> I have a part with no vendor recommended footprint. It's called VSOP30 > pin pitch = 0.22mm +/- 0.1 > center-to-center = 0.65mm > outside-to-outside width = 7.6mm +/- 0.2mm > pin size is 0.45mm +/- 0.2mm
My design rules are: * pad width for largest pin width, or more. * pads extend under the chip past the bend in the pin, perhaps to the body width. * pads extend outward by 10-20 mil to accomodate my smallest soldering iron tip. I wrote a footprint generator specifically designed for taking footprints from specs: http://www.gedasymbols.org/user/dj_delorie/tools/dilpad.html So I'd set PWE to zero or more, in this case perhaps instead setting PW to half the pitch, G (gap) equal to minimum BW (body width), and specify PLE (pad leg extension) according to your soldering preferences. CW (chip width) should be the widest the spec allows for. So for me (with part outline turned on)... http://www.gedasymbols.org/scripts/dilpad.cgi?units=mm&np=30&seq=A&bl=9.7&bw=5.6&pol=on&c=&cw=7.8&e=0.65&g=5.5&ll=&lw=0.23&m=&pg=&pl=&plc=&ple=15mil&pw=0.35&pwe=&pxl=&so=10mil&soc=&sw=5mil As always, print it out 1:1 scale and verify with an actual part. _______________________________________________ geda-user mailing list [email protected] http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
