Perhaps “limited” is not the right word- tedious perhaps. I had to draw 20-30 lines to get the outline I wanted, plus some more to make the left and right edges not be “frilly”. If I want to change it, I’ll have to delete some lines, maybe reset my grid and line width, and then re-draw what I want.
In the end I got exactly what I wanted, once converted to Gerber, it is just a region, all the history of lines etc is left behind.
You can add filled “zones” to footprints, just not through the footprint editor. Try opening the kicad_mod-file in a text editor. They are highly human readable. There is a polygon entity in this form
(fp_poly (pts (xy 3.5 -3.5) (xy 3.5 3.5) (xy -3.5 3.5) (xy -3.5 -3.5)) (layer F.CrtYd) (width 0.2))
You don’t need to specify going back to the first corner, polygons are closed by default. The width value adds a trace of that width around your polygon. Meaning your corners will have a nice radius. You’ll need to keep in mind it also expands the polygon by half the width value.
Copper pours for nets can’t be added this way though. There is no way of relating them to a pin number. You can add polygons to copper layers, but they won’t quite behave. They will interact more in a graphic item way than a copper item way.
1 Like
I have the same problem, I think the simplest way to deal with it would be to allow the copy between layers… (for all layers).
And the job is done, and I don’t think this is a feature that hard.
Locking up the copy between layer is a design error IMHO.
Old old old thread…
Copying a filled zone from copper to non-copper layer would be mostly meaningless. Anyway, you don’t say what you should be able to copy.
There are meaningful copies and there are meaningless copies. “Feature that hard” – you probably don’t know anything about KiCad internals, so you can’t tell what’s hard and what’s not. KiCad has been designed to do meaningful things in PCB design. Allowing anything imaginable isn’t meaningful.
I don’t know if graphical polygons existed back when this thread was started, but that is how one would create a rectangular (or any odd shape) hole in the mask layer with the current KiCad. The difference between (and why the two exist separately) a filled zone is intended to be an electrical connection amongst members of an electrical net. A graphical polygon is just that, graphical. It doesn’t know or care about electrical nets (and thus is dangerous to put on electrical layers).
One can easily put a graphical polygon on a mask layer to cut a window of the shape of that polygon out of the mask. When this is done for footprint reasons it is probably best to put this mask-layer polygon as part of the footprint so when the footprint has to be nudged slightly to make room for routing the mask-layer polygon maintains it’s registration with the footprint. Though, when putting the hole in the mask as part of the footprint (especially for thermal pads where there wants to be copper exposed) one just uses a SMT pad with the mask layer turned on.