Screaming Circuits: Via in Pad


I've been pretty occupied with the upcoming Embedded Systems Conference in Boston. The exhibition is next week on Tuesday, the 21st and Wednesday the 22nd. Screaming Circuits will be in booth 809. Stop by if you happen to be at the show.

In any case, I've been pretty much wrapped up in show preparation so I haven't had much time for original writing here. That being the case, I'm going to play an old TV sit-com trick and just select some old, but good, content to re-run.

And, there you go.

Duane Benson
Hide Wally Bee. Andre is back and he's got a fly swatter


QFP lots of vias QFP lots of vias stencil I've heard of vias in pads, but vias in paste aren't so common. Here's a QFP footprint with a lot of thermal vias in the center pad area. I'm guessing all of those vias are necessary for heat removal, but they sure aren't friendly to solder paste as created.

Further, the solder paste stencil had good intentions too, but ended up inverted in practice. It's good to keep paste off the vias. Even inverted though, I'm not sure how the stencil would have worked. You can't have dots of stainless steel just floating out there. The vias should be capped, or better yet, filled and plated over. The proper way to create the stencil layer would be with a cross hatch as shown in the third image.Good QFN stencil b

Capping (also called tenting) vias with solder mask used to be a pretty common practice. You'd put solder mask over the via out to about 100 microns bigger than the via on the component side. Some people would put the cap on the back side, but that still leaves a lot of volume for solder to wick down into.

The capping with mask practice is kind of falling out of favor these days. For one, if the mask is too thick, it can end up lifting the part up a bit. More likely though, the caps can break, leaving an open hole for solder mask to wick down.

The optimal method is to have the vias filled and plated over at the board house. There are some thermally conductive materials that do just about as good at heat transfer as would the open via.

Duane Benson
Solder paste is people! It's people!

Vias between BGA pads

I ran across a question posted on the Xilinx forum recently about whether vias in BGA pads needed to be capped, as suggested in my post about that subject. We do recommend that the vias be filled and capped with copper in BGA pads. There really isn't enough land surface to not plug the via holes. Some people are okay with an unfilled microvia that's only one layer deep, but even that can lead to excessive voiding.

If you've got a good board house, you may be just fine with vias between to pads down to a BGA ball pitch of 0.5mm (20 mil). Just make sure that there is solder mask between the land pad and the via as is noted in the illustration below.

BGA on HASL close with vias between pads

Duane Benson
Consider that two wrongs never make a right... but that three do.

Another Via-in-Pad reason

Just the other day - No not that one. The other one - I was reading through some of the open source BB Empty pcb via in connector pads Beagleboard information again and I came across an interesting tid bit. In one of the early revisions, they had some issues with SMT connectors ripping off the board. The pads detached from the board. I know that's not  a common issue, but it does happen.

Their solution was to put vias in the pads to strengthen the connection between the pads and the PCB. I hadn't thought of that, but it makes perfect sense. Note the four dimples in each of the pads on the audio connector footprint in this image. Also note that they are small and closed off.

If you've got some concern about losing your SMT connectors, you might want to consider the via-in-pad solution. Do, please, cap or plug them though.

Duane Benson
Who plays pinochle on your snout?

How to Fill a Via

We here at Screaming Circuits keep telling people to fill and plate over vias in BGA pads. The same goes for small passives too, like 0402s and 0201s. As I closed in this post, best option is to fill and plate over. Bigger parts can use some of the solder mask techniques, but BGAs and tiny passives really do require filled and plated vias.

The question of the day, however, is: "Just how do I get those vias filled?" Here again is another place where our old Gerber file format falls a little short.

Filled vias 

Copper filled via on the left and conductive epoxy filled on the right.

There are quite a number of different methods for filling vias: Copper plugs, copper plate, surface material (i.e.  HASL), conductive epoxy, non-conductive epoxy. Maybe others. But, the Gerbers don't have a method for specifying this.

So here's what you do. 1) You need to contact your fab house to determine what techniques they have available and what they recommend for your fab project. 2) You have to create a set of fab drawings or special instructions that point out which vias need to be filled and with what material.

Duane Benson
Maybe raspberry jelly filling?

Via in pad - tenting the bottom side

BGA via in pad bottom via capSpeaking of vias in pads, here's a reason we're not terribly fond of the technique of using solder mask to tent the bottom side of a via in a BGA pad.

As I mentioned in my last post, capping the bottom of the via with soldermask is sometimes an acceptable method for dealing with a via in pad. It's not a desirable method, but it does sometimes work. However, with BGAs, the top-open via can still wick solder down to fill the space. At the very least, you will end up with a hefty void in the BGA solder ball. At worst, you will end up with an open, as illustrated here.

Best option: Fill and plate over the via.

Duane Benson
Does cheap mass production = this perfect day?

Large Via In Pad

Large QFN vias I haven't written about via in pad in a while, but the issue hasn't quite gone away yet. This particular QFN, to the left, has the vias tented, which is good. However, it could be better. If you look close, you'll see that they're tented on the bottom of the board with solder mask.

Tenting on the bottom will usually prevent solder spillage out on the back side of the PCB, but with vias this large, the solder will probably flow down into the space, leaving quite a bit of voiding under the part. Sometimes outgassing will pop open the little tents too causing the spillage. And with immersion silver boards, outgassing can cause corrosion in the vias if you have the bottom tented and the top also sealed - like by the part.

If it's a low speed, low temperature QFN that just needs a little ground connection to the center pad, that voiding might not matter. But, in most cases with QFNs, you need minimal voiding for thermal or noise reasons.

The best option for manufactureability is always to have the vias filled and plated over at the board house, but that can be expensive. If you are going to tent with solder mask, this next image illustrates the three Soldermasked vias for blog b ways to do it.

A is the best: a cap on the component side about 100 to 125 microns bigger than the via. B, a larger cap on the component side, or C, a cap on the bottom, will also work but both come with a greater risk of excessive voiding.

Duane Benson
Do solder mask tents need a rain fly?
In Oregon - probably yes.

Crooked Components

I was looking at two different PCBs recently; one assembled here at Screaming Circuits, and one, a PC graphics card assembled someplace else in the world. In both cases, a crooked component caught my eye. The graphics card, at least, would have done a passable job of meeting IPC-A-610 Class II, but in both cases, the offset was enough to inspire me to take a closer look and write this blog post.

On the graphics card, the particular component was an SMT inductor. I've been having some issues with the card and when I had it out of the PC, I saw that inductor. With further examination, I found a lot of other crooked components. My off-the-cuff conclusion was that the manufacturing workmanship was poor, therefore I shouldn't be surprised that the card was having issues, and perhaps I should look for a different brand for my next purchase. Again, everything would likely have met IPC Class II, but perception is close enough to reality and that manufacturer has probably lost a customer.

SD land with hole In the case here at Screaming Circuits, only the one component, an SMT SD card socket, was crooked. In addition to the signal pads, this socket has four large SMT pads, one on each corner, for mechanical connection to the PCB. One of those four pads on this PCB has a big hole in it. Not just a little 10 mil via in the pad, but a either a really, big via or a bolt hole. The unequal surface tension in the solder, caused by that pad being cut in half, caused the connector to twist a bit.

Yes, in a prototype world, we made it work, but it caught our attention here and if such a thing went into final manufacturing, it might very well catch a customer's attention and elicit the same response I had to the graphics card. It will work okay and would probably stay secure on the board (maybe), but it's not good practice and it looks wrong and wrong looks can cause customers to go elsewhere. Yes, function is key, but if form chases customers away, then function never gets a chance to matter.

Duane Benson
We'll keep the robots in line
You keep the PCB in line

Toyota is as Toyota does

Everyone else seems to be writing about Toyota sudden acceleration problems, so I should probably do that too.

Or should I? Personally, I have absolutely no solid information about what's going on with Toyota cars. There's an awful lot written, much of if by people that also don't have any real information on the subject. Here's what I do know though:

  • Some people (some with actual knowledge and some without) are speculating that electronics might have something to do with the problems.

That's about all I know relative to the specific concerns. On the soft side, I do know that people tend to pick on the big guy. Funny how none of this was big news until Toyota became the #1 car maker in the world. Coincidence? Maybe. Maybe not. I also know that in any system there are gobs of places where LED via-in-padissues can lead to failures. Of course, to counter that, I know that good, well thought out design - both in the hardware and the software, can produce a quality product that will keep working. In summary, I really don'tSilk on pad know anything about the Toyota issues.

However, any time some sort of actual or potential technical problem makes big news, it's not a bad idea for those that design and build things to take a step back and evaluate our design practices. I've got software in my past, so I'd have to suggest a good solid code review, if you don't already do one, but today, I'm talking about hardware so I'll sample just a few things to double check.

  • Those pesky land patterns: Does the land pattern fit the part? Will the copper area and stencil opening allow for a good solid IPC-passing solder joint? It's so common (as you well know if you read here regularly) to re use or create new CAD part foot prints. Make sure the foot print, stencil, mask and silk layers fit properly.
  • Vias in pads: Plug them and plate over them when using small parts. If the solder surface is big enough, like with a power component, you might be able to just cap them, but don't leave the vias open. In some cases, you may be able to leave very tiny vias open on thermal pads, but it's best never to.
  • Thermal mass: This is important both for operation and for assembly. If you've got components that sink and/or generate lots of heat, make sure there is enough air flow to cool them during operation and make sure that the assembly house can build it. Put a couple of high thermal mass parts too close together and an otherwise perfect PCB assembly may end up with some cold solder joints or damaged components that later come back to bite you or your customers.

There are lot's of other things to check out too, but those three are just some of the more common traps to keep tabs on.

Duane Benson
I don't have a Toy Yoda. If I did, I'd sell in on eBay.

Inverted QFN Land Pattern

Have you ever experienced the heartbreak of inverted land pattern? It's not supposed to happen, but every now Inverted QFN land pattern 2and then, it does. Maybe something happened when creating a custom footprint. Maybe, somehow it got inverted in the CAD software and then placed on the wrong surface layer.

Maybe it was a subliminal attempt to make up for those giant open vias in the thermal pad. Who knows. But, it happened, so now what?

You could re-spin the whole board. Ugh. That's, like, wasteful and stuff. Certainly, if this is a production build, you'll have to re-spin. For some prototype applications - like if it's a high frequency or RF thingy, you may very well have to get a new set of PCBs fabbed up too.Inverted QFN land pattern

But, sometimes in the prototype world, you may be able to salvage the board run. We used to do stuff like this all the time with  thru-hole parts - need an extra chip, just dead bug hang it on up there. 

Flip the chip over and use some small gauge wire - maybe wire-wrap wire - and hand wire to the upside down chip. Gluing it down first may be helpful. Just keep in mind that since the thermal pad isn't soldered to the board, you will lose some of your thermal performance. Maybe solder a small heat sink on it or something. And don't forget to wire that pad to ground too (if it's supposed to be grounded).

Duane Benson
Just put it on the seventh surface of your tesseract and it will fit right.