You can: PCB Editor / Route / Interactive Router Settings and then set the Mode to Highlight Collisions and set Options to Allow DRC violations.
You can copy an (any!) existing track segment (this grabs it by an endpoint) and then snap it to one of the castellated pads. Creating an array of such segments also quickly get’s you away from the edge and the rest can be routed normally.
Your own workaround can also be simplified. You can skip steps 2, 3 and 4. Just changing the layer of the line on Edge.Cuts that triggers the violation is enough. It does mean the PCB outline is not a closed shape but that is not such a big deal.
I don’t like to have to Allow DRC violations, even briefly. But this is a good tip. And your improvement of my workaround is good too. Thanks for this solution. It will definitely accelerate my progress.
The simplest workaround is to just route a track to such a pad, instead of from it.
Nope, I also tried this and it does not help. This fabrication attribute seems to be ignored completely by the DRC. I created a test case for this and added it to the existing #1790 issue on gitlab, together with some comment.
I do not see why this should be defined on the footprint level.
In the test case I made, I did:
Use the wizard to create a DIP-8.
Set Fabrication Property / Castellated Pad (through hole only) for one pad.
From the popup menu: Copy Pad Properties to Default.
Select all pads and: Paste Default Pad Properties to Selected.
So it’s just a handful of mouse clicks and this seems quick enough to me for designing footprints. Also adding this to the footprint level would just make it more complicated and create room for confusion.
If I place a small, SMD pad inside the THT pad I can have a second starting point for the trace that is off center and this allows the routing from there
