Is this QFN PCB footprint ok for the propeller? (M44)

Mahonroy · 2017-01-16 17:18

Hey guys, originally I downloaded the eagle library for the propeller that contained the QFN footprint.

I noticed that the center pad was not connected to anything, and I noticed that there was solder mask covering the entire pad. I decided to shrink the center pad slightly, and expose this pad by removing the solder mask.

Is this how this footprint should be done? I'm assuming it should just be connected to ground, and I tossed 5 vias in the center as well. Do people not solder the center pad to anything and leave the solder mask on?

EDIT:
I am also thinking of connecting the corners of the center pad to ground as well... just to get better grounding.

Publison · 2017-01-16 17:31

You should exclude the solder mask from the center portion. The vias are good if the go to a ground plane.

How are you soldering? Standard IR oven?

Tracy Allen · 2017-01-16 17:53

Page 36 of the propeller data sheet suggests a land pattern, which for the center pad is divided into 4 smaller exposed pads. Do not use one large pad, the danger being 1) the chip will float up on the lake of solder and will lift off the signal pads and leave the chip at an angle and 2) the solder will release copious amounts of flux that will will outgas with the bad effects and will be difficult to clean off between the pins and lead to problems later on. I'd recommend smaller pads than shown in the data sheet, unless your application is power intensive and the QFN has to dump a lot of heat. As to vias, that is only essential again if the chip has to dump a lot of heat. The solder stencil opening is usually a few mils smaller than the pad. There is no need to connect the pads to ground, as they are not connected within the chip, however, connecting them to ground is a good idea on general principles. QFNs have all manner of manufacturing issues, so please do have a good reason if you are set on using that package.

twm47099 · 2017-01-16 18:49

The final "f" got cut off Terry's link above; it should be:

https://parallax.com/sites/default/files/downloads/P8X32A-Propeller-Datasheet-v1.4.0_0.pdf

Mahonroy · 2017-01-16 18:52

Publison wrote: »

You should exclude the solder mask from the center portion. The vias are good if the go to a ground plane.

How are you soldering? Standard IR oven?

They will be professionally assembled from a PCB assembly company from a pick & place machine, solder paste/stencil, and oven. The challenging part is that I need to solder some prototypes.

Tracy Allen wrote: »

Page 36 of the propeller data sheet suggests a land pattern, which for the center pad is divided into 4 smaller exposed pads. Do not use one large pad, the danger being 1) the chip will float up on the lake of solder and will lift off the signal pads and leave the chip at an angle and 2) the solder will release copious amounts of flux that will will outgas with the bad effects and will be difficult to clean off between the pins and lead to problems later on. I'd recommend smaller pads than shown in the data sheet, unless your application is power intensive and the QFN has to dump a lot of heat. As to vias, that is only essential again if the chip has to dump a lot of heat. The solder stencil opening is usually a few mils smaller than the pad. There is no need to connect the pads to ground, as they are not connected within the chip, however, connecting them to ground is a good idea on general principles. QFNs have all manner of manufacturing issues, so please do have a good reason if you are set on using that package.

Tracy, the diagram you are referring to with the 4 pads... I was under the impression that that is the recommended solder paste stencil to use... not the actual copper layout to use. For example, it seems you have 1 large exposed pad on the PCB, then you put 4 pads of solder paste (generally you don't completely cover the entire pad with solder paste for the reasons you mentioned).

I typically use the QFP chip. This is the first project that had the size constraint so I was required to use the QFN version.

jmg · 2017-01-16 19:00

Tracy Allen wrote: »

... QFNs have all manner of manufacturing issues, so please do have a good reason if you are set on using that package.

Not to mention supply issues ?
See this post by Ken
http://forums.parallax.com/discussion/comment/1292522/#Comment_1292522

"When these QFNs are gone, they're gone. I'd be happy to be in a shortage situation with QFNs because they move very slow. We will unfortunately EOL this part. The MOQ is too high for the inventory turns we have with them.

If somebody wants to order 12-25K at a time we'll build them; otherwise we can't afford to stock these.

QFNs are not preferred by contract manufacturers due to a lower yield during manufacturing."

Mahonroy wrote: »

...
I typically use the QFP chip. This is the first project that had the size constraint so I was required to use the QFN version.

What volumes do you expect ?
If it > 12k, or quite small, you may be ok with supply.

Another solution for size is double-sided assembly, or smaller passives, and I've found QFN are not as small as they first appear, when you factor in no-traces under package -> more vias and routing outside the package.

Mahonroy · 2017-01-16 19:50

I was not aware that they were discontinuing the QFN version of the propeller....hmmm.....

jmg · 2017-01-16 20:13

Mahonroy wrote: »

I was not aware that they were discontinuing the QFN version of the propeller....hmmm.....

Ken might chime in with a 2017 update on supply chain.... ?

Tracy Allen · 2017-01-16 21:18

Sorry, I misspoke about the pads vs the solder stencil openings. It has been several years since I've used the Prop QFN, having decided to save the hassle and use QFP instead. As jmg pointed out, there are factors in the layout that work in the QFP's favor in the overall circuit footprint, also in the inspect-ability and clean-ability. Initially I had wanted to cram the Propeller into a space that originally held a BASIC Stamp, which in a finer pitch 48 pin package occupied about the same area as the Prop 44 pin QFN.

I did have back and forth with the contract manufacturer after initial yield problems. Maybe 8 or 10 out of 100 boards on the first run had problems. Pinpointing issues is time consuming. The CM was experienced, but each new board has its own profile, as much art as science, so that is why you want to do a prototype run to work out the kinks. Another chip on the board, a DFN, was an even bigger problem due to high circuit impedances affected by leakage, but that is all worked out now and I still use that chip, but curse the manufacturer for putting it in DFN in the first place. Multiple problems, troubleshooting headaches. Be sure your CM offers x-ray capability.

As it ended up with the Propeller QFN, the second run reduced the center pad to 285 mil square rather than the 295 mil suggested in the data sheet, and the solder stencil openings were 90 mil instead of 104 mil. The center pad had no solder mask applied. I still don't know if that was a good idea, but the main consideration was to leave plenty of interstices under the chip for pressure washing. No vias, no power dissipation issues. A similar 185 mil pad was on the bottom of the board, connected to distribute Vdd to the 4 Vdd pins with low impedance and act as a very low ESR capacitor.

By the way, your layout looks quite nice. What PCB package are you using?

DigitalBob · 2017-01-17 04:10

Check out my Qfn

WBA Consulting · 2017-01-17 07:40

Here is the layout I use for my Prop QFNs, copied straight from the Propeller datasheet. I know the design is sound as I have manufactured over 200 of my M44D40+ modules and have yet to have a single issue. My Propeller BSC prototypes used the exact same footprint and also worked perfectly.

I don't agree with the fears of using QFNs, especially if you are dealing with a CM because QFNs are old technology nowadays. There really isn't much magic to placing a QFN. The key factor in a DIY field is accurate placement which is a challenge since hobbyists don't have the means for proper inspection/verification (AKA x-ray). Couple that with a lack of good educational data in hobbyist format and you can easily see why so many people shy away from them.

EDIT: Wanted to mention that these dimensions are used with a 5 mil stainless steel stencil. If I was to make a stencil now, it would be 4 mil, but with the same dimensions.

Peter Jakacki · 2017-01-17 08:10

I always use custom footprints not only with that little bit extra length on the pads but also a component outline on the silk screen that makes it a snap to visually line it up. You don't have to do it all the "traditional" way with markers under the chip that you can't see etc.

Also you don't have to put designators and values on the silk screen as the parts are just way too small and packed together to do it cleanly. You certainly don't want any silk screen on the pads etc. I just leave these values on mechanical layers so that when I print an overlay of the PCB I print it to fit to the page nice and big and I have these values nice and clear and readable either on paper or on a tablet.

I might have a better footprint to use but I found this and it is a fairly old one that I used successfully at the time and the extra length allows you to get in there and fix up any bad connections.

DigitalBob · 2017-01-17 16:47

I've included some simple artwork for the qfn to use with expressPCB.

Is this QFN PCB footprint ok for the propeller? (M44)

Comments