Duplicate pins with different nets

Diagnostic signature

Duplicate pins with different nets

The KiCad Electrical Rules Checker (ERC) detected multiple pins in a single schematic symbol that share the same pin number but are connected to different nets. All pins sharing an identical number in a symbol instance must be assigned to the same net.

What it means

In KiCad, schematic symbols can contain multiple pins assigned the exact same pin number (for example, to represent multiple physical ground pads on an IC that are internally connected, or a visible pin stacked over hidden power pins). When pins are grouped this way by identical numbering, the schematic editor requires them to be logically and electrically bonded to the same net. When the Electrical Rules Checker (ERC) runs, it verifies that identically numbered pins on the same symbol instance do not diverge to distinct electrical nets. If they are routed to different nets, or if one is left disconnected while the other is actively routed, the parser flags a "Duplicate pins with different nets" violation. This error indicates an unresolvable contradiction in the underlying netlist connectivity, as the tool cannot merge distinct nets onto a single physical pin number.

Why it happens

This diagnostic is emitted if you place a custom or multi-unit symbol with duplicate pin numbers and inadvertently wire those identically numbered pins to electrically distinct nets. It commonly happens when modifying a component library to stack invisible power pins but failing to align their external net assignments in the schematic. It can also occur if a user accidentally drags a wire from a shared pin origin to the wrong power rail. Additionally, the error is triggered if a part's pinout was incorrectly defined in the Symbol Editor by mistakenly assigning the same number to two pins that actually serve separate functions and require distinct connections.

Minimal reproduction

(kicad_sch (version 20211123) (generator eeschema)
  (symbol (lib_id "LocalLib:DUPE_TEST") (at 100 100 0) (unit 1)
    (in_bom yes) (on_board yes)
    (uuid "00000000-0000-0000-0000-000000000000")
    (property "Reference" "U1" (id 0) (at 100 97.46 0))
  )
  (wire (pts (xy 94.92 102.54) (xy 94.92 105)))
  (wire (pts (xy 94.92 97.46) (xy 94.92 95)))
  (label "+5V" (at 94.92 105 0))
  (label "GND" (at 94.92 95 0))
)

How to fix it

Resolve the conflicting net assignments by ensuring all pins with the same number are tied to the exact same net in the schematic, or correct the symbol definition to assign unique pin numbers to electrically distinct pins.

```kicad-sch
(kicad_sch (version 20211123) (generator eeschema)
  (symbol (lib_id "LocalLib:DUPE_TEST") (at 100 100 0) (unit 1)
    (in_bom yes) (on_board yes)
    (uuid "00000000-0000-0000-0000-000000000000")
    (property "Reference" "U1" (id 0) (at 100 97.46 0))
  )
  (wire (pts (xy 94.92 102.54) (xy 94.92 105)))
  (wire (pts (xy 94.92 97.46) (xy 94.92 95)))
  (label "GND" (at 94.92 105 0))
  (label "GND" (at 94.92 95 0))
)
```

Step 1

Run the ERC in the KiCad Schematic Editor and select the "Duplicate pins with different nets" error to locate the offending symbol.

Step 2

Inspect the schematic wires connected to the symbol. If the duplicated pins (e.g., multiple GND pins) are meant to be tied together, re-route the schematic wires so they both connect to the same target net.

Step 3

If the pins serve different electrical purposes and should be on different nets, the error originates in the symbol's library definition. Right-click the symbol and select "Edit with Symbol Editor".

Step 4

Modify the pin properties so that each independent pin has a unique pin number (e.g., change the numbers from "1" and "1" to "1" and "2", or match the manufacturer's physical pinout).

Step 5

Save the symbol, return to the schematic, select "Update Symbol from Library", and re-run the ERC to verify the error is cleared.

Upstream references

Schematic Editor | master | English | Documentation - KiCad Docs

Schematic Editor | 9.0 | English | Documentation - KiCad Docs