Personally I use the global pcb controlled soldermask as that is what the fab house tells me they’re capable of. Having clearances of less than that in any of the many footprints I use will be a problem for me that I like to avoid.
I naturally understand people that do layout 100% all day as their job - people who breath this - so for them to control the clearance for each pad might be what they need and can do.
So, to cater to all and give the user the freedom (we have that rarely with KiCAD) to do what he want’s to do, and not being nannied I support the current implementation and would oppose any changes.
I must agree with @Joan_Sparky. Soldermask swell really should be defined globally, driven (at the present time) by the capabilities of the board fab. (That means you just might have more mask clearance when you get a dozen prototype boards made by a quick-turn shop, and a tighter mask when a thousand get made for the low-rate initial production.)
There ARE places where mask clearances get adjusted for special reasons - the bearing surfaces around mounting holes, or the thermal pads under some IC’s, for example - so I want the option to override the global setting on a pad-by-pad basis but at least 99 times out of 100 I want to stay with the global, board-wide, setting.
As I said the first time, just open up your own github footprint repo and advertise it to people and try to do a better job.
I’m not affiliated with the KiCAD lib people in any way and all footprints I use I make myself, so I don’t even have a chip in this game.
They set the rules for their libs… I don’t need to use them, I don’t need to like their libs.
And sometimes it’s just easier to ignore what is irritating you than to try to get a camel through the eye of a needle -
But I like the option to be bale to define clearances per pad, footprint or board and the rules which setting overrides the other are logical and useful.
I really don’t see a problem from a technical point of view.
Nowadays in professional environment (e.g. IPC-7351C) soldermask openings in library footprints are defined to be exactly the same as pads themselves. And PCB manufacturer adjusts it according to their capabilities when they process customer’s Gerbers or ODB++.
I always set the global solder mask clearance to 0 and let the board house open it up to match their capabilities. If I need something fancy, I set it per footprint or even per pad / draw a zone on the mask layer…