Aspect ratio and different vias width

Question

I've recently been looking into the width of vias, and could use the feedback of more experienced designers.

Through-hole vias :

I've read that for through-hole vias, the way to go is 8:1 (so if your PCB is 1.6mm thick, then the ideal via will be 0.2mm wide).

From that point on, would there be any reason for me to use a different width ? If i were to use a 0.4mm via (4:1 aspect ratio), would that impact the reliability of my PCB ?

I've seen a lot of PCBs with vias much wider than that, and now don't really understand why. I used to naively think they'd be able to handle more current, but that's only up to the thickness of plated copper going down the barrel right ?

Going a bit further, with microvias and blind vias

I've been able to read a bit about microvias. To sum it up, they're at most 0.25mm deep, and the ideal aspect ratio is somewhere around 0.8:1 (so wider than deeper). My first question is, are aspect ratio calculated from the drilling size, or finished hole ? I've read contradictory opinions on the matter, and at such small numbers, the 35µ of copper start to matter.

Secondly, I've been able to read enough things about microvias, but blind vias seem to be overshadowed by their smaller brother. From what I've understood they're manufactured similarly to through-hole vias. As such, should their aspect ratio be calculated from the same 8:1 ratio ?

With all that being said (or asked), would defining my stack-up and calculating my via widths once from that be best practice ? As such, should all my TH vias be the same width ? No matter if they're stitching, high current, high speed or anything else ?

If you have any wisdom to share regarding via width/failure or aspect ratio, I'd be happy to read it.

Answer 1

My first question is, are aspect ratio [of a microvia] calculated from the drilling size, or finished hole ?

The main issue is just focussing the laser down into the hole without the edges of the hole getting in the way. So it should be the drilled size that matters. But ask your fab to be sure that's how they've written their spec.

From what I've understood they're manufactured similarly to through-hole vias. As such, should their aspect ratio be calculated from the same 8:1 ratio ?

I assume you're asking about blind vias here. Actually you should specify controlled-depth drills, because some people might consider microvias to be a sub-category of blind vias.

Controlled-depth drills are made by mechanical drilling, but the drill simply isn't lowered all the way through the board.

I'd expect the fab to limit the size to the same range as for through drills, so the aspect ratio that matters is the drill size to the full thickness of the board, rather than to just the drill depth. But again ask your fab to be sure. If you're drilling very shallow vias into a very thick (3 mm or more) board, I could imagine they'd let you use a smaller drill than they would allow for a through via.

If you aren't doing a controlled impedance design you should try to avoid controlled-depth drills, because they're a slightly fussy operation that the fab will charge you extra for.

(I assume you're considering micro vias in order to break out a high density component like a BGA and can't avoid them. If that's not the case you should also avoid micro-vias because adding additional operations to the fab process adds cost)

As such, should all my TH vias be the same width ?

No, there's no reason to make all your vias the same diameter. You'll want larger vias for high-current routes, for example. If you have through-hole components you'll also be making drills sized to fit the pins of those components and that won't match your minimum via diameter. The fab shop doesn't care about the difference between a plated mounting hole or pad and a plated through via --- they're all just drilling operations done prior to plating.

Answer 2

This is more a comment than an answer, but it wouldn't fit in the comment section and it does answer some parts of your question.

A larger drill size can carry more current; the current capacity goes up roughly linearly with via diameter. The plating thickness on a via is going to be about the same as the plating thickness on the board's outer layers, so 35 μm for a standard 1 oz copper board.

It's probably more space-efficient to use multiple small vias, though. Some PCB fabs might charge based on the number of vias, which could be a reason to use larger vias over smaller ones, though I've not encountered that personally.

Another consideration is cost. Some PCB fabs will charge more for vias below a certain size, because a 0.2 mm drill bit is going to break more easily, and thus require more frequent replacements, than a 0.3 mm one.