gEDA-user: new footprint guidelines

[DJ Delorie <dj@xxxxxxxxxxx>]

Yes, the old library parts are pre-hires and the pads can be "way off"
and should be fixed.  Thanks!

If we're hand-coding footprints, we could use "0.5mm" instead of
"1965" and preserve the *meaning* of the units.  We lose some
compatibility with older PCBs, but if the purpose is to update the
current distribution that shouldn't be a problem.

We should probably go with build-time generated footprint files,
rather than continue to use the m4 runtime generation.  That allows us
to use more than just m4, too.  Makefile rules for standard %.whatever
to %.fp conversions...

My general rules:

Mask should be 3 mil away from copper, and slivers should be at least
6 mil wide.  That means, if there's less than 12 mil between pads you
go with a gang-opening.

Silk should not overlap the *mask opening* and should be 3 mil away at
least.  5 mil min silk lines.

Origin and license should be stored in element attributes, not file
comments, so they're copied into schematics.

It would probably be a good idea to have more than one design for each
footprint; one for reflow'd boards and one with longer pads for hand
soldering.

All QFN parts should have some visual aids to centering :-) On my last
board, I added four diagonal lines on the silk layer to align each
corner (like a big X), that worked out well.

Refdes should be properly placed and sized but I'm not sure what's
best.  For example, on every single RESC1608N part I place I have to
make the refdes smaller and move it off the pads.  Getting size right
is far more important than position; it's easy (and often needed
anyway) to move things around in only-text mode.

Exposed pads should have a proper solder paste pattern on them too.
This usually means the one pad is made up of multiple pads, some with
"nopaste".  I use one big "nopaste" pad and a small paste pad for each
paste dot I want.


_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user