Symbol pin or wire end off connection grid

Diagnostic signature

Symbol pin or wire end off connection grid

An ERC violation indicating that a symbol pin or wire endpoint does not align with the standard 50-mil schematic connection grid, which can prevent correct electrical connectivity.

What it means

In KiCad's Schematic Editor (Eeschema), this diagnostic indicates that one or more endpoints of a wire, or pins of a schematic symbol, do not align exactly with the schematic's electrical connection grid. By default, KiCad expects all electrical connections to occur on a 50-mil (1.27 mm) grid to ensure standard component interchangeability. If a component's pin or a wire segment ends off of this specified grid size, the Electrical Rules Check (ERC) flags it as an `endpoint_off_grid` violation. This is a critical check because off-grid pins and wires might appear visually connected on the schematic canvas but remain logically unattached in the generated netlist, leading to missing connections on the printed circuit board.

Why it happens

This ERC violation typically occurs when the schematic grid is manually changed to a finer resolution (such as 25 mils, 10 mils, or metric sizes like 1 mm) during the placement of symbols or drawing of wires. When moving elements on a smaller grid, their connection points snap to the sub-grid and miss the standard 50-mil intersection nodes. It can also happen when utilizing poorly designed third-party symbol libraries where the pins were not originally placed on a 50-mil grid. Although KiCad's schematic setup allows the ERC "connection width" parameter to be modified from 50 mils, changing this value is highly discouraged as most standard libraries strictly rely on the default 50-mil alignment.

Minimal reproduction

(kicad_sch (version 20231120) (generator eeschema)
  (wire (pts (xy 10.16 20.32) (xy 10.414 20.32)) (stroke (width 0) (type default)))
)

How to fix it

Align the disconnected or off-grid items back to the standard 50-mil (1.27 mm) schematic grid.

```KiCad Schematic
(kicad_sch (version 20231120) (generator eeschema)
  (wire (pts (xy 10.16 20.32) (xy 12.7 20.32)) (stroke (width 0) (type default)))
)
```

Step 1

Ensure the schematic grid is set to 50 mils (1.27 mm) using the grid dropdown or right-click menu.

Step 2

Select the offending symbol(s) or wire(s) that the ERC has flagged.

Step 3

Right-click the selection and choose 'Align Elements to Grid' to automatically snap their coordinates to the standard 50-mil boundaries.

Step 4

Delete and manually re-draw any wires that did not perfectly reconnect to the symbol pins.

Step 5

Re-run the Electrical Rules Check (ERC) to verify the violations are resolved.

Upstream references

Schematic Editor | Documentation - KiCad Docs

eeschema/erc/erc_settings.h - KiCad Source Code