What this error means
Two different symbols carry the same reference designator — two R5s, two
U1s. The GUI ERC dialog sorts every symbol by reference and compares
neighbors; two entries with the same name, same number, and the same unit
produce Duplicate items U1 (multi-unit symbols legitimately share a
reference across different units — U1A and U1B are one package, not
a duplicate).
There is a second flavor: two symbols share a reference but come from
library symbols with different unit counts — say a one-unit U3 and a
U3B from a four-unit part. That reports as Differing unit counts for item U3 and U3B, under this same violation key.
Duplicates are not cosmetic. The reference is the identity used by the BOM, netlists, and footprint assignment; two parts with one name produce a BOM that undercounts and a netlist in which tools downstream cannot tell the symbols apart.
Common causes
1. A copied block kept its reference designators
Copy-pasting part of a schematic (or importing a design block)
duplicates the symbols with their annotations, so every reference
in the copied block now exists twice. This is by far the usual way
to get dozens of these at once, including on hidden #PWR power
symbols, which are annotated like everything else.
2. A reference was edited by hand into a collision
Renaming a symbol's reference in its properties to a value that is already taken — easy to do when "reorganizing" designators manually instead of using the Annotation tool's numbering options.
3. Two different parts were forced into one multi-unit reference
Giving a symbol the reference U3B by hand when U3 is a different
library part entirely. This is the Differing unit counts variant:
the two symbols cannot be units of one package because their library
definitions disagree about how many units exist.
How to fix it
Re-annotate the duplicated symbols
- Select the block you pasted (or skip selecting to fix the whole schematic).
- Open Tools → Annotate Schematic… and set Scope to Selection only (or Entire schematic).
- Pick the option to reset existing annotations within that scope, then Annotate.
- Re-run ERC (Inspect → Electrical Rules Checker).
Use when: The duplicates came from a pasted block. Resetting only the selection renumbers the copies while leaving the original block's references alone.
Rename one of the two symbols by hand
- Click the violation marker to find both offenders (the report names the reference).
- Select one, press E, and give it an unused reference.
Use when: A single collision, typically after a manual rename. Pick the symbol whose number is wrong rather than renumbering a part that is already placed on the PCB.
When it’s safe to exclude
Never. A duplicate reference is a real identity conflict, and every downstream consumer — BOM, netlist, assembly docs — silently misbehaves while it exists. Excluding the marker (right-click → Exclude) does not make the two parts distinguishable; it only removes the one tool that noticed. The fix is a re-annotate or a one-field rename — cheaper than debugging the undercounted BOM later.
Gotchas
U1Anext toU1Bis not a duplicate — that is one multi-unit package. The check only fires when the same reference and the same unit appear twice, or when the unit counts of the two library symbols disagree.- Pasted
#PWRpower symbols duplicate too. They are invisible in the annotation you see on screen, but the checker walks them like any other symbol; re-annotating clears them along with the visible parts. kicad-cli sch ercstays silent about duplicates — see the callout at the top. Headless CI will pass a schematic with two U1s.
Minimal reproduction
GUI (2 minutes): place a resistor annotated R1, copy it, paste it, and
edit the copy's reference back to R1 (or paste a block with annotations
intact). Run Inspect → Electrical Rules Checker:
[duplicate_reference]: Duplicate items R1
The checked-in file data/erc/samples/duplicate_reference.kicad_sch holds
two embedded symbols that are both U1, unit 1. Running it through
kicad-cli sch erc --severity-all under KiCad 9.0.8 and 10.0.8 produces
no [duplicate_reference] violation — only the two
lib_symbol_issues warnings that are artifacts of the self-contained
sample. That negative result is the point: the CLI never runs this check.
Related errors
- Symbol is not annotated
- Symbol has more units than are defined
- Units of same symbol have different values
- Different net assigned to a shared pin in another unit of the symbol
FAQ
I copied part of my schematic and now annotation reports duplicate items — what happened?
Copy-paste keeps reference designators, so every symbol in the pasted block collides with its original. Select the pasted block, run the Annotation tool with scope set to Selection only and the reset option enabled, and the copies get fresh numbers while the originals keep theirs.
How do I fix duplicate #PWR references without touching my other designators?
Power symbols are annotated like normal symbols, just with hidden
#PWR references, and they duplicate when pasted the same way. The
Annotation tool handles them: annotate with the reset option scoped
to the pasted selection. There is no need to edit #PWR references
by hand, and no benefit to doing so.
Why does my simulation fail with 'multiple symbols have the same reference'?
SPICE netlisting needs unique references to name its elements, so it refuses outright where the schematic merely gets an ERC marker. Fix the duplicate in the schematic (re-annotate or rename) and the simulator error goes away with it.
Sources
- Check implementation — SCH_REFERENCE_LIST::CheckAnnotation, eeschema/sch_reference_list.cpp at KiCad 10.0.3
- GUI ERC dialog annotation pre-pass — eeschema/dialogs/dialog_erc.cpp at KiCad 10.0.3
- CLI ERC job (no annotation check) — eeschema/eeschema_jobs_handler.cpp at KiCad 10.0.3
- KiCad 10 Schematic Editor manual — Reference designators and symbol annotation
- KiCad 9 Schematic Editor manual — Electrical rules checking