That’s why copper fills/pours are set back a bit from the edge.cuts - see their options when you create one.
If that’s not enough (or doesn’t give you expected results) you can also place no-fill zones.. I think on the pcbs below some of those NPTH holes would have caused ripples/waves in the copper zone edge, so I placed no fill zones over some of them to get straight edges.
As for routing through a little bit of copper - I didn’t had problems the last two times I did castellations at Elecrow, where the router was going through PTHs for a short stretch (even 2 different fab houses, as certain details aren’t the same). Mind you the router was 1mm in diameter though.. as those where at board edges - but you can see the copper pour stopped before the board edges at any case (top left, bottom right):
The footprints I used have the edge.cut layer marked on the cmts.user layer. I went for the biggest hole size I could get away with while still getting some copper around it on the pcb after considering accuracies of drilling etc. to stabilize the copper that is being cut away. As you can see on the picture, some PTH copper has not been cut but squeezed into the half-hole - it’s pretty easy to get that out with some sharp pointed tool.
KiCADinfo_Castellations.pretty.zip (1.2 KB)
Those are called mousebites.. have a read here for some guidance/info about them:
NPTH footprints I use for mousebites:
KiCADinfo_Mousebites.pretty.zip (2.3 KB)
Afaik, the factory will treat completely separated pcb pieces - even if they come from one set of gerbers - as single pcbs and charge you more.. thus people arrange them and keep them together, but make them easily separable. Some fabs don’t appreciate that and still charge you for separable pcbs though (more milling = longer time and more wear on router bits) but most Chinese fabs don’t care it seems (or it’s already priced in) and don’t charge you extra.
Another reason for this is if you want to use surface mount devices and have a solder mask made from the gerber set.. it’s easier to handle the complete piece, rather than smaller ones, and break apart after reflowing the whole thing.
As for having the copper pour also on the inner parts that are separated by break-away-tabs - you need to have some footprints or tracks going there to connect the fill-areas with the nets. The tracks can traverse edge cuts, no problem, it just won’t look nice where they leave/enter the board.
Or you can put down a separate fill area for the inner parts as I did here - adjust the priority level in the areas options dialog when you do this, otherwise it won’t fill or even be create-able if it overlaps another one.
Do you have a screenshot of what you have in mind?
In any case, make sure that the lines/arcs on the edge.cuts layer meet each other down to 0.1 mm I think - check with gerber viewer tools to make sure your edge cuts are closed (some can’t deal with nested edge cuts though, look at the link where I posted some tests). For simple 90 deg shapes/corners this can be done in pcbnew, but for anything more complex you want a CAD program that exports dxf that you can import into pcbnew (above example).
You also don’t need to round any internal corner unless the radius shall be greater than half the diameter of the router bit being used (usually minimum of 0.8 mm possible, 1 mm and up are more common) - that’s why I have sharp corners in there (makes closing the edge cut loop a breeze and doesn’t affect the outcome).