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

[sdb@xxxxxxxxxx (Stuart Brorson)]

Harry --

Thank you for your quick and accurate reply.  Indeed, my problem was
that I had only the GND polygon on the back, and PCB was rendering it
as a negative plane.  The board house wants positive planes on all
external layers.  Is that non-spec?

Questions:

1.  Is there some way we can force positive or negative rendering?
Perhaps a pop-up "layers" menu with check boxes for pos/neg?  Oh oh,
here goes the whole PCB layers debate again. . . .    :-) 

Maybe I'll create such a pop-up when the GTK port appears.

2.  A totally different question:  In the fab drawing, my name and the
board title are displayed.  Where did it get my name?  I didn't enter
any info for that to happen.  Also, the title is "unknown".  How do I
enter that info?

Thanks,

Stuart



> 
> 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
> 
>