Duplicate footprints

Diagnostic signature

Duplicate footprints

The KiCad Design Rule Checker detected multiple footprints on the PCB sharing the exact same reference designator, causing ambiguity in schematic parity.

What it means

The KiCad Design Rule Checker (DRC) issues this warning when it detects that two or more footprints placed on the circuit board share identical reference designators (for example, multiple footprints labeled 'R1'). The DRC engine groups this violation under 'Schematic parity DRC checks', which are strict validations designed to ensure that the physical layout accurately reflects the original logical schematic. Because reference designators must uniquely identify each component in a given design, having duplicates creates an ambiguous state where the toolchain cannot reliably determine which physical footprint corresponds to the logical symbol in the schematic layout.

Why it happens

This condition is typically triggered by user error or script bugs during layout drafting. A hardware designer might manually copy and paste an existing footprint on the PCB canvas (or use the duplicate tool) without immediately updating its reference designator. Similarly, a custom scripted placement operation might inadvertently stamp multiple identical instances of the same component. The KiCad engine evaluates the board state against the schematic logic; if multiple footprints claim the exact same reference designator and at least one maps back to a valid schematic symbol via its internal identifier path, the rules checker raises the violation. According to upstream KiCad documentation, this specific error is intentionally suppressed if the duplicated footprints do not correspond to any schematic symbols whatsoever, meaning they exist purely as unlinked board-level elements.

Minimal reproduction

(kicad_pcb (version 20240108) (generator pcbnew)
  (paper "A4")
  (footprint "Resistor_SMD:R_0805_2012Metric" (layer "F.Cu")
    (at 100 100)
    (path "/00000000-0000-0000-0000-000000000001")
    (attr smd)
    (fp_text reference "R1" (at 0 0) (layer "F.SilkS")
      (effects (font (size 1 1) (thickness 0.15)))
    )
  )
  (footprint "Resistor_SMD:R_0805_2012Metric" (layer "F.Cu")
    (at 110 100)
    (path "/00000000-0000-0000-0000-000000000001")
    (attr smd)
    (fp_text reference "R1" (at 0 0) (layer "F.SilkS")
      (effects (font (size 1 1) (thickness 0.15)))
    )
  )
)

How to fix it

Resolve the duplication by deleting the extraneous footprint from the PCB or by assigning it a unique reference designator that correctly maps to a new schematic symbol.

```KiCad PCB
(kicad_pcb (version 20240108) (generator pcbnew)
  (paper "A4")
  (footprint "Resistor_SMD:R_0805_2012Metric" (layer "F.Cu")
    (at 100 100)
    (path "/00000000-0000-0000-0000-000000000001")
    (attr smd)
    (fp_text reference "R1" (at 0 0) (layer "F.SilkS")
      (effects (font (size 1 1) (thickness 0.15)))
    )
  )
)
```

Step 1

• Open the DRC control window in the KiCad PCB Editor and locate the 'Duplicate footprints' violation to identify the coordinates of the conflicting components.

Step 2

• If the footprint was placed accidentally and is truly redundant, select the extraneous footprint on the canvas and delete it.

Step 3

• If the footprint is intended to be a distinct active component, switch to the Schematic Editor, place the corresponding new symbol, and annotate it with a unique reference designator.

Step 4

• Re-synchronize the layout by running 'Update PCB from Schematic' (F8). Ensure the newly annotated symbol links correctly to the footprint.

Step 5

• If persistent unlinked duplicates remain, you can enable the 'Delete extra footprints' option within the schematic update dialog to automatically clean up any footprints lacking a matching schematic counterpart.

Upstream references

PCB Editor | master | English | Documentation - KiCad Docs

pcbnew/drc/drc_item.cpp - KiCad Source Code - GitLab

DRC violation Severity need cleanup in presentation. (#6616) · Issues - GitLab