Vias on pads? - Page 1
Forum section: electronics / projects

author: blueskull
author_rank: Unknown
timestamp: March 01, 2015, 05:36:55 am
content: Hi,In my radio frequency generator project I used a triple row QFN device with 0.5mm pitch. Apparently I am having a hard time placing and routing the board. I'd like to know if anybody tried to put vias on top of pads? Will that work?The smallest vias I can make is 10/14 mil (OSH Park 4 layer). The board thickness will be 1.6mm. The bottom side of the vias will be covered with solder resist, so effectively they are plugged vias.I will be using stencil+low temp paste process to assemble the board. I don't care about DFM and quality, because what I want to do is just to prove my design, and this is not a product.Thanks,Bo

author: Ice-Tea
author_rank: Super Contributor
timestamp: March 01, 2015, 07:42:58 am
content: Two possible issues I guess: the via hole will suck the solder joint dry and the pad won't be 100% level anymore. But I guess that if DFM is no issue you should be able to get away with it

author: Howardlong
author_rank: Super Contributor
timestamp: March 01, 2015, 07:47:21 am
content: The problem with via in pad (disregarding thermal vias often used in power pads) is that the wicking of the solder will make production very difficult as getting a uniform solder distribution across pads is hard.Some PCB manufacturers offer Filled vias as an option but it tends to be expensive. This also is not perfect as although you've stopped the wicking, you haven't stopped the thermal differences between similarly sized adjacent pads so getting reasonable reflow yield may take a few attempts. Making them all filled vias is an option, maintaining the same thermal properties of all the pads, but then you'll often still have routing problems around the vias themselves.Is there an example fan out image available online for this package? I have seen "double" row QFN Type packages (Microchip use VTLA for example) but not triple, and at 0.5mm, fanning out is certainly going to be a challenge.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: March 01, 2015, 05:15:28 pm
content: Sounds like a crappy footprint... I'd just as well opt for a proper BGA.Doing it in two layers seems wildly optimistic, too.Tim

author: MagicSmoker
author_rank: Super Contributor
timestamp: March 01, 2015, 09:51:41 pm
content: Technically, putting a via inside a SMT pad footprint is verboten, but sometimes unavoidable. For example, a SMSC ethernet PHY is in a QFN package with the ground connection on the central bottom pad (sometimes called the "die attach pad" or "...paddle"). The datasheet says that package ground must have a low-impedance connection to the board ground plane and the best way to do that - assuming the ground plane is one layer below top - is to put a few vias in the central pad. You can spring for tented or filled vias at the board house (beware - can be surprisingly expensive) or you can just live with a bit of your solder paste getting sucked into the vias during reflowing. I chose the latter and haven't have a problem with the first 40 or so boards, but if the chip produces a lot of heat and relies on the DAP for heatsinking I would probably spring for getting the vias filled/tented.

author: ludzinc
author_rank: Unknown
timestamp: March 01, 2015, 10:22:22 pm
content: Quote from: blueskull on March 01, 2015, 06:14:41 pmYour via will suck the solder from your ball, and your part has a good chance of not working (open circuit contact).If I were you, I'd look for a different part (not always possible) or pony up for the correct PCB technique.

author: codeboy2k
author_rank: Super Contributor
timestamp: March 01, 2015, 11:33:18 pm
content: Those vias will absolutely not work. As said, the paste will just flow down to fill the via. If you continue with this part, you will need to get the board house to fill and plate the via for you to prepare the pad for solder paste.QuoteIf it's not a product, and just a proof of concept, then see if you can get a different part (i.e. bigger part) with a better pad layout. If it's one off (sounds like you are doing a home stencil ?? ) then perhaps you can go with the via in pad as you've drawn it, and fill the pads at home one by one yourself. It won't be too much work, and if you have a stencil then you can apply paste first to just that part, hot air that, do some additional work to level the pads as best as you can, let it cool, then apply paste again before applying the part.

author: Alex Eisenhut
author_rank: Super Contributor
timestamp: March 02, 2015, 01:25:18 am
content: Quote from: MagicSmoker on March 01, 2015, 09:51:41 pmI certainly hope not. Most of my layouts for the last few years have been HDI microvia-in-pad affairs. Will I be arrested?