So I imported an image to Usr.Eco1, then opened the footprint and moved the polygons from Usr.Eco1 to F.Cu. Next I placed that onto my PCB, make a zone telling to not fill inside of the graphics and another copper fill zone over the whole PCB.
And here the issue starts: No matter what I try, I can’t bring the copper zone to connect to the graphic:
The errors are ignorable / it is printable like that but having these errors sounds just wrong. So what’s the correct way to connect the copper zone to the footprint graphic without creating DRC issues?
In KiCad V7 graphics are treated as separate entities that are not part of a net, and therefore the zone does not connect to it. In KiCad-Nightly V7.99 it is apparently possible to directly assign a net name to graphics on a copper layer, but I have not tested this myself yet.
It is possible to add graphics to a pad in KiCad V7. To do this you have to design a footprint, import the graphics, add a pad (It must overlap with the graphics), and combine graphics and the pad into a custom pad by entering and exiting the Pad Edit Mode [Ctrl + E].
It’s all GND. The footprint graphic is surrounded by GND. I also thought about this beeing a net issue but can’t find a way to assign the footprint or the copper polygones of the footprint to a net.
//EDIT: @paulvdh Sorry, I overlooked your answer. That sounds exactly like what I need, so thanks a lot.
//EDIT²: Needed a bit more time as I used the chance and edited the polygones a bit so min spacing etc. is now enforced inside of the graphic, too. Anyway, the solution to make a custom pad out of it worked like a charm:
Another small refinement. By default KiCad enlarges the net name to cover most of the pad, but it is possible to put it in some kind of text box to give it a defined size. This makes your graphics better visible in KiCad. I only read this on this forum, I’m not sure about the details of how to do this.
