[TriEmbed] QFN/LGA soldering hazards

[Pete Soper]

At last month's meeting I passed around an Adafruit QFN32 breakout board 
with an Atmega328 soldered on it. I did this by hand with hot air and it 
was "just like in the movies", with the solder holding the chip in 
perfect alignment and the chip bouncing back into place when nudged to 
one side before letting the solder cool. Perfect the first time, and 
hugely easier than I expected. The rest of this is a comparison of the 
Adafruit breakout board and two that I had made by OSH Park.

Here's why I expected it to be harder. I'd tried many times to solder a 
QFN-16 accelerometer/magnetometer chip onto a board with a reflow oven, 
hot air, dogs barking at the moon, etc. Out of several attempts I've got 
two functional boards and several objects too small to be effective 
paperweights or door stops. Actually, I will pull those chips back off 
and try to reuse them.

And here's a photo of a board after I removed the chip following a 
failed soldering attempt. The picture is edge-on showing the corner of 
the chip pads and an outline of where the package sits:

http://triembed.org/images/badqfn16+chipoutline+text.jpg

The OSH Park soldermask is so thick there are "ledges" of it holding the 
chip off the pads.

But that's nothing. Later I made some boards for a different 
magnetometer that uses a "leadless chip carrier" package. This is 
similar to a QFN but with this chip the pads on the underside of the 
package are very narrow. After several attempts I only managed to get 
one or two sides of the board soldered and the other sides sat above the 
PCB pads by a tiny distance.

This picture of the board should make it obvious why the package pads 
had trouble "kissing" the PCB:

http://triembed.org/images/badbadbad.jpg

As you can see, not only are there ledges on the corners, the PCB pads 
are in "holes" of soldermask because the pads are so narrow there's room 
for mask in between. Weirdest of all, but probably hard to see clearly, 
is that the solder mask in the corners is hugely thicker than the mask 
around the pads. It's as if there are two layers of mask. That's because 
there is a ground plane around the perimeter: the "taller" mask layer is 
sitting on copper. Had I not added that "pour" and just used a single 
ground plane on the bottom layer I might have had an easier time.

And here is the Adafruit board. Notice how the pads are sitting well 
above the surrounding board all the way around:

http://triembed.org/images/goodgoodgood.jpg

The two solutions to my QFN misery are:
   0) Don't use a library footprint that allows solder mask within the 
package outline area of a QFN (or LCC or land grid array) package! Add a 
tstop rectangle large enough to keep the chip from sitting on solder 
mask, period.
   1) No copper pours into the corners of the chip footprint. A tkeepout 
rectangle will prevent encroachment.

A few other precautions are called for. The router may put vias and/or 
traces very close to the pad area, tempting the solder bridge monster. 
Also watch out for misaligned wires that encroach on the space between 
two pads. That is, a wire may go to a pad and sit diagonally or offset a 
bit, so the edge of the wire is narrowing the gap between two pads. You 
can suppress routing of vias and traces under the chip with trestrict 
and brestrict rectangles (important for magnetometers!)

-Pete