Re: gEDA-user: Ground-plane in Pcb

[Tuck Hartshorn <tuck@xxxxxxxxxx>]

On Saturday 23 December 2006 03:27, Harry Eaton wrote:
>
> 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)".
ok, now what?
(btw, why is there no ":DisplayFlag(selected,join)" ?)

> 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.
the command ref says the "s" key will increase the size of a TLAPV, which it 
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,
After playing around, I thought that was probably the case.

> 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.
Got that.

Ok, Harry. I did the "changeFlag" thingy  (That's my Will Smith coming out) 
and, that did the trick!
Grabbing the tracks, (not the nets), resetting the join flag and "pouring" 
copper, works just fine.
That sounds like a very useful technique that I can't find in the docs (other 
than the command reference), or in previous posts--at least for the last 9 
months.

Anyway, tnx to both you and DJ.
Tuck

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


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