What this error means

For every schematic file in the design, ERC compares the Sheet name of each pair of hierarchical sheets placed on it. The comparison is case-insensitive (Power and power collide) and runs on the displayed text, after text variables are expanded. A match between two sheets on the same parent is an error, with the marker placed on the first of the pair.

Only siblings conflict. The same name on two different parent sheets is fine, and the sheet file is never part of the comparison: any number of sheets may reference one file. The name is what has to be unique, because KiCad uses it to build the full net name of every net in the subsheet (a local label net1 inside sheet power becomes /power/net1) and to label the sheet in the hierarchy navigator and title block.

Common causes

1. A sheet was renamed by hand to a name its sibling already uses

The Sheet Properties dialog does not check for collisions, so typing a name already used on that parent (or a case variant of it) goes through silently and only surfaces at ERC time. Multi-instance hierarchies are where this happens: several sheets share one file, only the name tells them apart, and one rename too few leaves two of them matching.

2. The schematic was assembled outside the schematic editor

Sheet blocks merged in from another project at file level, schematics generated by a script, or a design carried over from an old KiCad version. Pasting inside KiCad 9 and 10 is not a cause: paste renames incoming sheets automatically (power, power1, power2, ...) precisely to avoid this error.

How to fix it

Rename one of the two sheets

  1. Select the flagged sheet outline and press E (or right-click → Properties) to open Sheet Properties.
  2. Change **Sheet name** to something unique among that parent's sheets. Leave **Sheet file** alone: a shared file is fine and is how multi-instance hierarchies work.
  3. Re-run ERC (Inspect → Electrical Rules Checker).

Use when: This is the fix; the only decision is which of the two sheets gets the new name. Renaming either one clears the violation.

Rename from the hierarchy navigator when several collide

  1. Open the hierarchy navigator with its button in the left toolbar; it docks as a tree of every sheet.
  2. Right-click a sheet name in the tree and choose **Rename**.
  3. Work down the tree, then re-run ERC.

Use when: Generated or merged designs with more than one collision. The tree shows all names side by side, which makes case variants easy to spot. Same path in KiCad 9 and 10.

When it’s safe to exclude

Never, realistically. The sheet name is the namespace for every net in the subsheet, and the conflict leaks out of ERC: in an exported netlist the two sheets of the repro are both listed as /power/, distinguishable only by their UUID paths, and kicad-cli prints Warning: duplicate sheet names. on every netlist export. Net highlighting refuses to run at all, with "Error: duplicate sub-sheet names found in current sheet."

KiCad tracks sheet instances by UUID internally, so the design is not corrupted — which is exactly why excluding the marker (right-click → Exclude) or downgrading the severity (Schematic Setup → Electrical Rules → Violation Severity) is tempting and still wrong: everything human-facing stays ambiguous to save a ten-second rename.

Gotchas

  • The match ignores case. Power and power are duplicates, which also disposes of renaming-by-capitalization as a fix.
  • Names are compared after text-variable expansion, so two sheet names that resolve to the same string collide even when the raw fields differ.
  • The error is not about the sheet file. Four sheets pointing at one channel.kicad_sch is the supported multi-channel pattern, provided the four names differ.
  • The marker lands on the first sheet of the pair; the report lists both positions, so read it to find the partner.
Minimal reproduction

In the schematic editor: add two hierarchical sheets to one page (Place → Add Sheet), point both at the same file, and give both the name power — the second one has to be renamed by hand in Sheet Properties, because paste would auto-rename it. Run ERC:

[duplicate_sheet_names]: Duplicate sheet names within a given sheet
    ; error
    @(38.10 mm, 38.10 mm): Hierarchical Sheet 'power'
    @(78.74 mm, 38.10 mm): Hierarchical Sheet 'power'

The checked-in sample data/erc/samples/duplicate_sheet_names/ is a two-file hierarchy (a root plus one shared sub.kicad_sch) containing no symbols at all, so the target error is the only violation in the report. Renaming either sheet to anything else drops the count to zero.

FAQ

Can two hierarchical sheets use the same schematic file?

Yes. Any number of sheets may reference one file; that is how multi-channel designs reuse a circuit. Each instance needs its own sheet name, and the symbol references are the only other thing that differs between instances.

Does the sheet name actually matter, or is it just a label?

It matters. KiCad builds the full net name of every net in the subsheet from it (/power/net1) and uses it in the hierarchy navigator and title block. The file name is just storage; the sheet name is the identity the check cares about.

I used a text variable in the sheet name and now ERC reports duplicates.

The check compares resolved text. If the variable expands to the same string for both sheets, they are duplicates no matter how the raw fields are written. Give each instance a distinct literal name or a variable that resolves uniquely per sheet.

Sources