I would like to know how to go about making a padded open-ended slotted hole on the edge of a PCB (see image below).
I was thinking about making the slotted hole on the Edge.Cuts, then adding a standard padded mounting hole footprint on the circular part of the slot.
Any thoughts? Thanks.
Because it’s a slot and not just a common half-hole used in castellated edges I suggest you ask your manufacturer. See also Castellated edge; plated half holes in board edge. (As it happens, I wrote it earlier today.) As far as the gerber interpretation goes, I don’t see any difference, but it may be mechanically different for the manufacturer because it’s routed, not drilled. Better be sure they are willing to do it, and know the price beforehand.
Thanks for your info and advice! I was thinking that although the slot gives a bit more degree of freedom for mounting, it’s probably just for aesthetics than anything else I feel. From your post though, the cost multiplier doesn’t sound great, so I may rethink including it in my board.
If I decided to go the slot route, would you know how I would go about making the pad for this slot in KiCAD/PcbNew (assuming there’s no footprint in the standard library already to my knowledge)?
• As you guessed;
• Draw Edge Cutout on Edge_Cut layer.
• Draw same shape on a Silk layer (doesn’t really matter as you’ll move it to Copper layer). Use the Graphic Polygon tool and Offset the outer loop.
• Double-click the Graphic Polygon and select desired Copper layer to move it to.
Quick example, below… with it on the Bottom Cu layer. I didn’t fuss with exactness/dim’s…
Thus; a PCB with and edge cutout that is typical (not any different than any other PCB with a particular shape). And, a copper fill or, in this case as I did it, a Graphic Polygon (which is what is used for making a custom Copper fill unless loading a custom graphic…)
Thanks for the detailed explanation! It’s simpler than I thought now that I think about it.
Even simpler is to just add an oval pad on the edge, as described in the FAQ article. But it doesn’t look so good in the 3D view
The basic principle is that when a manufacturer sees copper overlapping the board edge (or hole edge for ordinary through holes) they interpret it as through plating. They know to cut off the extra copper outside the board so it doesn’t matter, but because KiCad doesn’t support showing it that way, pedantic people may prefer customized copper area.
I see, as a new person on the platform, boundary conditions are always ambiguous to me.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.