This kind of edge where the board edge goes through plated holes and the holes are cut in the middle is called
- castellated edge
- plated half-holes
- semi-plated holes
It’s used in PCB modules which can be soldered to other PCB’s.
Castellation is made so that there are normal PTH pads first and they are surrounded by the board material. Then the board edge is milled or cut in some other way so that half of the holes are left. Cutting copper with milling bits is more costly, therefore castellation often costs more for you.
In general, there’s no special support for this in KiCad v5, nor in the Gerber X1 format (X2 has meta-information attributes, including CastellatedPad, but isn’t universally supported by all manufacturers yet). The board manufacturers usually interpret certain kinds of gerbers as having castellation. Basically it needs nothing else than PTH pads – holes and some copper on and around them – on the board edge.
(There’s no support for castellation in v5.1 3D viewer, either, which is good here because we can see that it’s just normal PTH pads.)
You can do this easily if you ignore the DRC in KiCad – allow DRC violations while routing and just ignore the DRC check errors with tracks which go too close to the edge. In the next post we will see how castellation can be made with KiCad so that it’s possible to route it without DRC problems and without ignoring DRC.
Here it’s important to notice that castellation isn’t cheap, so you may want to avoid it if possible. It easily multiplies the board price by 5 or 10. Sometimes you can consider avoiding the cost by surrounding the hole with an extra piece of board which you cut off manually yourself (with reduced quality and chance of breaking the board, of course, but for cheap prototypes this could be acceptable).
Castellation is a matter of interpretation and manufacturing capabilities. Never trust generic advice blindly, always check what your manufacturer wants and is capable of doing. See for example what OSH Park says:
the castellated vias must be indicated with round pads for copper and stop mask. The pads must also not extend more than 40 mil from the board edge. Square pads or pads that extend far beyond the edge will be trimmed, and the via will not be plated.
Some manufacturers require checking Castellation option when you make the order or they don’t plate the holes.
Find also other technical requirements of your manufacturer. The minimum hole diameter may be e.g. 0.6 mm. Holes must have enough edge to edge clearance, but your pitch requirement comes more probably from other mechanical considerations – for example fitting for standard pin headers.