Re: gEDA-user: PCB Panelisation and outline layers

[DJ Delorie <dj@xxxxxxxxxxx>]

DJ's Panelization Scripts:

http://www.gedasymbols.org/user/dj_delorie/

pcb2panel - combines boards into a "panel" board (outline for each
	board as an element) for easy editing).

panel2pcb - reads panel board and input pcb's, produces a composite
	panel pcb.

Although I've never done so, I assume the "panel" board could be
easily generated from a script, allowing you to automate gridded
panels.

I just a few days ago added an "outline" layer to PCB's default
stackup, and magic code to insert a rectangular boundary if it's
otherwise empty.  I'm not sure how it will interact with the
panelization script, or how it *should* interact - do you want the
outline gerber to have the overall outline, or the outlines of the
individual boards?

PCB's "board" dimensions are actually the dimensions of the work area.
In the absence of an outline layer, it assumes that's the board area.
It should produce a "fab" drawing with an outline on it; if you have
no other outline, send them the fab drawing.

Also: note that naming a layer "route" is a synonym for "outline" -
don't use that to mean something else.  "vgroove" is not a special
name; pcb assumes it's yet another copper layer.

As for arbitrarily combining layers, I suggest scripting something
that changes the Groups() line in the .pcb (to a temp file, of
course), a running "pcb -x gerber ..." to plot the various
combinations.  Sadly, we don't have the ability to export arbitrary
cam jobs like the Big Boys.

Another option is to look at gerbv and see if it has merging
capabilities.  I know PCB is careful to use a consistent set of
apertures across gerbers; a perl script should be able to merge
gerbers from pcb without too much work.


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