Via in pad more expensive to manufacture? - Page 1
Forum section: electronics / projects

author: eneuro
author_rank: Super Contributor
timestamp: October 09, 2015, 06:24:00 pm
content: Hello,I'd like to send to prototype many such 1inch x 1/2inch (25mm x 12.5mm) double layer boards, where inductor will be on bottom layer, so it could be easy connect its pins to top layer using... via in padHowever, didn't asked board manufacturer for any issues with that, but there were different views.You never do it or do it a lot?Does it costs moreto manufacture such board with via in pad?I've found linked in other EEVBLOG thread PDFVia in Pad GuidelinesDo you expect any problems with via in pad eg. athttp://smart-prototyping.com/PCB-Prototyping.html?I see no tolerances shown on its page, but small via in quite big ( a few mm size pad on bottom side) any problem with that?Probably, I will ask them before sending finished PCB design to manufacture, but what do you think about those two vias shown in PCB layout above?

author: Monkeh
author_rank: Super Contributor
timestamp: October 09, 2015, 06:30:45 pm
content: Ask yourself how a via in a pad is any different to a via in a trace or a via in a plane.As far as PCB manufacturing goes it's business as usual. Assembly can be another matter entirely.

author: calexanian
author_rank: Super Contributor
timestamp: October 09, 2015, 07:08:34 pm
content: It used to be a big thing to do Via in Pads especially with through hole. I believe it was more of a drill integrity and software DRC issue. Now with mostly surface mount from a PCB manufacturer point of view its a non issue. It may however effect reflow soldering.

author: rx8pilot
author_rank: Super Contributor
timestamp: October 09, 2015, 07:16:32 pm
content: I have not used VIP yet but I have been looking into it as my designs are getting tighter and tighter. The problem on the fabrication side is that the vias have to be so small that they are laser drilled which not all houses have. For larger drilled vias, they have to be filled so that the solder does no wick through and cause assembly problems. That is why it is more expensive.If you are going to hand build a few PCB's, you can get away with just putting un-filled vias on the pads and be cautious while assembling. For larger qty, it can be a major problem with solder leaking to the other side of the PCB during re-flow.

author: georges80
author_rank: Frequent Contributor
timestamp: October 09, 2015, 07:26:38 pm
content: I use via in pad very often - certainly on all thermal pads for dfn/qfn etc. The assembly house needs to tweak their solder paste quantity (stencil design) to ensure sufficient solder and to cater for what can wick into the vias.Of course you can get plugged vias too - but more $.Very small diameter vias is another option since little to no solder will wick - but again typically more $ once you go below around 10mil diameter.As always, TALK with your assembly house for what they recommend...cheers,george.

author: rx8pilot
author_rank: Super Contributor
timestamp: October 09, 2015, 07:29:29 pm
content: I just did a few jobs with RUSH PCB. They do laser vias and the cost difference is not bad - better than crossing my fingers on how much will wick. I have not yet asked what plugged vias cost.

author: eneuro
author_rank: Super Contributor
timestamp: October 09, 2015, 07:49:25 pm
content: Thanks for hints guysQuote from: rx8pilot on October 09, 2015, 07:16:32 pmProbably in my case those two shown vias can be larger, since during assembly I'll try to make such trick, that both sides of double layer PCB will be reflowed at the same timeThat is why I've designed this PCB in a way that the only part on bottom side is inductor:This is 12mm x 12mm square shaped inductorso, while probably it will be maunufactured at home using my custom made PnP,first top layer will be PnP placed than solder paste added to this square inductor in place where we have pads on bottom side and PCB placed on top of inductor ready to put into reflow ovenI didn't tested it yet, but I think it can work and this way solder will not wick through too much even if I'll have bigger vias hole since gravity will keep solder on the bottom side inductor padsA little bit tricky-we'll see if it works

author: Alex Eisenhut
author_rank: Super Contributor
timestamp: October 10, 2015, 12:31:48 am
content: There's no problem putting drill hits inside pads, what adds complexity is if you want them plugged and capped.

author: rx8pilot
author_rank: Super Contributor
timestamp: October 10, 2015, 12:35:02 am
content: Quote from: Alex Eisenhut on October 10, 2015, 12:31:48 amThat is exactly right. For small qty, hand built PCB's plugging and capping may not be needed. For bigger jobs, the labor needed to find and fix soldering problems is what justifies the cost. If the cost is too high, re-spin the layout.