Re: gEDA-user: Footprint with Unusual Pads

[DJ Delorie <dj@xxxxxxxxxxx>]

> Looking at the PCB docs it seems like SMD pads must either be round or
> rectangular, never both?

Right, but you *can* have multiple physical pads for each logical pad.
Just overlap them.

> They'r drawing longish pads which are round on one end and rectangular
> at the other end.
> 
> Also the die-attach pad has a very unusual complex polygonal form.

Both can be made from multiple pads.  See (also attached):
http://www.gedasymbols.org/user/dj_delorie/footprints/test/bq24070.fp

The trick is to name/number each individual pcb-pad according to the
part-pin it goes with.  For example, the two pads that are "pin 1"
would both be numbered "1".

> What's the right way to define such a footprint (preferably
> oldlib-style)?

The m4 libraries are deprecated.  Please create new symbols in newlib
style.  Also, you can create footprints inside pcb using lines and
rectangles, which is easier than figuring out the m4 stuff.


Element["" "" "" "" 11811 16732 0 0 0 100 ""]
(
	Pad[-1 0 3149 0 5905 2000 7905 "" "14" "square,edge2"]
	Pad[-4134 0 -3937 0 2756 2000 4756 "" "13" "square"]
	Pad[-6890 2953 -4921 2953 1102 2000 3102 "" "12" ""]
	Pad[-7874 2953 -5905 2953 1102 2000 3102 "" "11" "square"]
	Pad[-7874 985 -984 985 905 2000 2905 "" "10" "square"]
	Pad[-7874 -984 -984 -984 905 2000 2905 "" "9" "square"]
	Pad[-6890 -2952 -4921 -2952 1102 2000 3102 "" "8" ""]
	Pad[-7874 -2952 -5905 -2952 1102 2000 3102 "" "7" "square"]
	Pad[984 -6889 984 -4921 1102 2000 3102 "" "6" ""]
	Pad[-984 -6889 -984 -4921 1102 2000 3102 "" "5" ""]
	Pad[-2953 -6889 -2953 -4921 1102 2000 3102 "" "4" ""]
	Pad[984 -7874 984 -5905 1102 2000 3102 "" "3" "square"]
	Pad[-984 -7874 -984 -5905 1102 2000 3102 "" "2" "square"]
	Pad[-2953 -7874 -2953 -5905 1102 2000 3102 "" "1" "square"]

	)


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