Conflict between bus alias definitions across schematic sheets

Bus aliases are saved in the .kicad_sch file that was open when the alias was created, not in the project file. ERC collects the alias definitions from every sheet file and compares any two that share a name. Member lists are sorted before comparison, so order never matters and identical copies on several sheets are fine. Same name with different member sets raises one error naming both files.

The check is severity error because the conflict does not resolve visibly. For connectivity, KiCad 9 keeps a single alias per name in a cache that each sheet file overwrites in load order, so the definition loaded last wins for the whole project. A bus label like {CTRL} can expand to a different set of nets than the sheet that defined CTRL expects, and nothing on the canvas shows which definition won.

Never. The conflict means some sheets were drawn against a member list the netlister may not be using. Excluding the marker (right-click → Exclude) or downgrading the check in Schematic Setup → Electrical Rules → Violation Severity keeps that ambiguity in the design, and the fix is cheaper than the exclusion: delete one row in a dialog. KiCad 10 no longer warns about this at all, so clean a project up while a 9.x ERC still shows the error.

• The violation has no position. The report prints no coordinates and the GUI marker lands at the sheet origin, because the conflict lives in two files' alias tables, not in anything you drew. Look in Schematic Setup, not on the canvas.
• The dialog's duplicate-name guard only watches one sheet file at a time, which is why the second definition is always in a file you weren't looking at when you made it.
• Identical duplicates never warn. Five sheets can each define DATA with the same members, in any order, and ERC stays quiet — until one copy gains a member.