Re: gEDA-user: pcb footprint syntax

[DJ Delorie <dj@xxxxxxxxxxx>]

> How does this match? There are nine Arguments in my pin definition but
> only seven in the docs.

FAQ. Look in src/parse_y.y for pin_hi_format:

pin_hi_format
	/* x, y, thickness, clearance, mask, drilling hole, name,
	   number, flags */
	: T_PIN '[' NUMBER NUMBER NUMBER NUMBER NUMBER NUMBER STRING STRING flags ']'

> PS: "Copper width" is what Protel speak calls "annular ring", is it?

For pins, "thickness" is the outer diameter of the copper.  The
annulus width is thus (diameter - drill)/2.

Clearance, however, is the difference between the copper diameter and
the hole we make in polygons when the pin overlaps them.  Thus, the
annulus of the clearing is clearance/2.  Sigh.

> PPS: Is 4600 really the drill the fab is going to use? Or do they take a
> slightly larger one because the metalized hole will be smaller?

That's up to your fab.  Some want "finished size" in the drill file,
and they compensate for how much plating their process adds; others
want actual drill size, and you have to compensate for plating
(usually 0.1mm or so difference).

Note that drills in the "hi res" format (square brackets) are in 0.01
mil units, like everything else.  So, that's a 46 mil (1.15mm) hole.