X-Authentication-Warning:	delorie.com: mail set sender to geda-user-bounces using -f
X-Recipient:	geda-user AT delorie DOT com
X-Envelope-From:	paubert AT iram DOT es
Date:	Thu, 15 Jan 2015 09:58:08 +0100
From:	Gabriel Paubert <paubert AT iram DOT es>
To:	geda-user AT delorie DOT com
Subject:	Re: [geda-user] Unable to do a groundplane
Message-ID:	<20150115085808.GA22124@visitor2.iram.es>
References:	<2ae7289c4c348400d76b5abcd8dfd5e4 AT webmail DOT schinagl DOT nl>
MIME-Version:	1.0
In-Reply-To:	<2ae7289c4c348400d76b5abcd8dfd5e4@webmail.schinagl.nl>
User-Agent:	Mutt/1.5.21 (2010-09-15)
X-Spamina-Bogosity:	Unsure
X-Spamina-Spam-Score:	-0.2 (/)
X-Spamina-Spam-Report:	Content analysis details: (-0.2 points)
	pts rule name description
	---- ---------------------- --------------------------------------------------
	-1.0 ALL_TRUSTED Passed through trusted hosts only via SMTP
	0.8 BAYES_50 BODY: Bayes spam probability is 40 to 60%
	[score: 0.4632]
	0.0 URIBL_BLOCKED ADMINISTRATOR NOTICE: The query to URIBL was blocked.
	See
	http://wiki.apache.org/spamassassin/DnsBlocklists#dnsbl-block
	for more information.
	[URIs: schinagl.nl]
Reply-To:	geda-user AT delorie DOT com
Errors-To:	nobody AT delorie DOT com
X-Mailing-List:	geda-user AT delorie DOT com
X-Unsubscribes-To:	listserv AT delorie DOT com

On Thu, Jan 15, 2015 at 08:43:21AM +0100, oliver+list AT schinagl DOT nl wrote:
> Hey list,
> 
> For some reason, i am suddenly no longer able to fill a plane for
> ground in PCB correctly. I can draw the rectangle as I normally do
> around my routed single sided PCB, and at first glance, it looks
> like everything worked out allright. But on further inspection, the
> center traces all get flooded and become useless.
> 
> I've attached the file to demonstrate this, removing the plane is
> easy and should show how the PCB was intended to look.
> 
> What am I doing wrong?

Many of your "lines" (tracks) do not have the "clearline" attribute,
you probably had the "New lines, arcs clear polygons" option off
in the "Seetings" menu when drawing these lines.

A first possible fix is to edit the PCB file by hand and insert a 
"clearline" attribute in every line that defines a "Line" and does 
not already have this attribute set (not very hard to script).

However there are some cases where you want some lines to connect
to the ground plane (SMD pads to the plane for example). This can
easily be fiexd up after the facts and the ratsnest will help you
to find the lines that you have to join ("j" key under the GUI)
to the plane.

Another possibility is the GUI way: select "Thin draw poly"
(Ctrl+Shift+P) and type "j" while the mouse pointer over the
track segments that should not be connected to the ground plane.
At the beginning intermediate segments will not be visible 
(hidden behind the "thinly drawn polygon", something I consider 
a minor GUI bug) but by starting from a pin/pad and following
every track you'll hopefuly end up with the correct result.

    Gabriel

- Raw text -