Re: gEDA-user: footprint help please

[DJ Delorie <dj@xxxxxxxxxxx>]

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