How To Build A PCB: QFN Footprints
- May 25, 2018 -
QFN and DFN parts
Physically small size and footprint aren't the only advantages to a QFN. The smallest of these packages end up with very short lead wires. This allows for improved signal characteristics and excellent thermal properties. Most QFN and DFN parts have a large metal contact area on the underside, just inside the rows of signal contacts, as shown in the image above.
The silicon dice sits right on the thermal pad, thereby allowing for some impressive thermal performance. I've seen 3mm x 3mm QFNs that can output 5V at 800mA, which used to require a big TO-220 package and a heatsink.
This extra performance comes with a price, though. In this case, the price is largely in the arena of manufacturability challenges, which is how our conversation returns to my day job. At Screaming Circuits, we've learned what causes QFN problems and how to prevent those problems. It comes down to the amount of solder paste that is put down and the difference in surface area of the big thermal pad and that of the side contacts.
Solder is put on surface mount pads through a silk screening process or with a solder paste jet printer. In the silk screening process, a stainless-steel solder paste stencil is created by laser cutting openings for all of the surface mount component pads. This stencil is then placed on top of the printed circuit board (PCB) and solder paste is put down with a squeegee. This process is nearly identical in concept to making a silk-screened T-shirt.
Many shops, mine included, also use a paste jet printer to apply the paste. This has the advantage of allowing for easy modification of the paste pattern on the fly. Its disadvantage is that the paste droplets it applies don't give the precision needed by some of the newer super-small parts.
A typical solder stencil might be 3 or 4 mils (0.067 to 0.100mm) thick. Looking at the QFN photos above, you can see that the aspect ratio of area to a 4mil stencil thickness is quite large for the center pad but much smaller for the contacts along the sides.
When the solder paste melts in the reflow oven, the shape of the solder deposition will change. I won't go into the fluid dynamics of that setup, but the result is that, if the center pad is given a full dose of solder paste, the part will float up on the center pad and some or all of the side contacts are very likely to not solder, as shown in the illustration below:
QFN float (Source: Duane Benson)
The stencil opening is controlled by the CAD footprint. Unfortunately, the footprints of QFN and DFN parts in CAD libraries are almost always wrong in this regard. They provide a solder paste opening that is the same size as the copper pad. Not only are they almost always wrong in the CAD software, but they're almost as frequently shown incorrectly in the component datasheet.
Rather than a full-size opening, the stencil layer should be segmented to give 50 to 75% paste coverage on the center pad as illustrated below:
QFN segmented stencil (Source: Duane Benson)
The openings for the solder paste stencil (or the deposition pattern for the paste jet) are specified in the stencil layer -- sometimes called the "paste layer" or "cream layer" -- in your CAD software. Many footprint editors automatically create the stencil layer when you place a surface mount pad.
That's part of the problem. In many cases, the software automatically creates a stencil opening matching whatever the copper pad size is. The fact that the tool does this automatically means that many users are under the impression that they don't need to think about this, but they really do, because -- for a big QFN heat slug -- it will probably be wrong.
Correcting the footprint is a pretty easy task, but how would you know that you need to fix anything unless some PCB assembly person rants at you? You probably wouldn't, so here I am, ranting at you.
The solution, as I said, is pretty easy. Well, it's easy if you're familiar with the process of creating or modifying the footprints in your CAD software. I'll leave that specific detail to you, but if you know how, or once you've learned how, I'll tell you what to do.
In your footprint editor, turn off the automatic paste layer and hand draw it. The technique will differ based on the workings of your footprint editor, but what you need to do is the same. Make sure the stencil layer isn't being created by default, and then draw it in in the stencil layer. The illustration below shows an example of what it should look like.
QFN solder paste stencil layer good examples (Source: Duane Benson)
Shoot for between 50 and 75% solder paste coverage; i.e., the solder paste should cover 50 to 75% of the copper pad. If there are any vias in the pad, don't put paste on top of them. Vias need to be capped with solder mask, or filled and plated over. If you leave open vias, the solder will wick down and end up on the far side of the board. This is also not a good thing to happen.
One more thing: Is it 50% or is it 75%? In a prototype or small quantity world, anywhere in that range has a good chance of success. If you are building a high-volume product, you'll want to work with the manufacturing engineers at the company building your boards. They'll start in that range and tweak the stencil pattern to achieve the best possible results on their manufacturing line.
QFNs can be a bit intimidating, but they're here to stay. With a little extra care, you can be quite successful with them. You may even be able to shrink your board a little and save some of the fabrication costs.