Via directly on PAD - Page 1
Forum section: electronics / general

author: baku1413
author_rank: Newbie
timestamp: March 29, 2020, 07:30:04 pm
content: Hi.I'm prototyping board with tiny SMD IC (3x3mm) which will be switching rather high currents for it's size (even 5A). Can i place vias on to pads like in picture below, even when they are little bigger than trace outline? I wanted them smaller but JLCPCB can't make smaller vias.IC is SY6982E

author: T3sl4co1l
author_rank: Super Contributor
timestamp: March 29, 2020, 08:21:23 pm
content: No.I mean, you can, and if you're soldering it yourself, it's up to you to inspect it.That looks like one of those DFNs that's impossible to inspect outside of x-ray, so good luck.You say "high currents for it's  size", but have you checked if the device is not simply rated to handle that current with an ordinary footprint?Also, what happened to the, soldermask I guess, beside C4?And why use different sizes and numbers of vias in the chip components? C7 is going to be starved as all the solder wicks into those two huge vias, while R2, C1 and others have one lone via that won't actually affect much.Also, is this 2 or 4 layers? You may find it's better to keep solid copper (GND most likely) on the back side, to spread out what heat conducts through the board (not all that much, really), to keep stray inductance low, than to saw it up for thermal pads (which really don't have anywhere to go, among the 4-5 nets with heatsinking implied by your via use). Especially if it's switching 5A.Whereas if it's 4 layers, you can put whatever you want on the bottom side, and have ground on the inner top layer (assuming this is a top layer view), much closer to the footprint (less board thickness to conduct heat through), which does a quite good job indeed.You can also get better thermal performance using a thinner 2-layer board, but less than 0.8mm thickness is likely custom, and even then they usually charge a little more for 0.8 versus 1mm. Whereas the outer layer to inner plane distance in a 4-layer board is typically 0.2mm or thereabouts (see mfg layer stackup).Hm, I don't see an inductor (unless the big thing on the right is), is it actually just a battery management switch (over/under charge), not a regulator? You didn't say...Tim

author: thm_w
author_rank: Super Contributor
timestamp: March 29, 2020, 08:40:52 pm
content: 5A is the absolute maximum, not sure if you can design around that, but anyway, check the example layout in the datasheet and copy that:http://www.szyucan.com/upfile/IC-PDF/SY6982E.pdf

author: baku1413
author_rank: Newbie
timestamp: March 29, 2020, 09:13:43 pm
content: Many thanks for advices.There are visible pads on the side of IC so I think I can succescully check connections with DMM.I think there is no other footprint avaiable for this IC.Accidentaly removed soldermask but it's repaired.I put one small via only on signal traces like R2, I will reduce via size on C7It's 2 layer board.Yup inductor is the big thing on the right. It's a 2S li-ion charger that boost 5V to 8.4V with adjustment of charging current to protect weak sources like USB in PCBut when source is capable it can also charge them fast.It's just a prototype I will give it a shot

author: baku1413
author_rank: Newbie
timestamp: March 29, 2020, 09:21:11 pm
content: Looked on to suggested layout. My is very similiar. But now i think removing vias from under IC is better choice.

author: ogden
author_rank: Super Contributor
timestamp: March 29, 2020, 09:41:03 pm
content: Only if your PCB manufacturer do proper via-in-pad fill & plating. Obviously expensive tech, not subject for hobby or mass/consumer production. First internet search hit which pretty much explains what it is about:https://macrofab.com/blog/via-in-pad-pcb-design/

author: Doctorandus_P
author_rank: Super Contributor
timestamp: April 22, 2020, 08:43:04 pm
content: As said before, your solution has some problems.* It decreases clearance in an almost impossible to inspect spot.* Open via holes suck up the solder paste.And it's not needed at all.Just extend the pads of your IC outwards, and also the solder mask cutout.The extra solder on the pad will help keep resistance down.Just outside the IC you can make the track wider to handle your 5A current.Also those 5A is an absolute peak and of short duration.You will probably be all right if you design the PCB for the nominal 2A.