[gta02-core] PCF50633 footprint and footprints in general
werner at openmoko.org
Tue Dec 1 22:31:23 CET 2009
Dave, I've been looking at some of your new footprints and I noticed
some oddities with the PCF50633. This isn't the only QFN that's tricky,
so I'm posting this to the list.
First of all, except for most BGAs, footprints are larger than the
pads/legs of a component. Many data sheets only show the chip in all
its glory but remain silent about the corresponding footprint. (And
some have a decent enough chip drawing but then give a completely
insane footprint, but that's another story.) So one has to do a bit of
hunting, e.g., look on the vendor's Web site for additional material
or see if any competitor has a chip with the same geometry.
If the source for the footprint is different from the data sheet, only
the former should go into modules/INFO.
NXP are usually a great source of footprints. Their database is here:
Unfortunately, in the case of the 50633, they're not so helpful.
There are some general recommendations in AN10366
but they are all for simpler packages, without the elongated middle
The closest component with both package drawing and footprint I could
find is the HVQFN48:
This one has a pad width at the package between 0.18 mm and 0.30 mm
and at the footprint of 0.29 mm. In the case of the PCF50633
(HVQFN68), we have a pad width between 0.15 and 0.25 mm, so the
footprint should probably have a width around 0.25 mm too.
It's always a good idea to also have a look at what Openmoko has been
doing, i.e., the Gerbers of GTA02:
Here we can see that a width of 0.25 mm was used. No special
arrangements were made for the elongated pins, just is probably a
There is one violation of NXP's recommendations in the GTA02, and
that's the distibution of the solder paste on the center pad. NXP
recommend to put multiple small areas of solder paste instead of
filling the entire pad. (See the HVQFN48 example.) A nice example
of how this can be done with fped is the WM8753FL.
More information about the gta02-core