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."

 

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

Connectors Kill

Lot's of types of components can cause footprint woes. QFNs have their center pad issues. BGAs have escape via issues. But the most common footprint issues seem to be with connectors. At least with chips Connector footprint 2smand discrete silicon and passive components most manufacturers pretty much follow IPC standard footprints. Sometimes they'll create new ones for smaller parts, but generally they still stay reasonably close to in line.

Connector footprint 1smConnectors are another story though. I'm not sure any manufacturer follows anything close to a standard. This pair of ethernet jacks is a good example. Often the actual pin layout will match, but the mounting will vary widely. I've seen it on ethernet, mini-USB, micro-USB and even the old, old RS232 connector.

It gets more frustrating when they're almost the same. We see that a lot; the layout will almost, but not quite match a footprint in the library. The bottom line is never take a connector footprint for granted. Always double check before getting your boards fabbed.

Duane Benson
Carburetors man. That's what life is all about.

"Shrinky Dink"

I had some "Shrinky Dinks" when I was a kid. Amazingly you can still buy them. You can also use that concept in your prototyping. I did that recently. I have a robot board design that I'd like to shrink about in half and add in a LiPoly charger chip. Most of the design came from something I had built previously, but the charger chip was new to me as was the compression needed to meet my size goals. Sadly, you can't just put your PCB in the oven and have it shrink like a Shrinky Dink. Maybe if you could put stretchy copper traces on it so they wouldn't peel of while the substrate shrinks...

The charger comes in both DFN-10 and MSOP-10 packages and the MCU comes in SOIC and QFN packages. The QFN is the 44 pin version while the SOIC is the 28 pin version of the chip. Same core. Just more I/O.

LBDC Li LBDCmini pRather than test my ability to shrink and the use of the LiPoly charger at the same time, I added it into the original design without changing the size. There's much more room for probing or even for adding test points if I needed them. Once that design checked out okay (which it did), I just went into the schematic editor, changed the SOIC to the QFN package, the MSOP to the DFN and most of the passives to 0402 packages. I really didn't have to make any changes to the schematic.

That almost worked perfectly. The 28 pin MCU doesn't come in a variant with a QFN package, so I couldn't just change the package type in the schematic editor. I had to delete the SOIC version, place and wire in the 44 pin QFN variant. I made a few other changes too. I added in a QFN packaged RS232 driver and a hard power switch. In the original, I had envisioned a soft power switch but I changed my mind. I also had to modify the library parts to make sure that the solder paste layer on the QFN and DFN parts fit our guidelines. Lastly, I removed some LEDs that I only had on the board for debugging purposes.

The most important two considerations were watching out for physical part interference and getting the paste layer correct on the QFN/DFN parts.

Duane Benson
It's the size of a small walnut

Oh MSOP, My MSOP

LiP DFN unstuffedIn the land of protorypes, sometimes "close enough" is good enough. That can save money on PC boards and assembly when a particular package version of your part is out of stock. But, it's not universal. Sometimes you can't go that way.

I've got an MCP78338 Li Poly charger chip. It comes in 10-DFN and 10-MSOP packages. I originally used the MSOP version on my first PCB pass. Everthing worked just fine, so I re-layed out the board to be about half the area. That meant that wherever possible, passives went from 0603 to 0402 and chips went from whatever to QFN/DFN pacakges.

LiP MSOP on DFN padUnfortunately, the DFN package Li Poly charger seems to be out of stock with long lead times. That got me looking at my options. Option 1, would of course be to just wait. Option 2 would be to re-lay out the board for the MSOP part in that space. Option three is to use the "we'll make it fit" mantra. There are no gurantees at this point, but sometimes it's worth a try.

But... Twas not to be. If you look at the second image, you can see that the footprint of the MSOP part leads is wider than the land pads for the DFN. I suppose there are still a few really messy and potentially expensive options You could solder a small wire on to the pads, sticking out from the pads, effectively making them big enough to accomodate the chip. Very ugly, but might work. Probably too spendy though.

Duane Benson
Carpe DFN

Let's Get Small - 0.3mm pitch BGA

I recently got an email from Practical Components about their new 0.3mm pitch evaluation board and dummy 0.3mm pitch BGA. Now, we've been assembling 0.5mm and 0.4mm pitch BGAs for years. Those sizes are kind of not really anything special anymore. We've even been putting together POP (package on package) for a couple of years. But we've yet to see anything smaller.

Shrinking BGA pitchJust looking at the numbers, 0.3 may not look all that much smaller than 0.4, but that's 25% down. Thinking of it in those terms makes it much more intimidating. I haven't found the pad dimensions yet, but just using rough estimates, a 3 mil trace would have about 1.5 mils on either side for a between the pads trace. That's getting pretty dangerous. Likely, you'd have to do every thing with filled and plated-over vias in the pads. (NO OPEN VIAS! Not one. Don't do it.)

I can see a lot of good future use for this size in miniature devices; more processing power in hearing aids and embedded medical devices, for a start. I don't know how necessary 0.3mm pitch will be for phones. They seem to have stabilized in size and the trend is more toward system in chip than it is toward more shrinking. Regardless, I would expect that in a year, we'll be seeing mainstream parts in this form factor.

Duane Benson
Go ask Alice
I think she'll know
How to run your escape routing

Thru-hole to SMT

Thanks to a comment from Michael yesterday, I think everything is now cool with my Geiger counter. I had left the AT2313 default fuse setting at clock/8. That dropped the RS232 speed from 9600 to 1200 and it made the clicking sound into more of a tone, which just didn't sound right for a geiger counter. I still need a good radiation source though. I think I've picked up just a few clicks of background radiation, but that could just be wishful thinking.

WishfDFN-8ul thinking or not, that's not the point. The point is that this was an example of migrating from thru-hole parts to SMT. I managed to get virtually everything into SMT. The connectors, the power switch, the buzzer, batter holder and fuse clips for the tube stayed thru-hole. Although I'm sure I could have all but the battery holder and fuse clips into SMT had I wanted to. I tend to keep switches and connectors that will get a lot of use as thru-hole just for the extra staying power. If they aren't used frequently, then SMT is just fine.

There are a number of things to consider when switching from thru-hole to SMT:

  1. Everything is smaller, so you can fit more in the same space or the same in less space. I took advantage of the extra board area to add in a RS232 line driver so I could connect directly to a serial port. I also added in a power-on LED.
  2. Everything is smaller so your layout is more critical. Most PCB houses will build 8mil trace and space as standard process these days. That gives you a lot of flexibility in squeezing your routing into tight areas, but it doesn't give complete freedom. You have to be core careful because you frequently do have to route a bunch of traces into a pretty small area. When you get into the really fine pitch parts, like .5 or .4 mm center to center, you have to be extra careful.
  3. Some parts are dimensioned in metric and some in SAE units. If all are one way or the other, it's easy. But when you've got both, you may have to tweak with your grid spacing off and on to make sure your traces are centered in the SMT pads they connect to. It usually isn't a horrible problem, but it can make even spacing more difficult and can make you more likely to violate a design rule.
  4. You don't have automatic "vias" on each component leg so routing can be more difficult. You'll likely have to spend more time tweaking the part locations and the trace routing to get a decent layout. A lot of times everything's too close so it's not practical to just plant a lot of vias all over.
  5. Hand soldering is less or not practical. Some people do hand solder some pretty tiny parts, but it's not practical in more than isolated cases. If you're a hobbyist or on a tight budget, this might limit you to thru-hole or some of the largest SMT parts. For commercial work though, SMT is the way to go.

Some things to think about. But what do you get in return? Typically lower cost - especially if you want your design to go into volume manufacturing. You also get access to the newest parts that only come in SMT packages. And, many designs are space constrained, so you can cram more in while still keeping your board size down.

Duane Benson
I shot a neutrino into the air
And where it landed I already knew

 

Speaking of Small Packages...

T'was a a dark and stormy night when the news came through. Joe Layout had been both dreading and preparing for years. But it had always been little more than rhumors from a far off land. It was a looming threat, always dancing in the distance, but never quite real.

Until now. 1.27mm, 1.0mm, 0.8mm, 0.5mm, 0.4mm... and now... drum roll please 0.3mm pitch. I just got Shrinking BGA pitchan email announcing an Amkor 8 x 8mm 368 ball BGA at 0.3mm pitch. Yikes.

There's still some controversy over the best way to make a 0.4mm pitch BGA land pattern. Some say says you need to use solder mask defined pads. Some say you still need to use the non-solder mask defined pads. Now we throw something 25% smaller into the mix.

The image isn't to exact actual scale - because I don't know how big your monitor is - but the parts are in relative scale from 1.27 pitch to 0.3 pitch.

Duane Benson
If you can't see it, you shouldn't eat it