Screaming Circuits: CAD Parts Libraries


CAD Data Files

I've spent a fair amount of time researching and writing about the centroid file and about CAD library footprints. One of the challenges in this industry is that somethings that are "standard" really aren't all that standard. That's why we emphasize following IPC guidelines when creating library components.

Well, a few things have changed since we started doing this a decade ago. For one, some of the enhanced manufacturing file formats (as opposed to the 1970's vintage Gerber format) have become more prevelent. Those new formats are a very good thing.

Most CAD packages can now output either ASCII formatted CAD data or ODB++ format data. Those file formats have all of the data that would otherwise be found in the centroid and Gerber files. They also have more accurate data. If you can get one of those formats out, go ahead and send it to us. We can also take plain old Eagle CAD .brd files. If in doubt send one of these newer files along with the centroid and Gerbers. We'll use the file with the best data and, we may be able to simplify the file preparation Centroid snippet rot optyou have to do with future jobs.

And speaking of the Centroid, don't worry so much about the rotation column in the Centroid file. You can consider rotation to be optional now. You don't need to check the rotation, nor do you need to remove it.

Duane Benson
Who will win? Godzilla or Centroid? Maybe the Smog Monster?

 

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 if 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...

Creating a QFN Footprint - the center pad

I've written bits and pieces about creating footprints in Eagle and a lot about what the QFN solder paste layer should look like, so maybe it's time to connect the two dots. I'm using Eagle CAD here, so your process will likely be different unless you're using Eagle, but the concept should be the same. This process takes place in the package section of the Library editor. I'm assuming that you're already part way through and just need to put in the center pad.

Center pad Center pad position and sizeFirst, add the center pad to your QFN using the "Smd" tool and set the size based on the recommended pad size specified in your part datasheet.

The center of the pad should be located at 0,0 unless you have a QFN with odd shaped or multiple pads.

Make sure you un check the "Cream" box in the lower left corner as we'll be doing that manually.

After the pad is there and sized right, you need to add in the cream (solder paste) layer. You'll be drawing the cut-outs in the stencil with the rectangle tool. Use the rectangle tool to draw the stencil cut-outs. Set the rectangle to the "Cream" layer. In my installation of Eagle, the Cream layer defaults to layer 31.

Most parts should get 50 - 75% paste coverage to prevent floating (read this for more details). If your Stencil rectangle Stencil rectangle position and sizepart datasheet gives a specific number, use that. However, in my experience, most part datasheets just show a wide open stencil with 100% paste coverage. Unless you have good reason, don't do that.

Without any specific guidance, I usually aim for about 70%. In high volume manufacturing situations, the manufacturing engineers will likely spend time tweaking the coverage, but it'll be close and for a prototype, 70% is a good number.

Duane Benson

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

Let's Get Small, as in 0.3mm

Not long ago, I wrote about a 0.3mm pitch wafer scale BGA we received and were asked to place. The gist of that article was that those parts are very small and we d0n't yet have a process that we feel will give the quality, reliability and consistency that we want to deliver. That means officially, we don't, at the moment, support that form-factor.

However, as it turned out, we went ahead and built it and the x-rays all said it looked good. Whew! We still don't officially support it, but we're working on it. If you have one of these things, you can always give us a call and see if it's something our manufacturing engineers are comfortable with. If they say "sure, send it in", It will be a non-standard, essentially, experimental, operation so our normal guarantees won't apply. It will be "we'll do our best."

But that's not the point. The point is that there are still a number of unanswered questions with 0.4mm pitch, and now we have a smaller one??!!

I've only seen 0.3mm pitch in two places: some data from Amkor, and the data sheet for this part.The part in questions is a Maxim MAX98304 Mono 3.2 Watt Class D amplifier. The entire package is just 1mm x 1mm.

There is still a lot of difference of opinion on solder mask defined (SMD) vs. non solder mask defined (NSMD) at super small pitch like this. For BGAs 0.5mm and lager, the general consensus and IPC recommendation is NSMD. At 0.4mm, the Beabgleboard folks at Ti recommend SMD to reduce bridging. But I've had other folks say they get good results with NSMD. For 0.4mm, we've had best results with SMD. It's more than just that though, you also need to religiously follow the manufacturer's recommended pad sizes and such.

Shrinking BGA pitchFor this part, the datasheet shows the pad size (0.18mm), but doesn't cover the SMD vs. NSMD question. Instead, it refers to a Maxim app note (#1891) for that bit of information.

Of course, this is where it gets sticky. That app note, as of this writing, shows 0.5mm and 0.4mm, but no 0.3mm. It does reference IPC-7351, which is a very good thing, but I don't think IPC-7351 has 0.3mm pitch covered yet. Ugh. The 0.3mm part we placed used SMD pads.

Duane Benson
It's not just Facebook where you can designate something: "It's complicated."

 

Missing Mars Probes

Back in ancient times when multi-legged beasts ruled the earth, there were a lot more standards. Or maybe there were just fewer total things resulting in fewer total variations, which looks like more standards.

In any case, if you got a 7408 IC from one manufacturer, it was pretty much equal to a 7408 from any other manufacturer. Even connectors were more or less standard. If you plugged in one PCB mount DB25, you could plug in just about any PCB mount DB25. There were variations, just not as many as now. Today, though, there are a very large number of variations to a standard footprint. For example, while the pin footprint on most Ethernet jacks matches, I've probably seen a dozen different arrangements of mounting and alignment pins.

Another area that can throw monkey wrenches all over is the dreaded metric v. SAE units.

Metric vs imperial

This seems to pop up most often with connectors, as in this image, but it occasionally shows up on other types of parts as well. The footprint here is for a .1" (2.54mm) pitch connector. The connector has 2.5mm pitch. It would be fine for three pins, maybe four or five. But beyond that, it's just not going to fit.

I don't really understand the logic in 2.5mm pitch. If .1", which equals 2.54mm weren't such a ubiquitous standard, 2.5mm would make sense, but as it is, it's just too close. It's close, but they aren't the same. 2.5 != 2.54.

Duane Benson
It doesn't seem like much difference in mm, but in beard-seconds, it's 4,000* units off

*By some definitions, including the Google converter, it would be 8,000 units off