Re: gEDA-user: Two questions about pcb.

["harry eaton" <bumpelo@comcast.net>]

> 1)  I need to make a drilled hole without copper in a layout (see the
>     part at
>
http://rocky.digikey.com/scripts/ProductInfo.dll?Site=US&V=102&M=SJ-3524NG
>     )  Can I do this in pcb by making a via with holesize=viasize?  Or
>     is the board house gonna complain?

You want to turn the via  into a pure hole, by typing Ctrl-H (H for hole)
with the cursor over the via. That way it doesn't have a copper annulus
and it appears in the fab drawing as unplated and in the "unplated" drill
file.

> 2)  How do I make a pcb that is not rectangular in pcb?  That is, I need
>     to tell the board maker how to route the outside of the pcb.

You need to make one of your layers a route layer. Name the layer "route" or
"outline" and make sure it's in it's own group. Then draw a 10 mil path of
lines/arcs
for the board outline. The fab drawing will then show the center line of the
path
as the board outline. It's up to you to make sure all your stuff fits
properly inside.
You really should make a gerber file that has only the route too, but at the
moment
this isn't automatic because the gerber for that group will show all the pin
and via
pads too. To make this gerber file do this:
(1) save your design
(2) turn off the route layer so it's not visible, but make all other visible
(3) do a "select all"
(4) remove selected
(5) print the gerber files
(6) quit pcb *WITHOUT SAVING CHANGES*
(7) change the name of the gerber file having the route output to something
like "myroute.gbr"
so it won't be overwritten
(8) launch pcb and re-load your design.
(9) print the gerbers normally
(10) chuck the new gerber cooresponding to the route layer ('cause it has
pads in it)

Yeah, it's a kludge. I got to fix this some day, probably when we expand the
layer count and a dedicated
route layer.

harry