Kicad 7 - DRC error , footprint type

[Nick_W]

I’m getting a DRC error “footprint type doesn’t match footprint pads (expected through hole, actual SMD)”

Cause was that when the footprint was created, it was erroneously set as an ‘SMD’ type.

OK, been back in the footprint editor and corrected that, then in artwork editor, ‘Update footprints from Library’ but the error persists, cannot get rid of it. Also tried ‘Update PCB from schematic’, but that didn’t help either.

How do I get rid of this error?

[paulvdh]

The Update Footprints from Library should have gotten rid of that DRC violation. It’s probably a silly little thing. Theck this:

• The updated footprint is actually saved in the library.
• The footprint on the schematic & PCB are linked to the same footprint and in that same library.
• The footprint is actually being updated (there are a bunch of settings in the PCB Editor / Tools / Update Footprints from Library
• Or did you use the Update Footprint from Library from the properties dialog of one of the footprint? (Goes to the same dialog, but with different default settings).

An easy check is to open the properties window of such a footprint and see if the Fabrication Attributes / Footprint type: has been updated.

[Nick_W]

• The updated footprint is actually saved in the library.
  Yes it is.
• The footprint on the schematic & PCB are linked to the same footprint and in that same library.
  Appears so.
• The footprint is actually being updated (there are a bunch of settings in the PCB Editor / Tools / Update Footprints from Library
  It should have been.
• Or did you use the Update Footprint from Library from the properties dialog of one of the footprint? (Goes to the same dialog, but with different default settings).
  No.

An easy check is to open the properties window of such a footprint and see if the Fabrication Attributes / Footprint type: has been updated.
It hadn’t been, but once I manually changed it to Through hole, the error went away

Looks like there might possibly be a small bug there.

[paulvdh]

I’ve been clicking around for some 10 minutes but could not reproduce it. For me it works as it should, but there are many small details that form a line of domino’s. In addition to the list I already mentioned, during the PCB Editor / Tools / Update Footprints from Library you have to turn on the Update / Reset fabrication attributes checkbox. This checkbox is off by default.

[Nick_W]

Ah, don’t recall it so might have missed that. I’ll try it later, thanks.

[Nick_W]

Update:

Yes, you were quite right. I went back to the footprint, changed it to SMD and saved it. Ran the DRC in the artwork editor, and got a warning that the library version didn’t match the artwork. Updated from library with that option ticked, the warning was replaced by the error that the type didn’t match. Went back to the footprint editor and changed it back to through hole and saved it, back in the artwork editor updated without the option. Got the warning and the error. Updated with the option and both went away.

Thanks for your help.