Missing Hole

Layout Footprints
1

KiCad v7.0.10

M3Bracket.kicad_mod (1.2 KB)

Please can someone tell me why the edge cut hole in this simple footprint doesn’t appear in the 3d viewer?

2

Didn’t looked into your file (I write from Win7 so I have to save it, copy onto another PC where I have KiCad…).
But… place it at PCB and then see 3D view.
It is possible (I’m not sure) that KiCad assumes the edge cut in footprint are (by definition) to be a part of PCB edge cut and not the hole.
Some time ago I bug reported that holes in my footprints are not visible I I think it was fixed, but may be from any reason fix had to be reverted.

3

why the edge cut hole in this simple footprint doesn’t appear in the 3d viewer

Because the simple footprint incorporates a simple mistake.
To find that:

  • open a board with existing valid board outline, run 3D viewer → works
  • place footprint “M3Bracket” in pcb.
  • again run 3D viewer from board → get error message “board outline is malformed” → so there is clearly something wrong with the edge cuts item in your footprint
  • open the footprint in the FP editor
  • doubleclick your edge cuts circle (hole) → circle properties are looking good → must be a different problem
  • activate layer edge.cuts, switch to display mode “dimmed” (normally hotkey “H”, or in the right side appearance panel)
  • CTRL+A to select all items on that layer
  • look at the status bar: it tells you “3 items selected” → so there are not only your circle, but also more (unwanted) items on the edge cuts layer!!
  • search the two unwanted items (hint: look exactly in the middle centre of the big hole)
1 Like
4

Also the DRC check for the board tells what’s wrong: there are several very small circles there. (This is from v8.0.0-RC3.)

image

1 Like
5

Nice addition to the DRC, this error check seems to be new in v8.

But it reports every “unwanted” small circle twice, so there is room for more improvement. (I will make a bugreport, if I get some time).

Also this check could be integrated into the FP editor–>Inspect–>Footprint Checker command, so this mistake can be identified early in the drawing process. (possible feature request).

6

Wow! Thank you mf_ibfeew, as I would never have spotted this on my own.