Hello Matt, The power plane clearances are not proportional to a hole size. ie, the gerber d-code used to plot the void on the plane layers will be your requested clearance + hole size. For example, lets say you have a via with an 18mil hole. The gerber d-code used will be the specified clearance (let's say 20mil) + 18mil. So a void of 38mil will be on your plane layers around vias with that hole size. If you have a 126mil mounting hole, then the void placed on a plane layer for this feature would be 146mil. It can get confusing if your copper pad sizes (in your case - the top and bottom layer pad sizes) are proportional to your hole sizes. It will look like your plane clearances are shrinking as your hole features get bigger, and in some cases may appear to disappear all together.
Hope this helps. Cheers, Gareth. -----Original Message----- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] Behalf Of Matt Polak Sent: Friday, 4 March 2005 2:02 PM To: Protel EDA Discussion List Subject: [PEDA] DXP: Non-proportional clearance expansion on power planes? Hey guys, Got a weird one here. I'm doing a four-layer board (basically finished) and I've been tweaking up the power planes and things in the final check. I noticed something that seems very odd. In the Rules, I have the default "20 mils" set for Plane Clearance. Around all of my smaller holes (e.g. 20 mil vias), when viewing the power planes, the clearance pullbacks on the power planes are just fine. When I look at some larger mounting holes, though, such as 120 mil for DB-25 connector stress reliefs, the clearances (though still set 20 mils) are hardly even visible! The larger the hole gets, the thinner the clearance around it - it's like the clearance is NOT proportionally scaling to the hole size! If I temporarily change the Plane Clearance rule to, say, 50 mils, all of the smaller holes get extremely overkill clearances (obviously) but then at least a thin line appears around the larger holes. I've had multi-layer boards manufactured before (under 99SE) using these same exact parts and clearance rules, and didn't have a problem with them, which is making me wonder if this is a Protel display problem, or if my board house caught it and pulled them back more. I'm about to generate a set of Gerbers to look at to see if this is a legitimate output problem, or just an on-screen display problem. Anyone had this one happen before? Suggestions? Regards, -- Matt ____________________________________________________________ You are subscribed to the PEDA discussion forum To Post messages: mailto:[email protected] Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[email protected] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/[email protected] ____________________________________________________________ You are subscribed to the PEDA discussion forum To Post messages: mailto:[email protected] Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[email protected] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/[email protected]
