Re: gEDA-user: Ground-plane in Pcb

[Harry Eaton <bumpelo@xxxxxxxxxxx>]

Tuck Hartshorn wrote:

> On Friday 22 December 2006 20:37, DJ Delorie wrote:
>  
>
> > > latest as in cvs?
> > >      
> I got cvs but it failed to make completely. The current cvs is missing 
> some .pngs  in the ./doc dir, namely  puller.png and thermal.png
>
> But, I thought the binary might be ok, anyway. And, it does seem to work. 
> Shows version 1.99u instead of 20060822.
> It seems no better and it did not make isolation islands over existing nets.
> tuck
>  
All of the "nets" (a misnomer; they are tracks) that you've already 
drawn apperently
already have their join flag set. That is they have been told to touch 
any polygons they encounter.
It seems you wanted to draw them with the "new lines arcs clear 
polygons" setting checked.

No problem, simply select all lines then enter the command 
":ChangeFlag(selected,join,0)".
Now all of the lines are told to clear the polygons. Another (unlikely) 
possibility is that you have
flagged the polygon to not allow anything to make clearances in it. You 
can't create polygons with
that property to begin with, but you can give (and take) that property 
with the "s" key.

DJ misunderstood your problem. Older versions of pcb were perfectly 
capable of making
clearances in polygons around tracks, it just did not understand that an 
isolated island
created by clearing regions of the polygon was no longer electically 
connected to the other
parts of the polygon. The new version does.

Another important point is that the "gnd-solder" is nothing more than a 
name. It has no
meaning, you can change that name to anything you like and it won't make 
any difference,
except for the two special names "route" and "outline". Pcb has a 
strange feature allowing
grouping of layers into a single physical copper layer; people use that 
to color-code tracks.
When layers are grouped, turning off/on visibility of one layer in the 
group will do so for
all layers in the group. This is one hint that layers are grouped, but 
you should look at the
layer grouping dialog to truly understand which layer is where.  If 
"gnd-solder" is not
grouped with "solder" then don't expect tracks on the "solder" layer to 
clear a polygon on
the "gnd-solder" layer.




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