Mounting holes are a bit of a minefield. In the 2009 edition if you made the pad the same size as the hole (thinking you would just get a hole), but had zones on more than one layer covering the hole, kicad would take the copper pours right to the edge of the hole. Most boards of more than one layer require through-hole plating, so when the board manufacturer put the board through the through-hole plating process the power planes would end up connected together via the mounting hole plating. Since kicad had no knowledge of this the board would pass the DRC only to fail catastrophically when manufactured.
The 2010 edition corrects this by applying the design rules so that there will be a non-conducting annulus around the hole, preventing the short circuit. However, whilst better it is not ideal because the hole will still get through-hole plated but the plating will be unsupported. What is needed is a means of flagging holes that should not be through-hole plated so that two drill files get produced. Of course if you take advantage of that your board will have an extra manufacturing stage and will probably cost more. So unless it's essential that the the hole be completely non-metallic, it's probably best to give it at least a minimal copper supporting annulus and simply let it get plated. Although a little off-topic it's perhaps worth saying at this point that if the mounting holes is for a bolt, don't forget to allow in the PCB design not just for the bolt head but also the star washer that someone else will fit without your knowledge. When a power plane gets shorted to ground via the washer the PCB designer will of course get the blame even though the washer was never specified. Regards, Robert. On 16/08/2010 01:55, oecherexpat wrote: > Hi, > > If you try to make the hole larger than the pad you will get an error. What I > have been using in the past was to have the pad on NO copper layers. But in > the current version it also creates an error. > Maybe something to put as a suggestion.... > > Cheers, Heiko > > >> How about drawing a crosshair or circle as a silkscreen object and using >> that to mark the drill? Could also just make the copper pad smaller than the >> drill bit used so that it vanishes entirely when the hole is drilled. >> > > > > > ------------------------------------ > > Please read the Kicad FAQ in the group files section before posting your > question. > Please post your bug reports here. They will be picked up by the creator of > Kicad. > Please visit http://www.kicadlib.org for details of how to contribute your > symbols/modules to the kicad library. > For building Kicad from source and other development questions visit the > kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups > Links > > > > > > > No virus found in this incoming message. > Checked by AVG - www.avg.com > Version: 9.0.851 / Virus Database: 271.1.1/3073 - Release Date: 08/15/10 > 07:35:00 >
No virus found in this outgoing message. Checked by AVG - www.avg.com Version: 9.0.851 / Virus Database: 271.1.1/3075 - Release Date: 08/16/10 07:35:00
