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@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user