What this error means
Units that share a reference designator are one physical component — U1A
and U1B are two gates inside the same package. One package has one part
number, so KiCad requires every unit of a symbol to carry the same Value
field. The GUI check sorts symbols by reference and compares the Value of
neighboring units; any mismatch reports as:
Different values for U1A (7400) and U1B (74LS00)
Each placed unit is its own symbol instance in the schematic file with its own copy of the Value field, which is what makes drift possible at all.
Common causes
1. Two different parts were merged under one reference
The usual story: a 7400 placed as U1A, and later a 74LS00 placed
and hand-annotated as U1B on the assumption it would "join" the
package. The symbols joined; the values did not. The schematic now
claims one package that is simultaneously two part numbers.
2. One unit's Value was edited and others drifted
Editing the Value on one unit while another unit kept the old text — typically after hand-editing fields, pasting units from another project, or carrying a schematic across KiCad versions. Whatever the route, the file ends up with disagreeing Value strings on one reference.
How to fix it
Set every unit to the same Value
- Click the marker — the report names both units and both values.
- Select each listed unit, press E, and set the Value field to the part you actually intend to fit.
- Re-run ERC (Inspect → Electrical Rules Checker).
Use when: The units really are one package and one of the values is simply stale. This is the usual case.
Split them into separate references
- Select the unit that is actually a different physical part and press E.
- Give it its own unused reference (and unit A), with its own Value.
- Re-annotate if you want the numbering tidied, then re-run ERC.
Use when: The two units were never the same chip — you meant two packages. Two physical parts need two references; the error is pointing at a fiction, not a typo.
When it’s safe to exclude
Never. The schematic is making a physically impossible claim — one package with two part numbers — and the BOM has to pick one. Whichever it picks, half of your intent is silently lost, which is a worse failure mode than the error. Excluding the marker (right-click → Exclude) just locks the ambiguity in.
Gotchas
- The check compares the Value field only. Units can legitimately differ in position, orientation, and per-unit fields like pin assignments; only Value must agree.
- If you actually wanted gates with different values — e.g. treating a resistor-network symbol as four independent resistors — the multi-unit symbol is the wrong modeling tool. Units of one symbol are one component; use separate symbols with separate references instead.
kicad-cli sch ercstays silent about it — see the callout at the top.
Minimal reproduction
GUI (2 minutes): place both units of any multi-unit symbol (a dual op-amp works), press E on unit B, and change its Value to something else. Run Inspect → Electrical Rules Checker:
[unit_value_mismatch]: Different values for U1A (10k) and U1B (22k)
The checked-in file data/erc/samples/unit_value_mismatch.kicad_sch holds
an embedded two-unit symbol placed as U1 unit 1 (Value 10k) and U1 unit
2 (Value 22k). Running it through kicad-cli sch erc --severity-all
under KiCad 9.0.8 and 10.0.8 produces no [unit_value_mismatch]
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 has more units than are defined
- Different footprint assigned in another unit of the symbol
- Different net assigned to a shared pin in another unit of the symbol
- Duplicate reference designators
FAQ
Why do I get 'Different values for U1D (7400) and U1A (74LS00)' when annotating?
The annotation tool runs the same consistency check ERC does, and it found units of U1 disagreeing about what part they are. A 7400 and a 74LS00 are different chips; either set every unit of U1 to the one part you will fit, or give the odd one out its own reference.
Can units of one multi-unit part have dissimilar values on purpose?
Not via the Value field — units share a reference precisely because they are one physical component, and KiCad flags any Value disagreement as an error. Model genuinely different-valued elements as separate symbols with their own references, even when they live in one physical package; that is also the only way the BOM can count them correctly.
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