Screaming Circuits: Via in Pad

More Thoughts on Via Near Pad

The other day, I wrote about vias near pads. The post got a couple of interesting comments on the Circuit's Assembly blog, where it was also published.

Move via to the leftSome very interesting thoughts there. One of the things Mich said was: "When I was learning PCB design in the 1980's I was taught by a mentor that understood assembly very well." I think that highlights a big component of the problem. I suspect that a lot of folks doing layout today were not taught by anyone but themselves.

CAD packages may have instruction manuals and tutorials, but learning how to use a software package is a lot different than learning how to do the actual process well. It's possible to be very proficient at using a word processor, but still not know how to write well.

It's not an uncommon scenario these days, especially after the economic suckiness of last year, to come in to work expecting to hand off a schematic to the layout engineer only to find that "tag you're it."

Howard, in another comment, suggested that in his experience, filling and plating over vias in pads typically only adds about 8% to the PCB cost. In smaller prototype quantities, it may be a little more than that, but what's the cost of a failed assembly? If you have the room to move the vias off the pads, the only cost may be in layout time. If space is critical or if there are signal/noise/thermal issues that force the vias to be in the pads, then you'll just have to spend the extra to fill and plate.

If you do find yourself suddenly tasked with layout and you've never done one before, find a mentor (or maybe a Minotaur), read up online, call up a manufacturing person, study the Screaming Circuits blog. What ever you do, figure out all these little traps like vias in pad, components library foot print issues, spacing issues, thermal issues, etc. Then dive into the layout and learn from each one. Drink some tea too. It can relax you. Just try to stay away from Oreos and ice cream late at night.

Duane Benson
What's the deal with 1729?

Via Near Pad

Passive vias in both pads Vias don't go well in pads, of course. In fact, I think it's fair to say that vias go as well in pads as large igneous rocks go in peanut butter and jelly sandwiches.

But it's not just vias in pads that annoy people. Vias near pads can be pretty much a nuisance too. In the SOIC pictured here on the right, the pin 1 lead is at risk of having the solder Via near pad SOIC wicked off the pad and down into the via. If you've got to have a via right near a pad like that, always make sure there is something between the pad and the via that will keep the solder away. A thin line of solder mask, or even silk screen, like with the pads and vias on pins 12 and 14, will do. Anything to stop the solder from going where you don't want it to go.

Duane Benson
Jersey barriers, perhaps?

What's Wrong With This Picture?

Vias through stencilopeningsWhat's wrong with this picture?

I forgot to warn you that there'd be a pop-quiz. It's only worth 10% of your final grade though, so not to worry.

We're fully into the rainy season here in Oregon now. It's dumping and the puddles are puddling up. Last weekend, we thought we were in for another big snow and ice mess, like December 2008, but it turned out to be just media hype. We warmed up and it's back to the usual 40 degrees and raining.

Unlike with a QFN thermal pad, we do want open holes in our streets. We want the liquidy stuff to go down underneath and not stay up top, 'cause that would make our feet wet and Johhny doesn't like wet feet.

Duane Benson
If it's bipolar, it's a "collector." If it's a MOSFET, it's a "drain." What is it if it's a street?

Parts Substitution Gone Big

Cap too big tant I've mentioned some cautions with parts substitutions before; wrong V values on barrier or flyback diodes, counterfeit parts and things like that. Here's another example of something to watch out for if your supply is tight and choices are limited.

One of the things that I've run across a couple times, especially when hunting down capacitors, is the package size issue. Say, I need a 16uf, 10V cap on one of my boards. It's not a critical app. I don't particularly care about ESR, temperature or even much about tolerance. I just need a little head room in case of minor spikes or power line ripple. I'm not expecting a lot. I just want that safety margin.

Cap too big electBut when I run over to my parts supplier, the specific cap I picked two weeks ago, when I started the design, is out of stock or jumped in price. I want to get building, so I just look through my parts drawers for something close. There it is, a 22uf, 50volt cap. It'll still work just fine. The problem is, of course, that I neglected to realize that the part  jumped up a notch in size. Bummer days.

I've run across the same problem, not due to a sloppy sub, but also due to picking the wrong footprint in my CAD package. I find that particularly easy to do with SMT electrolytic caps.

The other thing in these examples to watch out for is the open vias next to the pads. Granted, they aren't in the pads, but they are close and without any kind of a break in the metal before the via. In the left pad of the yellow tantalum cap, I added in an example of a little solder mask dam between the pad and the via. That's the way you should do it. Even though the vias are off pad, solder can still wick away and down the via - especially with leaded solder. Bad news if that happens.

Duane Benson
Have no fear, Underdog is here...

Via in Pad with Passive Components

Most of the via-in-pad writing I do concerns BGAs and QFNs. I do cover other parts from time to time, but the subject seems to come up most often with those packages. It is an important subject with passives too though. If you need to make your board smaller, putting vias in the pads of all of your passives may seem like a viable option to gain a lot of space. If you fill and plate over the vias, then, yes. It's a good plan. If you leave the vias open, then no. It's not.

Here are some via-in-pad guidelines:

Part type
open viaSolder mask
capped via
6mil or smaller
open via
filled and
plated over
BGA and LGA land padsBadBadBadGood
QFN, TO-(power part) thermal padsBadAcceptableMaybeGood
QFN signal padsBadBadBadGood
Passive padsBadBadBadGood

You can probably see a somewhat common theme in the table above.

Move via to the left Silver QFN vias vAll of these pictures show bad stuff. These are from the "don't ever do this" camp. Open vias on passive parts can lead to 9x13 via in pad BGA land tombstoning, poor mechanical connections, solder blobs on the back side of the board and crooked parts. Open vias on BGAs can also lead to the solder ball being sucked off of the the BGA. Bummer dude.

If you do use solder mask capped vias in a thermal pad, most manufacturers recommend the via cap be about 100 microns bigger then the via. This prior post here shows a decent example of using solder mask caps in the center thermal pad of a QFN (the rules from QFPs and DFNs are the same as for QFNs). And, I'm calling it a thermal pad in the center of the QFN, but the rules still apply of the pad is just for grounding and not for cooling.

Duane Benson
Where are we going? Planet ten
When are we leaving? Real soon


Tented QFN/QFP Via in pad

Tented vias in padHere's a pretty decent example of mask-tented vias in the thermal pad of a QFP. Most manufacturers recommend no more then 100 - 125 um wider than the via to minimize voiding and thermal insulation in cases like this. This is a reasonably inexpensive way to handle vias in the thermal pad. Sometimes though, the tents will pop open allowing solder to wick down through the via.

The mask over the center via on the right looks a little thin, so you'd want to give it an extra look over after reflow to make sure it's okay. (We'd do that here, of course)

We'd rather not see this technique on really small parts because it gets difficult for the fab house to put the mask down with enough precision. With small parts, filling and plating over the vias is the preferred technique. Well, that's always the preferred method. It's just more important with smaller parts and BGAs. This method is acceptable for most QFPs and larger QFNs though.

Duane Benson
All your via are belong to us

Via-In-Pad - Let It Slide???


Sometimes, you can get by with vias in your pads. Sometimes, but not very often. I wrote about this a while back here. The thing is, I was talking about big pads - like QFN or QFP thermal pads and stuff like that. We never like to see it and it's always a manufacturing risk at some level, but as described in the earlier post, sometimes you can just roll with it.

9x13 via in pad BGA landPretty much never with a BGA pad though. The pic on the left shows just about aTiny vias in qfp pad worst-case scenario. Very big. Very bad. Relatively very big holes anyway. This is for a .5mm pitch Bluetooth module BGA.

The vias in the image on the right worked okay with a QFP because they're really small - practically closed up - and it was lead-free solder. We still wouldn't want to see a via, even that small, in a BGA pad though. Process variations leave enough opportunity for a few of the vias to be open all the way through and even if one BGA ball gets sucked off the BGA, you're out of luck. Even if it's just partially sucked off and still connected, it's much more susceptible to cracking and things like that. (By the way, we did find a way to build the board on the left and make it work. We won't guarantee that we can make something like this work though.)

A lot of fab houses will epoxy fill your vias these days. Even micro-vias. And, yes, you should even have your micro vias filled and plated. Especially with small BGAs. It's just not worth all the risks that come along with it.

Duane Benson
We need little moles to fill those holes

Getting on My Via-In-Pad Soapbox Again

There's never enough time. There's never enough money. There's never enough room.

I certainly say those things often enough, and sometimes it's actually true. But other times, I'm just not looking in the right places. Here's a board that is pretty much plumb out of room. Everything is so tight that many of the vias have to be put in the pads. Well, maybe. Via holes in pads- how to fix-a

Take this IC footpront to the right. It needs a via to take a couple of connected pads to the other side of the pcb, but there isn't enough room between the IC and the part just below it. Naturally, the logical thing seemed to be to put the via in the pads. Unfortunately, doing so will make it difficult to get a good solder joint. The big open hole will wick solder down to the other side of the board.

Via holes in pads- how to fix-a-after At first glance there doesn't seem to be any thing to do. But upon closer examination, there is some unused space here. I'd just slide the part up a little bit as in the illustration on the left. Then move the via South a bit and connect it to the pads with a trace just long enough to accept some solder mask. The solder mask will stop the solder from chasing the via off the pad and getting sucked down.

Duane Benson
Some solder suckers sit South of Sunday

Layout 101 in 1989

I just noticed a twitter tweet about my most recent via-in-pad post: "I could understand this if it was 1989, but egads, thats layout 101 @pcbassembly A Few More Via In Pad No-no's", from mnphysicist.

I tend to agree that this is pretty basic layout advice in that post of mine. The ironic thing though, is that back in 1989, this type of problem was probably much less common than it is now. The company I worked for at the time had a number of electrical engineers and a CAD layout engineer. The electrical engineers did all of the schematic work and handed the completed schematic off to the layout specialist. The layout engineer knew all of these type of things as well as all of the FCC, UL and other regulatory issues. I think that was pretty typical back then.

Our boards rarely had problems like this. These days, though, a lot of those layout specialists, along with documentation specialists and other technical resources have unfortunately been laid off. That leaves the design engineer to do the layout as well as the schematic. We find that quite a number of these folks entered their career without a lot of training in layout. It's a different skill set than circuit design and some folks have both skills and some don't.

It also doesn't help that so many of these components are getting so much smaller and many of these designs are going into space-critical applications. This pcb had a lot of spare area to work with, but a lot of them don't.

Duane Benson
Take it to the other side

A Few More Via In Pad No-no's

Move via to the left This first footprint will result in a minimal connection at best on the pad on the left. The via takes up nearly the whole thing so the pad barely has any metal and the open via will suck the solder down in it. There was plenty of spacing below, above and to the left on this board, so the easy solution would simply be to move the via in one of those directions far enough so that it's not in the pad and there is a web of solder mask between it and the pad.

Move via and equalize pads The second image has two problems. It has a similar via in pad issue and it also has unequal pad sizes. Having a small pad on one side and a larger pad on the other side encourages tombstoning.

Unequal pad sizes will likely exhibit different amounts of surface tension in the solder, which is a cause of tombstoning. The solder paste may melt at different times on the different sized pads due to different thermal mass, again a common cause of tombstoning in small parts. Also avoid putting different width connecting traces on the two different pads. Watch for anything that may act as a heat sink on one pad and not the other - large traces, inner layers, big components nearby. Things like that.

Duane Benson
Boot Hill is six blocks that way and to the right sixty paces.