Screaming Circuits: Layout


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...

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

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."

 

It (.3 mm) Finally Happened

Back in January of 2012, I wrote about the possibility of 0.3 mm pitch BGAs being used here and there. I predicted that in a year, we'd see some 0.3 mm pitch BGAs showing up. I was about three month's off. Almost to the day.

I delivered a session at PCBWest last month and asked if anyone had used a part with that pitch yet. One hand went up. That actually surprised me. What surprised me even more was when one of them (a .3mm pitch BGA, not a hand) arrived on our shipping dock in a parts kit earlier this week.

0.3mm pitch trimFor comparison, the land pattern for an 0402 passive component is about one millimeter long. This specific part is just shy of a millimeter square. Even as small as it is, this part can supply 750 mA continuous. The olden days are so very long gone.

We do many, many complex parts and PCBs. We've put 5,000 parts on a single PC board. We've built boards to be shot up in rockets and dunked way down in the ocean. Some very crazy stuff has come though our shop, but we don't do everything. We don't do 01005 passive components at the moment. Our machines have the technical capability, but we don't rework them, which has to go along with the assembly capability, so we don't support that form factor for now. 0.3mm pitch components pretty much fall into that camp. Our machines can physically pick up and place the component, but until we've developed to process to assemble those parts with the quality people expect from us, we won't be supporting them.

I expect we'll be getting more and more requests for the form factor, so we'll be looking at it. Keep checking back. One of these days, we'll have the process down and reliable.

Duane Benson
It's (Huey mm, Dewey mm, and Louie mm)/10

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

 

More Thermal Examples

Speaking of thermal relief... Here's an interesting example I ran across the other day.

Thermal relief can be a pain. If you've got a high current device, you may want more than just the thin little connections, one per side, that you get with thermals. You might feel the need for greater current capacity or you may need all the copper to distribute heat. You might have one pad, like in this image, that lands on a plane but not the other one.

In this particular board, the designer just made a few parallel traces coming out of the pad rather than one thick one.

Multi-via passive

The other side of this passive part sits right on the ground plane and has the standard thermals so the other reason this might have been done is to keep the amount of copper trace coming into the pad to be equal to that on the other side. It doesn't have exactly the same amount of copper going into both pads, but it's much close than if just one thin trace had been connected on the left pad.

Duane Benson
One thin trace rides away