PCB Design - Vias in Pads - Page 1
Forum section: electronics / projects

author: dannybeckett
author_rank: Contributor
timestamp: June 24, 2013, 12:02:13 pm
content: Hi guys -Just a quick question about using vias in pads - are there real world problems with doing this, or is it not such a bad idea? In principle, I see no problem with putting a via in a pad - it saves space on the board and could potentially provide the shortest signal path possible. In reality, I've heard that there can be soldering issues, mainly being that the solder gets wicked down through the via whist the part gets soldered. I've seen no evidence for this however, just people saying i's a bad idea. Does anyone have experience with this technique?

author: digsys
author_rank: Unknown
timestamp: June 24, 2013, 01:21:53 pm
content: It's no different to having a plate through hole with the bottom layer retaining the solder mask.IF you're doing automated assembly and depending on where / size relative to the pad of the via, theremaybe some issues,but easy to fix. I've done it many times for various reasons, no biggie. Some may say it's notconventional. YMMV

author: ddavidebor
author_rank: Super Contributor
timestamp: June 24, 2013, 01:29:43 pm
content: If the board is good quality it's good.With poor crap soldermask, the solder can move under it. Well, it's not a great problem, work fine anyway.

author: millerb
author_rank: Regular Contributor
timestamp: June 24, 2013, 01:32:26 pm
content: If you get them filled and plated then no worries.QuoteThere are about a bazillion articles, academic studies, etc out there on the net about this and they all indicate that putting vias in pads is a bad idea unless they're plugged and plated over.

author: Psi
author_rank: Super Contributor
timestamp: June 24, 2013, 01:53:37 pm
content: If you're hand soldering then there's no issue at all.

author: poorchava
author_rank: Super Contributor
timestamp: June 25, 2013, 07:56:25 am
content: Vias in pads are a no-no when assembly is done by reflow, because vias will suck in the solder due to capillary effect. For wave soldering and hand soldering they are not an issue.

author: steaky1212
author_rank: Regular Contributor
timestamp: June 26, 2013, 11:59:37 pm
content: If getting reflowed then talk to the assembly house. They might want to increase the amount of paste to compensate for the via, and it might affect the thermal profile of the board...But if you need short traces for low inductance then you can't really beat via in pad.

author: lgbeno
author_rank: Frequent Contributor
timestamp: June 27, 2013, 02:04:13 am
content: Yeah I have to say via in pad is great but for sure if you are doing large scale production of a reliable product, they should be filled and capped otherwise your process really won't be repeatable. For large thermal pads a leaded parts maybe to impact isn't as great but to fine pitch parts where you only have a micro dot of solder to begin with, this will lead to big problems.Maybe your board will pass test at room temp or with zero vibration but what about when it is in the field and fails because of a weak joint or some other latent issue. Might take some time or abuse to sheer apart.If its a hobby and not production, have at it but I would argue that it wouldn't be wise to sell and ship product using unfilled vias in pads...

author: frank26080115
author_rank: Regular Contributor
timestamp: June 28, 2013, 07:35:17 am
content: I had a problem where the flux in the hole would explosively burst out of the hole, this was during hand assembly, wear your goggles!

author: thinlayer
author_rank: Contributor
timestamp: June 28, 2013, 11:07:56 am
content: The problem is variation in your PCBs, by your PCB manufactuers.You'll get one batch where the LPI is thick enough for a plug, and you'll think things are ok. The another batch where a different guy ran the machine and suddenly it's too thin, you get wicking, you get open balls. Only really a problem with small pads, fine QFN BGA no no. QFP 0.5mm grey I wouldn't, larger fine.And if you specify capping you pay for it, and some cheap houses can't. Somethings a void will pop! Escaping gasses are always fun. You could try specifying dry mask as this has consistent thickness... anyone done it with dry? Again, limits number of PCB houses as LPI seems most popular.What about specifying a HAL solder finish? Then the via would take all it can wick during the finishing of the board? Anyone done that?

author: lgbeno
author_rank: Frequent Contributor
timestamp: June 28, 2013, 10:37:38 pm
content: Quote from: thinlayer on June 28, 2013, 11:07:56 amWrt to LPI or solder mask filling the holes, I don't think this is possible because they are already masked away, vias are in the pad after all.HASL question is interesting since it would likely fill in vias as you are suggesting. The pitch that we are talking about for when unfillied via in pad no longer makes sense could be about the same argument for HASL... I guess I'm more familiar with RoHS soldering with either ENIG or Immersion Silver. Only my hobby stuff is done with HASL, at work we would use something a little more premium.Fill and cap is $$ though...