Warnings for mounting holes

Layout Footprints
1

I’m struggling since long time with mounting holes. When I use a standard mounting hole I got a warning “additional footprint” with “REF**”. I also got a warning “doubple footprints” where two times “REF**” is mentioned. In the past I’ve always ignored this. But I would like to have “working mouting holes”.
I tried to modify the mounting holes also in the footprint editor, but no success.

Do the holes have to be in the schematics to get rid of this additional footprint?

I don’t need any ref number for a mounting hole. They don’t have to be numbered. But in the footprint editor I can’t delete this property.

While I tried with modified footprints I also had it that there seems to be two “parts”. When I try to select one I got a question whether I want to select the pad or the footprint. All is very strange.

Any tip to get “good working holes”?

2

You may have 2 overlapping holes, check the layout. (Actually I don’t think so, it’s just that you can select the entire footprint or parts of it. I think it’s the duplicate refdes warning you are getting.)

I usually assign refdes like H1, H2, etc. to avoid the warning about duplicates. You can hide the refdes in the layout display.

You can either put corresponding symbols for the holes in the schematic, or turn on the property Not in Schematic for the footprints.

3

I always include the fixing holes on the schematic and assign the relevant footprint to it. This way it is easy to change if required.
I also put the schematic symbol just outside of the drawing area so it does not show if the schematic is printed.

4

This answer is given for kicad v9. Please add the used kicad version to your next question/thread.

When I use a standard mounting hole I got a warning “additional footprint” with “REF**”

This DRC warning appears for every footprint which has no corresponding symbol on the schematic. possibilities:

  • accept (ignore) this warning
  • disable this DRC-check in Board setup–>design rules->violation severity
  • open footprint properties dialog: set checkbox: “not in schematic”
  • add a hole-symbol in the schematic and assign the wanted hole footprint to that symbol. (this also solves the refdes-issue)

I also got a warning “double footprints” where two times “REF**” is mentioned.
I don’t need any ref number for a mounting hole. They don’t have to be numbered.

But Kicad requests the Reference designator as mandatory.
If you don’t need the RefDes you can set it to “invisible”.
possibilities:

  • set a unique Refdes for each mounting hole
  • accept (ignore) this warning
  • disable this DRC-check in Board setup–>design rules->violation severity

While I tried with modified footprints I also had it that there seems to be two “parts”. When I try to select one I got a question whether I want to select the pad or the footprint.

This happens always if you LMB-click to select something and multiple items are displayed (and selectable) at this screen position. Your mounting hole footprint itself consists of the footprint and of the individual items inside the footprint. The hole itself is normally created with a mechanical THT-pad. If you directly LMB-click (to select) on the hole/pad its ambiguous for the selection algorithm if you want to select the pad only or if you want to select the complete footprint. Hence the display of the “disambiguation menu” - so can choose.
Try to disable “pads” in the selection filter (bottom right screen).

1 Like
5

I inserted the holes now also in my schematic. And the print to disable pad selection was very helpfull.

Thanks

1 Like