KiCad Extra Footprint DRC Violation

Diagnostic signature

Extra footprint

The KiCad PCB Editor (pcbnew) DRC engine triggers an "Extra footprint" violation when a footprint exists on the board but lacks a matching symbol in the schematic and is not explicitly marked as a board-only item.

What it means

The KiCad Schematic Parity DRC check compares the internal identifiers (UUIDs) and reference designators of all footprints on the printed circuit board against the symbols defined in the project's schematic. If a footprint exists in the layout editor but no corresponding symbol exists in the schematic, the design rule checker raises this violation to alert the designer of a logical mismatch between the schematic definition and the physical layout.

Why it happens

This warning is emitted when a user manually places a structural or mechanical component—such as a fiducial, mounting hole, test point, or logo—directly onto the PCB canvas without marking its 'Not in schematic' attribute. It also occurs if a symbol is deleted from the schematic editor, but the user does not check the 'Delete footprints with no symbols' option when subsequently running the 'Update PCB from Schematic' action, which leaves an orphaned footprint stranded on the board layout.

Minimal reproduction

(footprint "Fiducial:Fiducial_1mm_Mask2mm" (layer "F.Cu") (attr smd))

How to fix it

Identify if the footprint is an intentional mechanical layout item or a remnant of a deleted schematic symbol, and either mark it as 'Not in schematic' or remove it.

```KiCad S-Expression
(footprint "Fiducial:Fiducial_1mm_Mask2mm" (layer "F.Cu") (attr smd board_only))
```

Step 1

• If the footprint is an intentional mechanical component (such as a mounting hole or fiducial), double-click the footprint on the PCB to open its Properties dialog.

Step 2

• Navigate to the 'Attributes' section and check the 'Not in schematic' box to exempt it from the parity check.

Step 3

• If the footprint is an unintentionally orphaned component from a deleted schematic symbol, select the offending footprint and delete it manually.

Step 4

• Alternatively, run 'Update PCB from Schematic' (F8) and ensure the 'Delete footprints with no symbols' checkbox is checked to automatically clean up orphaned components.

Upstream references

PCB Editor | 8.0 | English | Documentation - KiCad Docs

Pcbnew: DRC issue with Missing and Extra Footprints (#5303) · Issue · kicad/code/kicad