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 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: References: <54BDF302 DOT 9030903 AT neurotica DOT com> Mime-Version: 1.0 Content-Type: text/plain; charset="UTF-8" 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 Content-Transfer-Encoding: 8bit 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