Screaming Circuits: Parts Form-factors

Using Package on Package (POP)

Back in August of 2009, we at Screaming Circuits assembled our first package on package chip set. We did a number of test components first to tune the process and then built up some Beagleboards. We've done a few more since then. It's not yet a high-demand item, but it is getting more popular.

Amkor POP sm At the ESC (Embedded Systems Conference) last week, we had a number of folks stop by our booth and ask about how to use the part. The OMAP processor from Ti that comes in a POP form factor is a great high-performance part, but I think a lot of designers are still intimidated by it. Really, though, there's nothing special about designing with POP.

It's a 0.4mm pitch BGA and that gives some challenges with escape routing and PCB masking, but those are standard BGA-type issues. For escape routing, go to, download the beagleboard reference manual. They have their version of the escape routing in the book. And, check out this post for some advice on the BGA footprint.

That's pretty much all there is to it. The memory chip just plops on top of it, so as a designer, you don't have to worry about that. Just do a good 0.4mm pitch BGA layout and your POP will come out just fine.

Duane Benson
Does Kellogg make Raspberry flavored Package on Package Tarts?

Castellated / Half-Vias, parts 2 - 255

I've written about the Castellated / half-via mounting system a couple of times in the past. Now I can't seem to avoid them. I'm seeing them everywhere. The GPS I recently wrote about, low noise amplifiers, POL power modules, frequency synthesizers, VCOs...

When did this become the package of the day? I haven't even seen what IPC has to say about it yet but these things are all over the place. Our engineers and assembly folks are cool with it. It's not that tough to build, fortunately. But, as I saw with the ublox part I wrote about, there are new design issues to contend with.

I can certainly see the advantages of the package. The half via can allow for a good solid fillet providing good mechanical connection. They're typically a pcb-type substrate so the coefficient of expansion and flex strengths should be similar to the underlying pcb. On the other hand, like with an LGA the low profile after soldering will tend to exacerbate any expansion or flex risks.

Duane Benson
Once in a dream
Far beyond these castellated walls...

Castellated / Half-Vias

Castellated Modules with castellated mounting holes are showing up more and more these days. I've also heard it called a "half-via" setup. Both seem to fit. The copper mounting pads on the bottom of the module's little PCB wrap up the side of the PCB with a half-via. Thus, the name "half-via." If looked at from the base, the edge does look a bit like the outline of the top of a castle wall, so that makes sense too.

UBlox paste layer Whatever. The name isn't that important. There are a few things that are important though, such as the land pattern and the solder deposition. I hadn't heard any special requirements for using this type of part until recently when I ran across a GPS receiver module from ublox. What they say is that you need more solder on the outside of the pad, than on the underside of the pad, so that it can properly wet up the half-via. That makes perfect sense. There are probably multiple ways of doing this, but you can see their take on it in the image here on the right that came from their data sheet.

Obviously, follow the datasheet that comes with your specific part, but if you don't have any official guidance and can't get word from your part manufacturer's applications engineers, you might take a hint from this method. The copper land is just a standard rectangle, as is the solder mask. The paste layer, however, is not. It's wider toward the outside of the part. This will help create a proper fillet up the via while reducing the chance of solder balls and other messy things that can happen when you have too much solder under a part.

Duane Benson

Foot Prints

I write a fair amount about component foot prints / land patterns / CAD library components - whatever you call them. What are you supposed to call them anyway? I've heard them called all three of those things and a few other names as well. Seems like a good case for some terminology standardization. Or maybe I just need to do some more research on that specific subject.

PCB123 cut out capture I'm curious as to how common it is that a designer needs to create a custom footprint for a part. I seem to have to create at least one for every project I do and I rarely use new parts or complex packages. Of course, I don't use CAD packages that cost gobs of money either. Just Sunstone's PCB123 and Cadsoft Eagle. PCB123 has all of the NXP parts so that's good, but it's not just the big components that get you.Eagle library design

In a board I 'm just finishing up - 22 BOM line items, I had to make a custom library part for a crystal and modify a library part for my microcontroller. I had to create some custom footprints for a couple of connectors too, but half way through the layout, I upgraded Eagle and discovered that someone else had just done the same thing I needed for the same connector, and uploaded it to the Eagle site, so I used their work. Hopefully I haven't made any of the mistakes I always write about.

I really am curious as to how many designs typically require at least one custom footprint and how many custom footprints per design would be a typical rule of thumb.

Duane Benson

Parts Too Close For Comfort

Another tale from the sometimes kind of kooky world of prototypes. I think what happened here is that the board was originally laid out for caps with a smaller voltage rating (or even a smaller capacitance value). We're seeing things like this more often these days due to availability issues. The part gets swapped at the last minute because the exact one is out of stock. Operationally, it won't hurt and if the board had been laid out with more space, this wouldn't have caused any issues at all. Of course, then, it may not have fit in the box.

Caps interfere with eachother

The moral of this story is that with last-minute swaps, don't forget to double check things like the part package and board spacing. This board works fine, but it won't be meeting up with any IPC standards as long as these parts are like this.

Duane Benson
Parallel parking is hard. I'd much rather diagonal park.

Pitch Switching

I recently started reading the magazine Chip Scale Review. It's a different take on things than I'm used to. Most of what I read for work is in the engineering and assembly realm, but this one goes back to the component packaging. I think it will be a good one in terms of keeping up on what sorts of things we'll need to be assembling in the future.

So far, I haven't seen anything really scary in it. There is talk of .3mm pitch BGAs, but those aren't totally new. I'm not sure if we've done any .3mm pitch before, but we've been doing .5mm for years and have done plenty of .4mm pitch as well, even in package-on-package (POP) forms.

Pitch switching adapter Speaking of really fine pitch BGAs and CSP type things, one topic I found interesting has to do with pitch switching adapters. It's basically a small PCB platform that has an underside footprint of a 1mm or 1.27mm pitch BGA and a land pattern on top for a fine pitch BGA. It has solder balls on the bottom, so once sandwiched together, it's treated just like a big BGA for assembly purposes. [Credit where credit is due: The image I'm using came from the Aries Electric web site.]

Such a part can negate the need to re-spin the PCB if your big part is updated and replaced in a new fine-pitch form-factor. (Although, personally, I can only imagine that if the chip is rev'ed, there will be some other change that has to be made to go along with it). The theory is, that if you've got a really expensive design, this might be a viable option allowing you to upgrade without a relayout.

Certainly though, at the very least, this could allow you use some newer fancy chips without having to resort to filled micro vias and tiny trace & space advanced (expensive) pcbs. Could be quite handy and same some money.

Duane Benson
Platform shoes are back!

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...

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

Pin BGA Interconnects

My post "Speaking of Art in the Process" used a photo of a point of load power module as an example. The specifics aren't really relevant to this post though, but a commenter by the name of "Me" asked what type of pins those are connecting the module to the main PCB.

"Do you know where to get those pins to attach two boards like that?
I mean do they sell just the pin for example on digikey and give it a name, or is it just wire.
Can't see if they are pins with a lip to lift board to a set height."

Module assembly from side Module assembly several This part came with the pins already on so I don't have a specific part number for the interconnect pins. I have some underside photos here that give a better view. They are basically solder-type terminal pins with a solder washer and BGA ball on one side (to attach to the main PCB) and either a press-fit or solder type side to affix to the module PCB.

I wasn't able to find this exact part on DigiKey or Mouser. Vector sells the solder washers and lots of interconnect pins of this sort, so they may be able to steer you to them with a phone call. This board uses the BGA style, but we've seen other POL modules of a similar type with thru-hole solder pins too. DigiKey has lots like that. Here's one example of some thru-hole terminal pins from Mil-Max. You could use the solder-washers (like a T124 from Vector) to put some space between the module and the PCB.

Duane Benson

QFN Land Pattern Mix-Up

Another QFN oopsie here. The QFN looks good and the stencil cut-outs look good. The mask, though, as shown in the middle, is not good. In general, you shouldn't put mask on the QFN land pad except to cover up open vias.

The QFN center thermal pad for this part should be free of solder mask. The stencil does give a good amount of paste -Mask and stencil issues roughly 50% coverage, maybe a little more. That's the way we like it. But, with the mask on the board, there will be too much solder and too much with nothing to stick to. It will either flow to the small metal areas and raise the QFN up so the sides don't solder or the excess solder may turn into solder balls and short something out.

There are some cases where it's okay to only expose the metal in small areas of the QFN thermal pad (see here), but if you do that, the stencil has to match the pattern. Otherwise, like in yesterday's post, you'll probably end up with a gloppy mess.

Duane Benson
That's the way aha aha your pcbs like it aha aha