Background: I have recently used the footprint editor successfully to design and order a through-hole pad with an oval hole shape.
Now: I wonder how to make a U- or C-shaped plated slot using KiCad 8 or newer?
Specifically I would like to try make a different footprint for the XT60 connector, which is like a half-cut-pipe. For this half cut pipe, I would like to create said C-shaped slot. I tried the circular default footprint before but I would like to iterate and test a new C-shaped version. How do I proceed?
The Aisler guide wasn’t too helpful
you probably make a through hole with a cut through it and add a note to the manufacturer about the details. For such “out of spec” things it is always best to talk with the manufacturer. I don’t think there is a native way to define plated cuts in KiCad
I’ve never had one of these things in my hands, but from the pictures I see online, it seems that enough of the ‘uncut’ section of the pipe remains to positively register in a round hole.
Reading carefully this guide shows the solution preferred by Aisler for plated slots: “Older legacy tools (like EAGLE) do not have this functionality, designers using such tools have to create a plated slot by drawing the slot using the milling layer inside a copper fill”.
So if you want to use Aisler for your board productuction then:
draw half-cut-pipe slot on the edge.cuts layer
draw a copper shape which is slightly larger than your plated slot
use gerber files for production, so Aisler can’t say if the files are from eagle or from kicad
maybe write an additional note
AISLER is not alone with this proposed solution. My preferred pcb manufacturers (multi-pcb + aetzwerk) work with a similar approach. (documentation see: Plated-through slots (slits) - Multi Circuit Boards)
I’m not 100% sure if it’s possible to draw the “slightly larger copper shape” already in the kicad FP editor, but at least it’s possible to add this graphic shape later in the pcb editor.
Note also that this solution will violate the “copper to edge” clearance constraint, so you will get DRC errors later in the design process.
This picture shows a quick made example. polygone drawn on edge.cuts, then two polygones on TOP+BOT copper surrounding the slot.
Sorry for the late reply - indeed you are right. in my application, the Connectors are unfortunately offset due to space constraints because of other larger connectors on the same PCB, but luckily a solution was provided by mf_ibfeew. Thanks!
