Re: gEDA-user: footprint critique request

[DJ Delorie <dj@xxxxxxxxxxx>]

Some quick comments:

Your holes are 35 mil, the spec says 59 mil

Inner ring is 0.28in diam, spec says 0.30in

Outer ring is 0.824-0.848in diam, spec says 0.87in.

Note: radial layouts like this really want to be done by a perl script
or other program, which can position the pins more precisely.  Even if
you just have it dump the pins and you add everything else manually,
it's better than doing all those pins by hand.

Since the copper pads will be used for mechanical strength, make them
MUCH bigger than you have.

The default location for the refdes interferes with the other silk;
better to move it just below pins 6/7

Your pin A seems to have a thermal to layer 9 pre-defined.

You should use the Attribute() syntax to include copyright and
authorship information in your element; regular comments will not be
preserved in a layout.

Your arcs, for some reason, have origins at various off-by-one
coordinates.  Note that the file format *does* allow full circles;
it's only the GUI that limits you to creating 90 degree arcs.  Create
one arc in the GUI, and later edit the .fp file by hand to change the
angles to "0 360".


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