Hand To Machine

It's getting very difficult to hand solder many parts these days. Some people give it a try, but in general, if you're dealing with the really tiny parts or leadless parts, it's just not possible, or at least not  practical.

QFN worng part library Sometimes a designer will start out with the idea of hand soldering the board up and then either decide against it when first looking at the raw PCB, or will build one and then decide that it's too much work. That's not a bad thing. You can get more reliable assembly and it keeps me employed. But there are times when a layout designed with hand assembly in mind does not work for machine assembly.

Case in point, this image. Now there are two things wrong here. The first is that the land pattern is for  a smaller part than the actual component. Let's pretend that problem doesn't exist. The other problem is that big via hole in the middle of the pad. When hand soldering parts with a solder pad underneath, like QFNs or QFPs, folks will often put a large hole there. They'll solder the outside connections first. Then, turn the PCB over and stick a soldering iron and some solder in that big via to solder up the pad.

That works more or less for hand soldering, but it's a really bad thing to have a big open via like that when machine assembling parts. The solder will flow down and out the other side. You'll get a mess on the bottom of the PCB and you may get little or no solder on the pad.

So, the moral of this story is that if you've designed your PCB for hand soldering and later send it out for automated assembly, go through the layout and make sure you remove things put in there for hand soldering that aren't conducive to reliable machine assembly.

Duane Benson
Don't fall in...

0.4mm Pitch BGA Redux

I've written about it before, and again here.

When dealing with new technology parts, it's really important to look up all of the manufacturer's component information that is available. I'm going to quote from the Texas Instruments document "PCB Design Guidelines for 0.4mm Package-On-Package (PoP) Packages", Section 10 (PDF page 8)

"Industry reliability studies have revealed that NSMD-type pads are highly recommended for most 0.5mm pitch BGA applications. However, there is a problem with this approach at 0.4mm pitch.

Real-world assembly experiments with the BeagleBoard and the OMAP35x EVM revealed a tendency for solder bridging between pads when NSMD were used. There was insufficient solder mask webbing between the pads to ward off bridging. Therefore, a SMD design was used which resulted in much better assembly yields with no solder bridging."

If you are using a 0.4mm pitch BGA with the balls aligned in a grid (as opposed to staggerd), read the design guidlines from the manufacture before laying out the board.

In a presentation about the development of the Beagleboard, Gerald Coley, Beagleboard designer, notes that their first two runs had non soldermask defined pads resulting in a 10% yield. After another run of PCBs where the pads on the PCB were the same size as the pads on the device and the PCB pads were soldermask defined, their yields went to 96%. And verify that your PCB house does in fact follow your instructions. Some will think they know better and will change the mask layout.

If you are still unsure or think your design will have different requirements, call an applications engineer at the component manufacturer and discuss your project and the layout.

Duane Benson
Trust but verify

Et Tu Embedded Passives

I don't know if or when embedded passives will become the "next big thing" in PCB design, but they are on the way. We, at Screaming Circuits, have been asked about the use of embedded passives a few times.

Embedded passives
The purported advantages of the technology lie primarily in the ares of cost reduction and space reduction. You could potentially get your bypass caps much closer to where they need to be as well. The space parameter is pretty obviously an advantage, but the jury is still out on costs. I suspect that at this moment, it's pretty difficult to find a board house that can fabricate a PCB with embedded passives.

If you're not familiar with the concept, capacitors or resistors are built up on the inner copper layers of the substrate. There are a couple different methods used such as plating, printing or thin-film. As shown in the illustration, the resistors and capacitors inside the PCB negate the need to mount them on the outside. I can see rework being a problem if any of those embedded parts has issues.

In terms of assembly, we wouldn't treat such a board any different than any other PCB. If your fab house notes that there are temperature or any other restrictions, let your assembly house know. Beyond that, all the standard rules apply.

Duane Benson
Note from Forbin: Colossus is watching

On Final For Landing on Runway 0805

S part pad shift in oven process Keep out areas can be a problem when adapting a CAD component land pattern, but that's not the only potential problem. Sometimes the part may be close, but the footprint is different enough to cause problems, as in the picture on the right.

You can also run into issues that don't necessarily cause PCB assembly problems, but can be expensive none the less.

Say you are designing with a small microcontroller and the schematic symbol and land pattern don't exist for the one you're using, but something close does. Even though the two parts may look like pin for pin replacements, they may have a few differences.

The PIC family has a number of examples of this. For example, the PIC18F2321 and the PIC18F2455 have enough similarities that they look like pin for pin replacements. However, upon closer inspection, you'll find that RC3 exists on the 18F2321, but doesn't on the 18F2455. SCK/SCL and SDI/SDA are in differnt places on the two processors. You could end up with a bunch of jumpers and a PCB re-spin if you just used one land pattern for the other. It pays to check for those little details.

Duane Benson
Turn left at the big tree, and go until you see the creek.

Keep Out and Keep Off the Grass

The part land patterns in your CAD package parts library should all come with a valid keep-out area defined. That's the theory anyway. However, theory and practice don't always match up so well. I've written a lot about such things as verifying that the actual footprint matches the physical part. That's important. But it's not all that's important.

Caps under BGA Sometimes the footprint will match up just fine, but the body of the part won't. This might be because you're using a different variant of the same part or perhaps a different part altogether that just happens to have the same footprint.

It's common practice to modify an existing library component for a new part, but if you do that, make sure you consider the physical dimensions of the part body too. Sometimes you can get away with the keep-out area being different, but as shown in this image, not always.

Duane Benson
Keep off my lawn, ya young whippersnapper!

Via Caps

The best way of dealing with via-in-pad requirements is to have the vias filled and plated over at the board house. There can still be some issues with that technique, but if done right, is very reliable and the best way to go. But, what do you do for a Klondike bar? I mean what do you do if you can't afford to fill and plate over your vias, or don't have the time? Well, if your vias are in a BGA pad and you don't want to have them filled and plated over, than you can just go back to the drawing board because your board most likely won't work. There may be some secret, prototype-only things that your assembly house can do, but avoid it at all costs.

If your vias are under a QFN or SOT-23 or something bigger like that, you have more options. Don't leave them open. Worms will use the open vias as homes. You can usually use soldermask to cap your vias in cases like this.

Soldermasked vias side view for blog

C is not an option. A and B can work. D can work also, but should be your last choice. With the tight masking like in A, most manufacturers recommend that the soldermask cap be about 100 to 125 micron wider than the diameter of the via. B is self evident - just make it bigger.

The pitfalls with D are that solder will still get sucked down into the via which can lead to excess voiding. Or, the via cap could pop open which results in effectively a C. With all soldermask via caps, top ot bottom, you need to check carefully to ensure that the soldermask gives a complete seal. And there is always a risk of the cap breaking. Ugh. Now do you see why everyone recommends filling and plating?

Duane Benson
The worms crawl in
The worms crawl out
The worms play pinochle on your snout

I'm a capitalist and I'm okay...

I'm a capitalist and I'm okay
I work all night and I sleep all day

300px-LaunchPad_wireframe Well, I don't work all night so much anymore. I used to.  I am a capitalist though. I think money is good (what some people do with it, not so much). And, I also think that when people make money, they should do so in such a way that others benefit as well. That's one of the reasons I like Ti's Beagleboard so much. Speaking of Ti, they have another microcontroller product that I'm excited about as well.

The MSP430 LaunchPad is a little development board designed for education in general as well as familiarization with the MSP430 line of microcontrollers for experienced developers. (I hope they don't mind that I'm using their picture on the right here. I don't have one so I couldn't take my own picture of it.)

A lot of companies have development boards for their chips. That's nothing new. But what is really cool is that they have set a retail price for this of $4.30. Yes, the price of a 16 ounce latte.

Now I know that a latte is important. Some people have speculated that civilization would collapse without caffeine. But, here's what you get in the place of that latte: (from the Ti website, again)

"For $4.30, the LaunchPad includes a development board, 2 programmable MSP430 microcontrollers, mini-USB cable, PCB connectors for expandability, external crystal for increased clock accuracy, and free & downloadable software integrated development environments (IDEs)"

Cool. I can explode one and still have another to finish the project with. I'm going to get me one of these and spend some time with it. I don't have any personal experience with the MSPP430 line, so it will be filling it's primary mission.

On the subject, I ran across an interesting website dedicated to the MSP430: www.43oh.com. If you're already a 430er or are just intrigued by the chip, go check it out.

Duane Benson
Buttered scones, anyone?

« November 2010 | Main | January 2011 »