Re: gEDA-user: Can't truncate plane layers on backside?!?!?

["harry eaton" <bumpelo@xxxxxxxxxxx>]

Stuart,

What you have is most likely a "negative image" plane.

Some vendors complain about "composite layers" which pcb normally produces
whenever polygons
exist. In order to support the many people that have asked to be able to
produce negative images for
simple ground and power planes, pcb treats "simple" planes as a special case
in order to avoid
composite layers.

A negative image assumes that everywhere is copper except for clearances
around pins and vias in the plane.
It is produced only when:

(1) The layer has exactly 1 polygon and
(2) All pins and vias pierce the polygon and
(3) There are no lines or arcs on the layer

Originally I inteded to also require that the polygon fill the entire board
area but it turns out that this
can be hard to achieve when you want to do it. I should probably add a check
box in the print
dialog so that negative planes are only produced when the above are met and
you ask for them.

In order to get the polygon you want, what you should do is to simply draw a
hidden line in the middle
of  the plane that touches it. Set the settings so that new lines join
polygons, then draw a line in the plane
away from any vias or pins. You will not be able to see the line once it is
drawn, but its presence
should prevent the special negative-image gerber from being generated, thus
you will get what you
want.

This would not be an issue if every vendor would just simply accept anything
that meets the RS274X
Gerber specification, but many don't.

harry

"----- Original Message -----
From: "Stuart Brorson" <sdb@xxxxxxxxxx>
To: <geda-user@xxxxxxxxxxxxx>
Sent: Tuesday, February 22, 2005 10:16 PM
Subject: gEDA-user: Can't truncate plane layers on backside?!?!?


> Hi PCB hackers,
>
> I have created a simple PCB with a back-side GND plane.  I define the
> plane  using a polygon drawn on the solder side.  The polygon
> terminates about 100 mil before the edge of the board.  That is, the
> GND plane is 100 mil smaller than the PCB outline along all four edges
> of the board.
>
> When I export the Gerber file & view it, the GND plane extends to
> infinity.  However, I though I drew it to be smaller than the PCB
> outline.  Um, what am I doing wrong?  Or have I found a bug?
>
> If requested, I can post a .pcb file & some Gerber snapshots.  But
> maybe this is just newbie confusion. . . . .
>
> Stuart