Steven, On 4/28/2018 11:10 PM, Strontium wrote: > Wayne, > > I think it is an acceptable solution for V5 because this shouldn't get > in the way of a V5 release. > > For V6, would it be feasible to define 0.000001/0.00001% to be a special > value (like zero) which means "effectively zero" and then the pad gui > can be updated with this special knowledge so that users don't look at a > pad and say "Why is this set to 0.000001??" and then change it thinking > its a rounding error or something. > > I am not a fan of coded values in gui's because the whole idea of a gui > is to abstract the implementation details into something human friendly. > And 0 meaning "inherit", and 0.000001 meaning "effectively zero" is an > implementation issue and not something the user should have to know or > think about.
I would rather not use magic values. They make the file format less human readable which is a design goal with any kicad format. The person reading the file would have to know that 0.000001/0.00001% meant do not apply clearance and/or ratio to the pad. I would rather use a flag such as no_clearance and/or no_ratio to ignore the normal priority. This makes it clear that that clearance and/or ratio calculations do not get applied to the pad . > > Actually, it would be nice in the pad gui, if it IS set to inherit that > the field display a READ ONLY value that would be used NOW based on the > current global/parent settings, and which is it (a global value or a > parent value). > > Steven > > > On 28/04/18 23:35, Wayne Stambaugh wrote: >> Just to be clear, the library developers are asking for the ability to >> ignore clearance and ratio settings when creating solder mask and >> solder paste only pads. If this is the case, it will require a board >> file format change to add a flag to ignore the global and footprint >> level settings. I would be opposed to changing the code to just >> assume that if it's a solder mask or solder paste only pad that no >> tolerance or ratio is applied. This would break an existing pads >> defined this way and silently change existing boards. Given that we >> are deep into feature freeze, the least painful solution would be to >> set the tolerance to 1nm and the ratio (as JP suggested) to 0.00001% >> for the footprints that need to maintain the dimensions of solder mask >> and solder paste only boards. The change to the overall pad >> dimensions using this method would be far below any board >> manufacturer's tolerance capabilities. Is this not an acceptable >> solution? >> >> Cheers, >> >> Wayne >> >> On 04/28/2018 08:44 AM, Eeli Kaikkonen wrote: >>> >>> >>> 2018-04-28 15:04 GMT+03:00 Rene Pöschl <poesc...@gmail.com >>> <mailto:poesc...@gmail.com>>: >>> >>> The global settings here are less for ensuring correct alignment and >>> more for a global paste reduction. >>> >>> >>> That's right, that's what I meant. In the example datasheet you have >>> 0.05mm tolerance for the location of the mask in relation to the >>> copper because. But making the mask openings larger or smaller by >>> 0.05mm would be against the recommendation. >>> >>> It just doesn't make sense to apply global paste and solder mask >>> clearance values to "pads" which don't have copper. The whole reason >>> why non-copper pads can exist is that you need control over the size, >>> shape and location of paste or mask, right? Changing the behavior >>> could lead to problems but luckily the current behavior can be >>> circumvented by adding to clearance fields a very small value which >>> is negligible in practice. >>> >>> Eeli Kaikkonen >>> >>> >>> _______________________________________________ >>> Mailing list: https://launchpad.net/~kicad-developers >>> Post to : kicad-developers@lists.launchpad.net >>> Unsubscribe : https://launchpad.net/~kicad-developers >>> More help : https://help.launchpad.net/ListHelp >>> >> >> _______________________________________________ >> Mailing list: https://launchpad.net/~kicad-developers >> Post to : kicad-developers@lists.launchpad.net >> Unsubscribe : https://launchpad.net/~kicad-developers >> More help : https://help.launchpad.net/ListHelp > > > > _______________________________________________ > Mailing list: https://launchpad.net/~kicad-developers > Post to : kicad-developers@lists.launchpad.net > Unsubscribe : https://launchpad.net/~kicad-developers > More help : https://help.launchpad.net/ListHelp _______________________________________________ Mailing list: https://launchpad.net/~kicad-developers Post to : kicad-developers@lists.launchpad.net Unsubscribe : https://launchpad.net/~kicad-developers More help : https://help.launchpad.net/ListHelp
