Re: gEDA-user: 2 newbie Qs

[DJ Delorie <dj@xxxxxxxxxxx>]

> How do I make a single gschem element that refers to only one of the
> pins, say pin 3?

Create a gschem symbol with one pin.  Name it "3".

Go to www.gedasymbols.org and look at Darrell's xilinx symbols.
They're a good example of breaking one footprint up into multiple
symbols.

> 2. In a linear array of pins, say one side of a DIP or a single row header,
> given a hole diameter H and an interpin distance D (commonly 0.1 inch or 2
> mm, but could be others,) are there any good suggestions for formulas for
> thickness T, mask M and clearance C?

This is subjective.  Here's what I do.

For a given line/space (L/S) rule, L+2*S+2 mils between pin copper to
leave room for one trace between pins.  If you need two traces, it's
2*L+3*S+2.  Thus, for a pin spacing of D, pin copper diameter P is
D-(L+2*S+2) mils.

For small vias, I make the annulus width ((P-H)/2) the same as the
line width (i.e. 20 mil drill = 36 mil copper for 8 mil rules) I'll
use it for (i.e. larger copper for wider traces), up to a maximum
size.

I make mask S/2 mils bigger than the copper, so that the edge is
halfway between the pin copper and the trace copper.  For SMD pads
that are too close for a line between, I use G/3 (where G is the gap
between pads) for smaller devices and G/4 for larger ones.

Poly clearance can be anything you want, but it must be at least S.  I
used 10 mils in my current project, where lines were 8 mils and the
fab's design rules are 6/6.  For SMD parts, I make clearance just big
enough so that there aren't copper strips between pads on small pitch
parts, especially when the strips would be smaller than the design
rules.

Note that fabs often have different rules for inner layers than for
outer layers.


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