What this error means
ERC tests three kinds of item against the schematic's connection grid: both endpoints of every wire and bus segment, the connection points of bus entries, and the position of every symbol pin. A point passes only if its X and Y coordinates are exact multiples of the grid. The grid defaults to 50 mils (1.27 mm) and is set per schematic in Schematic Setup → General → Formatting → Connection grid (minimum 25 mils).
The check is pure arithmetic on coordinates; it does not test whether anything is disconnected. It exists because off-grid geometry is how disconnections happen: a wire end 0.01 mm from a pin never joins its net, and no zoom level you would actually work at will show you the gap.
Common causes
1. The schematic was imported, or predates KiCad 8
The Altium importer is known to leave rounded coordinates like 24.9999 mm where 25 mm was meant, and imports from other tools land off-grid the same way. Older KiCad projects trip it too: KiCad 7 tested endpoints against your editing grid with a 25 mil floor, KiCad 8 and later test the fixed connection grid — so a file that was clean in 7 can open with hundreds of these warnings.
2. It was drawn on a fine or metric grid
With the grid overrides turned off, everything snaps to whatever grid is active — 0.25 mm, 10 mils — and lands between the 1.27 mm connection-grid lines. The schematic is internally consistent, but not on the grid the check demands.
3. A library symbol has off-grid pins
Converter-generated vendor symbols sometimes place pins at metric or otherwise odd offsets from the symbol origin. Then every placement of that symbol flags, no matter how carefully you wire it. The symbol needs fixing, not the schematic.
How to fix it
Select everything and run Align Items to Grid
- Press Ctrl+A to select the sheet (or drag-select the flagged region).
- Right-click → Align Items to Grid. Repeat on each sheet with markers.
- Re-run ERC (Inspect → Electrical Rules Checker). Aligning moves things: any new pin-not-connected errors mean an endpoint landed apart from its pin and needs rewiring.
Use when: The bulk cases — imported schematics and pre-8 projects with warnings in the dozens or hundreds. Same menu path in KiCad 9 and 10.
Drag the flagged endpoint back onto the grid
- Click the violation in the ERC dialog to jump to the marker.
- Drag the wire end or symbol; with the default Grid Overrides (Preferences → Preferences… → Schematic Editor → Grids), connected items snap to a 50 mil grid, so the drop lands on grid.
- Re-run ERC.
Use when: A handful of markers on an otherwise clean schematic. More surgical than a whole-sheet align.
Fix the pins in the symbol itself
- Right-click a flagged symbol → Edit Symbol.
- Move each pin onto a 50 mil multiple; KiCad's own libraries place pins on a 100 mil grid, which satisfies any connection grid.
- Save, then run Tools → Update Symbols from Library… and re-run ERC.
Use when: Every placement of one symbol flags — the signature of a converter-generated vendor symbol with off-grid pins.
When it’s safe to exclude
For a hand-drawn schematic, don't. Each marker is a two-minute fix, and the bug this warning predicts — a wire that looks attached but isn't — surfaces later as a missing connection on the board.
The defensible case is a large imported schematic you trust and do not plan to rework. Run Align Items to Grid first anyway; it clears most markers in one pass. To silence the rest, exclude individual markers (right-click the marker → Exclude) or downgrade the check in Schematic Setup → Electrical Rules → Violation Severity — accepting that every future off-grid edit now goes unreported. A design deliberately drawn on a 25 mil pitch is the one case for lowering the Connection grid setting instead.
Gotchas
- The count understates the work: a wire reports at most one endpoint (the end is only checked when the start passes) and a symbol at most one pin per run, so fixing a marker can surface a new one on the same item at the next run.
- In the
kicad-clitext report, the@(x, y)coordinate identifies the item — for a wire, its start — not necessarily the off-grid end. The GUI marker sits on the actual bad point. - KiCad 10 skips pins whose electrical type is Unconnected; KiCad 9 flags them like any other pin. A schematic can gain or lose a warning moving between the two.
- Current defaults snap connected items to a 50 mil grid while you draw (Grid Overrides, on by default), so fresh violations in new work usually mean the overrides were switched off.
Version notes
- KiCad 8.0: UI title changed from "Symbol pin or wire end off grid".
Minimal reproduction
In the schematic editor: place two resistors and wire them together. In Preferences → Preferences… → Schematic Editor → Grids, untick the Connected items grid override, pick a 0.1 mm grid, and nudge one resistor one step sideways. ERC reports the moved pin and the wire end:
[endpoint_off_grid]: Symbol pin or wire end off connection grid
; warning
The checked-in file data/erc/samples/endpoint_off_grid.kicad_sch is
the same situation in miniature: U1's pin and the wire start sit on the
default 1.27 mm connection grid; the far wire end and U2's pin sit at
x = 121.93 mm — 0.01 mm off. Two embedded warnings about the missing
repro library are artifacts of the self-contained sample. Editing
121.93 back to 121.92 (and 127.01 to 127) clears both violations —
Align Items to Grid in file form.
Related errors
- Pin not connected
- Wires not connected to anything
- Unconnected wire endpoint (reference page coming soon)
FAQ
I opened a KiCad 7 project in a newer version and ERC now shows hundreds of these warnings. Was my schematic broken all along?
Probably not. KiCad 7 checked endpoints against the editing grid with a 25 mil floor, so a schematic drawn on 25 mils passed. KiCad 8 and later check a fixed connection grid defaulting to 50 mils, and every point between those grid lines now gets flagged. Connections that worked in 7 still work; select all, run Align Items to Grid, and re-check.
ERC flags a pin that looks exactly on the grid. Why?
Coordinates a fraction of a mil off render identically at any usable zoom, and imported schematics often carry values like 24.9999 mm where 25 mm was meant. Select the item and run Align Items to Grid rather than trusting your eyes.
Can I change the connection grid size so these warnings go away?
The setting is in Schematic Setup → General → Formatting, and lowering it to its 25 mil minimum is legitimate when the whole schematic is deliberately drawn on that pitch. As a silencer it is the wrong tool: nothing moves, so a wire end that misses its pin by a hair keeps missing it — the report goes quiet, the risk stays.
These are only warnings — do I actually have to fix them?
The failure they predict is quiet: an off-grid wire end that misses its pin produces a netlist without that connection. This warning flags the geometry before it becomes an unconnected-pin error — or a dead net on an assembled board. Fixing is one command.