What this error means
Every placed symbol records which unit of its library symbol it is (unit 1 for ordinary parts; A/B/C/… for multi-unit parts like quad op-amps). This check compares that number against how many units the library symbol actually defines, and fires when the placed unit number is higher. The GUI report line spells it out:
Error: symbol U1A (unit 2) exceeds units defined (1)
A schematic cannot get into this state through normal placement — the editor only offers units that exist. It happens when the library definition changes after the symbol was placed: the schematic remembers "I am unit 3 of U2", and the symbol it points at no longer has a unit 3.
Common causes
1. The library symbol was edited or replaced with fewer units
The dominant case, and the one the source code itself names: a symbol had units when the schematic was drawn, then the library version was redrawn with fewer (or the symbol was swapped for a single-unit drawing via Change Symbol / a library migration). Every placement of the now-missing units trips this error.
How to fix it
Point the placement at a unit that exists
- Click the marker to find the offending symbol (the report names reference and unit).
- Right-click the symbol → Unit and pick one of the units the library symbol still defines — or delete the placement if the unit genuinely no longer exists.
- Re-run ERC (Inspect → Electrical Rules Checker).
Use when: The library's new, smaller definition is the correct one and the extra placements are leftovers.
Restore the multi-unit library symbol
- Open the symbol in the Symbol Editor (right-click → Edit Symbol) and check how many units the library version defines.
- If the schematic is right and the library regressed, restore the multi-unit drawing in the library (or switch the placement to the correct library symbol via right-click → Change Symbol).
- Update the schematic symbols from the library and re-run ERC.
Use when: The schematic's unit usage was correct and the library is what changed. Only edit symbols in libraries you maintain.
When it’s safe to exclude
Never. The placed symbol references a unit that does not exist, so its pins, body, and connectivity are undefined — there is nothing meaningful on the schematic at that spot. Excluding the marker leaves a phantom placement that the netlist and PCB cannot represent. Resolve the unit mismatch instead; it is usually a few clicks per offending symbol.
Gotchas
- You cannot cause this by misusing the editor today; it is almost always archaeology — a library that changed out from under an older schematic. Check the symbol's library source (right-click → Edit Symbol) before assuming the schematic is at fault.
kicad-cli sch ercstays silent about it — see the callout at the top.
Minimal reproduction
Not reproducible through normal editing — the editor only offers existing units. To see it in the GUI: place a multi-unit symbol's unit B, then edit the library symbol down to one unit (or hand-edit the file), reopen the schematic, and run Inspect → Electrical Rules Checker:
[extra_units]: Error: symbol U1A (unit 2) exceeds units defined (1)
The checked-in file data/erc/samples/extra_units.kicad_sch encodes the
end state directly: one embedded single-unit symbol placed as (unit 2).
Running it through kicad-cli sch erc --severity-all under KiCad 9.0.8
and 10.0.8 produces no [extra_units] violation — only the
lib_symbol_issues warning that is an artifact of the self-contained
sample. That negative result is the point: the CLI never runs this check.
Related errors
- Symbol has units that are not placed
- Units of same symbol have different values
- Symbol doesn't match copy in library
- Duplicate reference designators
FAQ
My symbol's units got letters A, B, C after annotation — is that this error?
No. Trailing unit letters on a multi-unit part (U1A, U1B) are
normal annotation. This error is the reverse situation: the schematic
claims a lettered unit that the library symbol does not define, which
only happens when the library changed after placement.
The symbol in my library only has one unit now — how do I fix the placements that used the old units?
Decide which drawing is right. If the new single-unit symbol is correct, delete the placements of the vanished units and rewire against the surviving one. If the old multi-unit drawing was correct, restore it in the library (or point the schematic at a library that still has it via right-click → Change Symbol), then update symbols from the library.
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
- KiCad 10 Schematic Editor manual — Symbol units and alternate body styles
- KiCad 9 Schematic Editor manual — Electrical rules checking