0.4mm Pitch BGA is Awesome

I recently had a conversation with a friend about 0.4mm pitch BGAs. The specific part is the Freescale FreescaleKL03KL03 ARM Coretex-M0+ microcontroller in a 1.6mm x 2mm, 04.mm pitch package. That's a 20 ball wafer scale BGA form factor.

I don't have an actual part to photograph next to a grain of sand, but trust me (or don't), it's really small.

Ti 0.44 pitch dimensionsThe challenge, and the reason I suggested a QFN form factor instead, is the costs
involved. If you have the extra budget money for more expensive PC boards, then go ahead and use this form factor. You probably won't be able to use this package in cost constrained situations.

The simple reason is that you can't escape route the inner six pins without using super small vias between pads, or in pads and filled and plated over. The page on the left is from a Ti doc, but any variations in geometry will be minor.

You can see that you can't put a trace between the pads. Maybe a 2 mil trace, but maybe not. There just isn't much room. The recommended method is to put micro vias in the pads and have them filled and plated over at the board fab house. Never put a via in a micro BGA pad unless it's filled, plated over, and flat.

Duane Benson
There are more things in heaven and earth, Horatio, 
Than are dreamt of in your philosophy.
But open vias in pads aren't one of them

VLV - Very Large Vias

I recently received a question over on Twitter. Tomaž Šolc, AKA avian2 asked:

"@pcbassembly What is your opinion on the "one big plated drill in QFN ground pad" pattern? pic.twitter.com/M9ZLftpuo0"

From Avian2 Ban_N62IEAAm3acI answered back: "Bad for machine assembly, okay for hand assembly." That's definitely true, but it's worthy of a bit more explanation. Here's the photo avian2 included along with the question. We're looking at the side opposite of where the QFNs are mounted. The two big openings in the square gold pads are the big vias (plated drill).

This is often done when hand soldering QFNs. Somehow you get the little pins on the outside edge of the QFN soldered down. Then you turn the board over and poke your soldering iron into the big opening to solder the pad down.

Generally, there wouldn't be any reason to do this with machine assembly, as we do here in our plant. You put a number of small vias, cap them, and segment the solder paste layer (refer to this post and this post). Thus, we would never recommend using big vias like this for machine assembly.

However, I can envision some situations that might call for this. First, there's the hand solder method I mentioned above. Next, there may be some very specific need to expose a lot of the pad to open air for cooling. In general, this is not the best way to get cooling, but maybe in some special case. Third, perhaps you need access to the pad as a test point and don't have enough room to get access any other way.

You wouldn't do any of those three things in a production environment, but in a prototype world, sometimes things happen differently.

Duane Benson
Hurray! Only one day until Mitten Tree Day!

Pads on Ground Plane

Pour-no thermalGenerally, small pads for passive parts are connected  with a single PCB trace of equal size to each pad. That's the right way to do it.

However, sometimes, circumstances dictate a little different approach. The illustration on the upper right here shows something of a worst-case. This is for a snubber (resistor, capacitor pair) between two power planes.

A couple of things will likely happen. The power plane will act as a heat sink, preventing the solder paste on one side from melting, resulting in a poor connection. Or, the unequal melting could lead to surface tension pulling the part up, causing tombstoning.

Pour-with thermalMost designers are aware of that, but sometimes, thermals will be deliberately turned off to allow for better current capacity to and from the large power Mosfets (not shown). If that's the case, make sure that you can turn the thermals (see image on loer right) on or off by the part, rather than just by the plane.

Duane Benson
The rain falls mostly on the ground plane due to static attraction

Super Small Via In Pad

Via in pad is an old issue that still pops up now and then. Our standard answer hasn't changed: No open vias in pads. But one of the questions we get related to the subject is: "What if we make the vias really small?"

Beagleboard U6 viasLogically, that makes sense. In fact, in some cases, the via is so small that it's essentially closed. If it's so small that it really is closed, then it's not an open via. But look close - if it's closed with solder, that solder may melt during reflow leading to an open via.

The images here show some pretty small vias. I believe they're 0.3 mm in diameter.

Beagleboard vias back sideIn the first picture, on the left, it appears that the vias are open. They aren't though. This board (an unstuffed Beagleboard) uses soldermask on the back side of the PCB to close off the vias, as shown in the image on the right.

Our recommended method (se more detail here and here) is to plug the via with copper or epoxy and have it plated over at the board fab house. Next, we'd recommend via caps on the component side. FInally, capping the back side with soldermask, like this example can work, but it comes with the risk of voids. The via caps and also pop open, leading to an open via.

Duane Benson
No more open vias-in-pad, I mean it!
Anybody want a peanit?

Push-me Pull-you LEDs

I may never get tired of talking about LED and diode polarities. It's so much fun. Not long ago, I wrote about two LEDs from the same manufacturer, marked with opposite polarities. I recently ran into another one, but at least this one tells you on the same datasheet. This image is an actual unmodified clip from the datasheet.

LED confusing polarityI can't for the life of me understand why this would be done on purpose. I could maybe understand is one was designed in a different building, but it couldn't have been too hard for someone to say: "Hey - wait a minute..." before sending these things off to manufacturing.

Of course, maybe they built a million before noticing and then just decided it would be easier to change the datasheet. Regardless, it's kind of nuts in my opinion.

The other thing here is that, while you can generally get away with the indicators "+/-" on an LED, you can't with all diodes. Thin Zener and TVS.

Duane Benson
Matter + antimatter makes what?
Does it really matter?
Does anybody really know what time it is?

LEDs - Seeing Double

Dual LEDLike I do so often, I'm being a bit redundant. While I'm all for stamping out and eliminating redundancy, this is redundancy with a purpose (not a porpoise). Not long ago, in a galaxy not far away, I blogged about annoyances in surface mount diode polarity markings. You can read that here.

I'll wait.

Messy isn't it? Well, after reading that blog, someone asked me about dual diodes. For some reason, I can't seem to find the page covering dual diodes in my IPC book, but that's not the important part. What is important is the way the diodes are marked on the PC board.

We do ask for centroid data which, in theory, contains the component rotation. That would be cool except that we find that far too often, the zero degree orientation (and the rotation from that) differs from the standard. That, and there are seemingly half a dozen or so standards.

Since LEDs don't work too well backwards, we really would like to see everything marked in a non-ambiguous way in silk screen (or in an assembly drawing if you don't have silk screen). A "cathode bar" won't work because it could be a bar indicating the cathode or negative. The cathode isn't always negative, especially when looking at TVS or Zener diodes.

Mimicking the diode markation pattern printed on the part may not be secure either. Read that article I linked to right at the start of this blog. What if you put silkscreen down to match one of those LEDs but ended up buying the other one? That's exactly what I did myself. Trust me. It just leads to disappointment and possible soldering iron induced finger burns.

So what is the answer, and why am I talking about single LEDs and TVS diodes when the blog is about dual LEDs? Well, the answer is the same. The best way to communicate the desired polarity of an LED or any kind of diode is with a mini version of the schematic symbol. It doesn't matter if it's a single LED, dual LED, Schottky, Zener or what ever kind of diode. The schematic symbol is the clearest way to go.

Led marking

The diode footprint has the manufacturer's polarity marking, but I don't care. I still put the diode schematic symbol next to it. If you don't have room for silk screen, put it in an assembly drawing. You won't regret it.

Duane Benson
And they called him Flipper...

More cautionary tails

I recently wrote about the horrors of LED marking variations. Unfortunately, LEDs aren't the only place to find inconsistencies in our world. Another part to keep a close eye on is the ubiquitous three-terminal voltage regulator. For just short of a million years, pretty much all three-terminal voltage regulators followed the 78XX convention. Lm7805 convention
It is not completely universal though. Is saying "completely universal" repetitive and redundant? There are some regulators that divert from convention in thru-hole and in SMT form-factors. Despite the overwhelming prevalence of the 74XX pin-out, you may find some parts that dispense with convention and can bite.

Take the LM1085, low drop out (LDO) regulator, for example. It looks, for all intents and purposes, to be a standard TO-220 or TO-263 three-pin regulator. You'd look at it and assume that it's a direct replacement for any old 75XX series. But, rather than In-Ground-Out, it's pinned as Ground-Out-In. The LM1117T is the same.

Mismatched SOT-223You might think: "Of course, it's different, the part numbering doesn't follow the 74XX number scheme." That sounds logical until you look at the LM2940. It follows the 74XX pin convention, as does the MIC39100. It's not the LDO specification that justifies change the pin-out either. The LM2940 is also an LDO.

Unlike the LED polarity issue, this one isn't as likely to bite you during assembly. The SMT regulators can only go onto the board one way. If your CAD library footprint is correct, it will be assembled correctly. The thru-hole can be easily reversed though if your silk-screen isn't clear. Marking pin 1 on the board (and checking the CAD footprint) is the recommended approach.

Duane Benson
In the land of the insane, only the sane are crazy.

How NOT to mark a diode

A while back, I wrote about ambiguity in the markings on electrolytic capacitors. In doing that, I cobbled together a little image to illustrate how surface mount electrolytics are marked. Take a look at the image below:

Capacitors

Note how I have illustrations showing how tantalum and metal can electrolytic capacitors are marked. Further note, that I have the capacitor schematic symbol there too. Finally, note that all three are oriented in the same direction. I have the plus side on the left and the negative side on the right.

Now for comparison, I have two nearly but not quite identical 0805 SMT LEDs in the following photo. Look at the photo of the two LEDs below. I did not alter this image in any way. The mark on the LED image could be interpreted either way. The bump could be seen as pointing toward the cathode, since it is the cathode mark. Or, The line could be on the side of the cathode. That would make sense because the line on the schematic symbol represents the cathode.

There's one final thing to look at - wait for the punchline:

Backwards markings

The punchline is that the  cathode is on the left on both of these LEDs in the photo. I have empirically determined that to be the case, both by putting them on a board and by subjecting them to a diode checker. Punchline number two is that both are correct according to their respective datasheets. The following excerpts from their respective data sheets shows the problem.Reverse marked LEDs

And, drum-roll please ... The third punchline is that both of these parts are from the same manufacturer!

If your board uses SMT LEDs, send the datasheet with your assembly order. Include it as a PDF in your files set. It would also behoove you to double check your CAD library footprint against your specific part number datasheet. IPC says the cathode is pin-one and pin-one zero degree orientation is with pin-one to the left.

Duane Benson

Forward, the LED pick and place
Was there a machine dismayed?
Not tho' the engineers knew
Someone had blundered
Cathodes to right of them
Cathodes to left of them
Cathodes behind them
And I cannot reason why

More Beagle CAD Paws

Continuing on from my last post...

As I said, I do everything I can to avoid re-using the package footprint when adding the the parts library in Eagle CAD. The schematic symbol can be a different story though. It still takes a lot of caution, but it's less risky (in my opinion) than reusing the package footprint.

Eagle version 6 made some improvements in the way copy and paste works. It's still a little different from your typical word processor, but it's not that difficult.

Eagle footprint menu bar 3 buttonsBut before I get to that, I want to mention one item that caused me a fair amount of confusion early on. And that's the way all of this fits together. There are three buttons you will need to worry about. From left to right in the green oval are; the device, the package footprint, and the schematic symbol. In my last post, I pointed out the package footprint and today I'm talking about the schematic symbol.

Really, you only build the footprint and the schematic symbol. Then you connect the two up to create the devices. And, you can build the footprint or schematic symbol in either order, but you have to have them both before the last step (the icon in the green oval with four little AND gates).

If you're using a chip that comes in a couple of different packages (e.g. DIP28, SOIC28, TSSOP28) you most likely only need to make one schematic symbol. You can make the multiple footprints and connect them up in the device section as different variants of the same part.

There are a few exceptions though. Sometimes QFN, QFP or BGA parts will have a few extra pins. In those cases, it may be better to create a different schematic symbol.

Duane Benson
This solder paste stencil glows blue when goblins are around

Speaking of Reference Designators...

In my prior post about BOMs, I gave a few examples of reference designator formats in the BOM. BOMs are a common item that have standards but no standards as are reference designators. There are actually a number of standards covering reference designators, but I still find people referring to documents published in the 1970's!

Some aspects are pretty obvious. They are a code letter followed by a sequential number. Each and every placement on the PCB has to have a unique reference designator. The code letters are somewhat standardized, in practice. Some vary based on the particular user. Pretty much everyone uses "R" for resistor and "C" for capacitor. The mostly standard designator for an integrated circuit chip is "U", although I've seen "IC" used enough times. Crystals and oscillators are supposed to be "Y", but I've also seen "X", "Q" and "U" used. Check this page over at Mentor Graphics for their recommendations.

Things start to get sticky when people have more than ten of a given type of component or when putting together a family panel (several different designs on the same PCB panel). Let's say you have 15 resistors. You could designate them as R1, R2, R3 - R15. But maybe you're a little OCD and you want them to all have two digits. In that case, you might have R01, R02, R03 - R15. To a human, "R1" and "R01" might very well be exactly the same thing. But to a surface mount robot, they are two different things. The robot would be happy with R01, R02, R3, R03, R4... but that could cause problems for a human reworking or maintaining the circuit later. It's best to be consistent. Basically, the assembly systems see reference designators as text items, not numerics.

Let's take the example of a family panel. One board has C1 and C2 are a 10uf, 24V tantalum cap. The other board has C1 as a .01uf, 50V ceramic and C2 as a 220uf 24V metal can electrolytic. If you were having them built separately, there wouldn't be any problems, but the two of those on a surface mount machine in a family panel and you will have bad news.

First you could avoid running your boards as family panels. That's not always practical though. Second, you could just start numbering the second design where the first one stops: design one: R1, R2, R3, R4. Design two: R5, R6, R7, R8. That makes a lot of sense for a family panel. Just treat it all like one big design. That can get confusing though if you later run them individually or need to do some rework. Some poor tech could go crazy looking for R1 on design two. Even worse would be: design on: R1, R3, R7. Design two: R2, R4, R5, R8. Again, fine as a family but darn confusing when separated.

Personally, I would probably go with something like: design one: R101, R102, R103. Design two: R201, R202, R203.

Duane Benson
You know the nearer your designator, the more you're silk screening away