These are all difficult technological question, I'll try to answer to them but of course YMMV...
> I've been writing up some documentation and can't find where the delta's are > entered for the masks. In the old kicad there was a mask offset, in the new one its set in the design rules, with solder paste offset too. > Normally, the hole in the solder mask is made slightly larger than the pad - > 5mils and the mask for > paste is slightly smaller. That's depend on the manufacturer equipment. Some board manufacturer do photo resist, other ones silk resist (for cheap boards :D), and some even adjust automatically the resist flash to give the correct coverage. There are similar issues with solder paste, since it depends on stencil thickness *and* cream gauge/composition. Usually you provide a stencil big as the pad and the manufacturing facility adjust it. This isn't true for big pads (i.e. thermal bonds on CSP) which should be only partially covered with paste (usually about 30%, the chip manufacturer usually gives the recommended solder pattern). For example, for our current board maker I have to send the gerbers with both offset to zero. With the previous one I had to apply solder mask offset but not the solder paste one. > I can think of a way to create a module with extra pads with number zero to > achieve this, but these > numbers must be set someplace? You use extra pads for special stuff, like extended masking or stippled cream. Your idea is correct but there is no need, kicad is able to automatically apply simple offsets to the pads. > There should also be a place to enter drill deltas - the module should > specifiy the finished hole > size - depending on the manufacturers needs the drill list should oversize > the holes slightly to > account for the plate-thru. Where are these numbers? This must be took in account by the manufacturer. The drill tape *always* indicate the *finished* hole size. Drill compensation for plating is done by the board manufacturing facility. And bigger/oval holes are actually milled so there is no way you can think about it before :P BTW what is missing now is a way to specify a second/third drill pass hole (i.e. unplated holes, drilled after metallisation). > I'm also noticing that no one uses the adhesive layer in the libs - is there > a reason? The reason is that these days adhesive isn't used except for special productions... it's main use is to keep components down during *wave* soldering. SMD is now usually done using *reflow*, where components are kept by the solder paste (and, BTW wave soldering requires different pad shapes and cautions in component placement and orientation). As a result adesive is today used for, I think, only two things: - Keeping components on the underside when reflowing dual mounted boards in one pass (but then is usually better to reflow twice with two different temperatures) - Keeping components during wave soldering when you have a board with SMD on both sides and a lot of THT components too (you wave the THT and the glued SMD in one pass, after reflowing the upper side components). Please note that these are both somewhat specialized circumstances, requiring special modules anyway.
