:09 amSorry but this advice is incorrect. HASLsometimesgetssomesolder into the vias, but not reliably.(I have made exactly that mistake and seen the results so this is why I know.)

author: OM222O
author_rank: Frequent Contributor
timestamp: July 25, 2020, 11:32:02 am
content: I have mostly used it with 1206 , 0805 and SOIC or QFP packages. Others likeSOP or SOT are usually way too fine pitch to actually use via in pad.I actually never had issues with too little solder or unreliable joints. I order from jlcpcb with HASL which I assume fills the vias beforehand? If solder sucking was an issue I assume you can increase the paste "extension" on the pads which have vias in them, since a bigger stencil cutout means more solder for the pad?Also no issues with tombstoning.

author: Unixon
author_rank: Frequent Contributor
timestamp: July 25, 2020, 12:05:16 pm
content: Quote from: Siwastaja on July 25, 2020, 11:27:34 amOh, thanks for correction, I should have said "probably safe", HASL is not that much reliable especially for small vias.

author: ogden
author_rank: Super Contributor
timestamp: July 25, 2020, 12:46:52 pm
content: Quote from: OM222O on July 25, 2020, 09:38:42 amVia-stitching of ground planes, transmission lines, mechanical holes, also thermal pad vias shall not be confused with via-in-pad. Thermal pads have through vias for a good reason. When youmanufacturemake products for yourself or "use at your own risk" market - everything that works for you is fine. When you work for volume consumer/industrial market - use only plugged+plated via-in-pad or better avoid if possible because such adds to the cost. Furtherreading1reading2I wonder - anyone here with experience using blind vias as "lower cost" via-in-pad?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: July 25, 2020, 03:28:13 pm
content: Quote from: Siwastaja on July 25, 2020, 10:18:24 amParticularly on lead-free, which flows much more slowly than leaded solder. I've seen QFN pads that didn't wick with this combination, 0.3mm even. (Some vias do wick visibly, and moreso the larger the hole. It's not a perfectly repeatable thing, sometimes none do, sometimes a few...)By the way, do not use tented vias, in an effort to block the flow of solder into the hole -- this backfires, quite literally: the solder flux (and other residues from PCB fab) outgasses through the open end, causing voids in your solder joint. Either leave the via open both sides, or tent/cap it both sides.A tented viatouchinga pad, however, will neither void the solder joint, nor steal solder. This can help squeeze out precious fractions of a mm in a design.QuoteYup. There's also filled and capped vias. Expensive -- there are additional steps to mask, paste and plate only the target holes, by hand as I understand it. The result is fantastic, not as conductive as copper-filled of course, but the vias are completely flat and no solder wicks away.Speaking of laser drilled, they often plate shut anyway. You might see a little dimple on the board, not planar like filled-and-capped, but hardly anything to worry about. HDI has this between every layer pair, so you don't have vias blocking traces or components on the opposite side, it's a routing free-for-all! You can easily route fine pitch BGAs.Tim

author: Someone
author_rank: Super Contributor
timestamp: July 25, 2020, 11:14:23 pm
content: Quote from: ogden on July 25, 2020, 12:46:52 pmI have only ever seen that on the "not recommended" list, for the same reasoning as tented vias; as discussed by T3sl4co1l above.