Component Packages - Let's Get Small

I've been on a bit of a package binge lately. First talking about metric vs. US passive sizes, and then a very tiny ARM Cortex M0 from Freescale.

The Freescale BGA part checks in at 1.6mm x 2mm. That's cool and I'm almost always in favor of making things as small as possible, but, as I wrote in my prior blog on the subject, it's not always possible. The 0.4mm pitch BGA is problematic unless you can spend a lot of money on the raw PC boards, or will have super high volume.

Small boardAll is not lost, though. You still can use a tiny ARM Cortex M0 part. Just not quite as tiny. That same part also comes in a 3mm x 3mm QFN package. You lose four pins (16 vs. 20) going from the BGA to the QGN, but if you can handle that, it's a very viable option that doesn't require any exotic PC board technologies.

A few years ago, QFN's were scary, but not so much any more. I've designed a few of them in using Eagle CAD. Just be sure to pay attention to the footprint. A 6 mil trace is more than small enough for a 0.5mm pitch QFN.

Duane Benson
Strive at all times to bend, fold, spindle and mutilate

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

When is an 0201 Not an 0201?

Metric vs US resistor packageI'm working on a special project here that involves some 0402 LEDs and 0201 resistors. When doing such a thing, you should always check the footprint you're using against the data sheet. When using extra small parts, like this, I recommend making a custom footprint unless the one you picked is exact, and I mean exact. There just isn't an margin for error at these geometries.

Take a look at the table on the right. The dimensions are in mm. Spot anything a bit off? Counter to most data sheets, the sizes listed in the "Type" column are metric sizes. At DigiKey, the package was listed as "0201 (0603 Metric)." I see that all the time, but for some reason, most data sheets Metric vs US resistor package Conversionshow the package name in US size while listing the dimensions in metric.

The first table was at the front of this data sheet (page 5). The second table was on page 35 - the opposite end of the data sheet.

We do occasionally get boards with metric size pads for a US size part, or vice verse. Sometimes we can make it fit, but not always. Bottom line, is to check and double check. I caught this one because the dimension .54 mm is about 21 mils, which is too small for an 0402. That, and the fact that the table doesn't list an 0201 size.

Duane Benson
Is it Bigfoot or Sasquatch?

 

Surface Mount, But Not Really

Sometimes parts labeled as surface mount aren't quite ready for prime time. I've written about this subject before (read here), and I'm going to write about it again - whether you like it or not. This time, however, I'm not talking about components that aren't up to thermal par. Today, it's about components that can take the heat, but aren't set up to be machine assembled.

Surface mount machines need a flat surface to pick on. They use small vacuum nozzles that need to seat on that flat spot. Chips, of course, are flat on top, as are most other components. Connectors, however, are often not flat on top. That doesn't leave any place for the "pick and place" machine to pick.

Single row header with pick and place padGenerally, manufacturers will place a small tab of Kapton® tape or a small snap-in plastic pad on top of the connector, giving the machine a surface to work with. You can see that in the photo on the left. Once the board has been fully assembled, the tape or plastic pad is simply removed.

Every now and then, we'll see connectors come in without that flat pick and place surface (like on the right). That means the machine can't place it, so it will have to be placed by hand. 1.25mm-Wafer-SMT-Connector

When buying your surface mount connectors, if you have a choice between a part with the tape and one without, you're better off picking the one with the tape. No offence intended to all of you humans, but machine assembly is generally preferred over human assembly.

Duane Benson
Only three more days until Mitten Tree Day!

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?

Will a Via Fit Between?

I don't know that it would be accurate to say that BGA's have ever been easy, but with 0.4mm pitch being common and 0.3mm pitch showing up, some of the older size, like a WHOLE millimeter pitch seem 0.5mm pitch padspositively spacious. With 1mm and larger ball pitch, putting a via between the pads (not in the pads) is a no-brainer.

IPC-7095B classifies 0.8mm and smaller pitch as fine-pitch. It really starts to get complicated at around that point. For example, take a 0.5mm pitch BGA. Since we're looking to put a via between the pads, the diagonal pitch is the critical measurement. In this case, it's 0.71mm (17 mil). It might immediately seem like that's plenty of room for a 6 mil via, but upon closer examination, not so much.

0.5mm pitch pads viasIPC states that a 0.5mm pitch BGA will have a nominal pad diameter of 0.3 mm. It should be a non-soldermask defined pad, which will add about 0.07 mm to the pad diameter. That gives 0.44 mm total pad diameter. The radius is 0.22 mm (8 mil). Take that out of the 0.35 mm (14 mil) you have to work with and you're not left with much space.

If your fab house can do 3 mil trace and space, you will end up with enough room for a 0.06mm (5 mil) via, including annular ring. That's not much space. Most designers, at that point, will seriously consider putting the via in the land pad and having it filled and plated over. You can't leave the via open or un plated.

Duane Benson
All was in chaos, 'till Euclid arose and made order

 

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

Beagle CAD paw prints

Unfortunately, I can't generically hand out Eagle CAD QFN footprints without knowing the specific part, but I can illustrate the areas I initially had difficulty with. All of the traps that used to get me seem blindingly obvious now, but they weren't when I first tried to make my own library parts.

The very first thing I would recommend is to make your own library file. When I started in with my own parts, I would just add them to an existing library. For example, I'd put a new Microchip PIC processor into the "microchip.lbr" library. It seemed the logical choice because there are other similar parts to start with. But, when it's time to upgrade, migration of those custom parts becomes a nightmare. So, now all of my custom parts go into "dfb-parts.lbr."

Eagle footprint menu barSpeaking of modifying existing parts, another recommendation I have is, except for parts where the package footprint is EXACTLY the same, start from scratch with the package footprint.

The schematic symbol is easier to reuse - just make sure you have the right pins in the right place - but subtle differences in the copper footprint can have a big difference at the assembly stage.

Datasheet footprint page land patternI also don't try to hand size and hand position the pads on the silk screen. Start by just putting a pad in the footprint area. The use the Properties/Info button (the big "i") and use the dimensions given in the data sheet to enter the size and position by number.

Look for the "recommended land pattern" or similar diagram toward the end of the component datasheet. Entering the numbers in the Properties/Info box will bypass any position precision issues. Just make sure that you use the right units (i.e. metric to metric).

Stay tuned for the next installment.

Duane Benson
World to end at 9:30. Details at 11:00