X-Authentication-Warning:	delorie.com: mail set sender to geda-user-bounces using -f
X-Recipient:	geda-user AT delorie DOT com
X-Injected-Via-Gmane:	http://gmane.org/
To:	geda-user AT delorie DOT com
From:	Kai-Martin Knaak <knaak AT iqo DOT uni-hannover DOT de>
Subject:	Re: [geda-user] possibly dumb PCB question
Date:	Tue, 20 Jan 2015 12:48:55 +0100
Organization:	Institut =?UTF-8?B?ZsO8cg==?= Quantenoptik
Lines:	63
Message-ID:	<m9leui$bpk$1@ger.gmane.org>
References:	<54BDF302 DOT 9030903 AT neurotica DOT com>
Mime-Version:	1.0
X-Complaints-To:	usenet AT ger DOT gmane DOT org
X-Gmane-NNTP-Posting-Host:	130.75.103.107
User-Agent:	KNode/4.14.1
X-MIME-Autoconverted:	from quoted-printable to 8bit by delorie.com id t0KBgOhj024683
Reply-To:	geda-user AT delorie DOT com

Dave McGuire wrote:

> Hey folks.  I am drawing a footprint for a surface-mount component
> that has two pads with fairly wide spacing between them, and I must not
> have any copper (i.e., from the power/ground planes) between them.  Is
> there any way I can specify this in the footprint?

Pads have a property called "polygon clearance". You can manipulate it in 
the GUI. Put the mouse above the pad and type [k]. This shortcut increases 
the clearance by an configurable amount. An overlapping polygon will 
recede to the new increased the minimum distance is reached. Repeat until 
the spacing in between the pads is open.
You can type [shift-k] to decrement the clearance.

If you wish total control over clearance, you may consider to use a text 
editor and directly set the numerical value. Polygon clearance is the 7th 
parameter of the pad statement. Recent versions of pcb happily accept 
values with real world units like "1.60mm".

This approach will result in a wide clearance all around the pads. If you 
need small clearance on the outside, but large enough clearance on the 
inside to clear the gap, you can go for composite pads. Make the original 
pad with small clearance. Then add a narrow strip on top of it. Place the 
strip near the inner border of the main pad. Increase the clearance of the 
strip as necessary to clear the gap.
Attach the same pin number / label to both objects. That way, pcb 
connectivity check will treat the combined shape like it were a single pad 
with a more complex geometry. This trick works with pins, too. 

BTW, make sure, mask clearance is set to a proper value. You most probably 
don't want a large unmasked margin around pads. I habitually set mask 
clearance to 0.1 mm in my footprints.

Hope that helps,

---<)kaimartin(>---
-- 
Kai-Martin Knaak                                  tel: +49-511-762-2895
Universität Hannover, Inst. für Quantenoptik      fax: +49-511-762-2211	
Welfengarten 1, 30167 Hannover           http://www.iqo.uni-hannover.de
GPG key:    http://pgp.mit.edu:11371/pks/lookup?search=Knaak+kmk&op=get

- Raw text -