Re: gEDA-user: Making a board: what's next?

[DJ Delorie <dj@xxxxxxxxxxx>]

> (1) How do I mark drill holes for mounting the fabricated board? Are 
> they just vias?

You can do it with vias or real symbols.  Most people create a
"mounting hole" symbol and add as many to their schematic as they need,
and give it a suitable footprint.  For example:

http://www.gedasymbols.org/user/dj_delorie/symbols/nvconnector/right-screw-term.sym

That puts all the footprints on the board, then you place them in the
right locations.  Usually such footprints consist of a single pin with
a drill hole bigger than the screw, and a copper diameter bigger than
the washer.  I've attached a 2-56 one.

> (2) How do I indicate the size of the board?  Right now I just drew a 
> silkscreen border.

Two ways.  For simple boards, set the board size in the "board sizes"
dialog (edit->board sizes for lesstif).  That sets pcb's working area
to "the board".  The advantage here is that the coordinates in the
toolbar are board coordinates.

Otherwise, rename one of the unused layers to "outline" and draw your
outline on that.  This layer is treated slightly special, in that it
will use it to draw the outline on your fabrication drawing.

> (3) The next step if fabrication, can a company like pcbexpress.com
> handle output from the gEDA suite? Or are there other companies
> known to be gEDA-friendly?

I've used advanced circuits (4pcb.com) and pcb-pool.com without
needing to do anything with the gerbers.  Sierra (protoexpress.com)
wants the outline on the solder mask, which requires a patch I've
posted here before.  For 4pcb, offer the "fab" drawing as the
fabrication drawing.  I don't recall what pcb-pool wants.


Element["" "" "MH1" "" 0 0 -5000 12500 0 100 ""]
(
	Pin[0 0 22500 2000 23100 9340 "1" "1" ""]
	ElementArc [0 0 12500 12500 0 360 1000]
)


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