Propeller Land Patterns?

Phil Pilgrim (PhiPi)

I haven't located any recommended PCB pad dimensions in the Propeller docs — only package dimensions. Can anyone recommend a source of this data for both the QFN and LQFP packages? (My CAD software includes ten different QFP-44 layouts, and no QFN-44's.)

Thanks,
Phil

cgracey

It turns out our LQFP-44 package uses the smallest of the (L)QFP-44 footprints. We will get recommended land patterns together soon and add them to our docs. For now, I'd just verify that the smallest land pattern that you have measures out against the chip okay. This was·a huge issue when it came time to pick a test socket for our testers. Some (L)QFP-44 sockets were so big that our chip fell right the hole of the socket. I would have thought they'd all be the same, but they vary a lot, even though the pin pitches are identical.

For the QFN, there are a few things to consider. Foremost, you need an exposed copper pad on your PCB to mate up with the big square in the middle of the chip. The copper pad should mate to the chip 1:1 and be grounded. Another critical thing you need is a paste mask that deposits paste on only 1/2 of the area of this square pad - do this in quarters. You don't want the chip to float too high on solder and miss its pin connections. For the pins, just make sure you cover them 1:1 with copper pads, with a little extra copper going away from the chip so that you'll be able to see the joints. The paste mask should deliver copper to the entire pin pads (unlike the 1/2 coverage required by the big middle square pad).

Phil Pilgrim (PhiPi) said...
I haven't located any recommended PCB pad dimensions in the Propeller docs — only package dimensions. Can anyone recommend a source of this data for both the QFN and LQFP packages? (My CAD software includes ten different QFP-44 layouts, and no QFN-44's.)

Thanks,
Phil

▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔


Chip Gracey
Parallax, Inc.

Tracy Allen

I have the same question about the specific land pattern for the QFN. It is tempting because it would take about the same PCB real estate as the SX48 in the TQFP package. But soldering and inspecting the QFN sounds pretty formitable without the best equipment and care.

A couple of most informative documents I've found online are,

www.freescale.com/files/analog/doc/app_note/AN1902.pdf
which shows a 9mm QFN, but it is a 64 pin chip with lands on 0.5mm centers.

I think the Propeller QFN is 9mm with 44 pins on 0.65mm centers. These documents talk about how some QFNs have the lands exposed on the edge of the package, and some don't (depends on sawed vs punched singulation). It seems like the advantage of the exposed end is that it can form a fillet that you can inspect visually after soldering. Otherwise, its x-rays and crossed fingers.

www.amkor.com/products/notes_papers/Board_Level_QFN.pdf
has a lot of experimental reliability test information based on different soldering and land parameters.

They both go into the considerations about islands of solder coverage on the center pad. They also recommend vias under the central pad through to the ground plane for thermal reasons, with no thermal isolators. The vias should be covered with solder mask to prevent down wicking of solder during reflow.

▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
Tracy Allen
www.emesystems.com

cgracey

Tracy Allen said...
I have the same question about the specific land pattern for the QFN. It is tempting because it would take about the same PCB real estate as the SX48 in the TQFP package. But soldering and inspecting the QFN sounds pretty formitable without the best equipment and care.

Yeah, it's small enough to fit onto BASIC Stamp-sized modules (600-mil wide DIPs with leadframe pins).

A couple of most informative documents I've found online are,

www.freescale.com/files/analog/doc/app_note/AN1902.pdf
which shows a 9mm QFN, but it is a 64 pin chip with lands on 0.5mm centers.

I think the Propeller QFN is 9mm with 44 pins on 0.65mm centers.

That's correct.

These documents talk about how some QFNs have the lands exposed on the edge of the package, and some don't (depends on sawed vs punched singulation). It seems like the advantage of the exposed end is that it can form a fillet that you can inspect visually after soldering. Otherwise, its x-rays and crossed fingers.

Ours is the sawed variety, so there will be less to see. We bring our pads out 5 mils beyond the edge of the package.

www.amkor.com/products/notes_papers/Board_Level_QFN.pdf
has a lot of experimental reliability test information based on different soldering and land parameters.

They both go into the considerations about islands of solder coverage on the center pad. They also recommend vias under the central pad through to the ground plane for thermal reasons, with no thermal isolators. The vias should be covered with solder mask to prevent down wicking of solder during reflow.

My intitial experience with these packages was awful - we couldn't get one to work. Now that we've got the paste limited on the center-pad solder stencil. We have not seen a single failure in all the Propeller Demo boards we've built (each has two QFN parts). Once you get the paste thing straightened out, you can't mess it up!

As far as the Propeller goes, it barely gets warm, so vias for thermal relief would not be critical. I think that the die being brought so close to the PCB·would·have·a tremendous heat disipation·advantage over LQFP, also.

▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔


Chip Gracey
Parallax, Inc.