Analyze your ERC report

Paste the output of kicad-cli sch erc (plain text or --format json), the report saved from the ERC dialog, or even a single violation line. You get every violation grouped by type, linked to its reference page.

Parsing happens entirely in your browser — nothing you paste leaves this page.

All KiCad ERC errors

48 violation types across KiCad 9 and 10 — 41 written up so far, the rest are in progress. Checks that exist in only one version are marked.

Power

ErrorDefault severitySummary
Ground pin not connected to ground net KiCad 10 only
ground_pin_not_ground
warningKiCad 10 warning: a GND-named power pin sits on a non-ground net while another pin of the same symbol is grounded. Rewire the pin or rename the net.
Input Power pin not driven by any Output Power pins
power_pin_not_driven
errorEvery net with a power input pin must also contain a power output pin to drive it. Power symbols like +5V and GND are inputs, not drivers, so a net fed from a connector or battery trips this error until you add a PWR_FLAG.
Power pins are similar (lower/upper case difference only)
similar_power
warningTwo power symbols name what looks like one rail with different letter case (VCC vs Vcc), so KiCad keeps two separate nets. Rename to one spelling.
Symbol has power input pins that are not placed
missing_power_pin
errorA multi-unit symbol's power unit was never placed, so its supply pins connect to nothing. Place the unit ERC names (LM324: unit E) and wire it.

Connections

ErrorDefault severitySummary
A pin with a "no connection" flag is connected
no_connect_connected
warningThe net under a no-connect flag reaches more than one pin — usually a stale flag on a pin that got wired later. Delete the flag or the wire, not both.
Bus Entry needed (coming soon)
bus_entry_needed
error
Four connection points are joined together
four_way_junction
ignoreFour wire ends or pins meet at one point. Off by default; when enabled, fix by dragging one wire a grid step so the cross becomes two T junctions.
Input pin not driven by any Output pins
pin_not_driven
errorThe net has an Input pin but no driver: no Output, Bidirectional, Tri-state, Power output, or Passive pin. Usually the net isn't reaching its real driver.
Label connects more than one wire
label_multiple_wires
warningThe label anchor sits on a wire crossing, so it attaches to one wire chosen arbitrarily. Move it onto the wire it names, or junction the crossing.
Pin name resembles stacked pin KiCad 10 only
stacked_pin_name
warningA pin number contains brackets but isn't valid stacked-pin notation. Rewrite it as [1-3] or [A1,A2] style, or drop the brackets entirely.
Pin not connected
pin_not_connected
errorEvery pin must join a net or carry a no-connect flag. Press Q to flag intentionally open pins; otherwise the wire is not landing on the pin end.
Symbol pin or wire end off connection grid
endpoint_off_grid
warningA pin or wire end is off the 50 mil connection grid, usually after an import or fine-grid editing. Select all, Align Items to Grid, re-run ERC.
Unconnected "no connection" flag
no_connect_dangling
warningA no-connect flag sits on nothing — no pin, no label. Usually left behind after a symbol was moved or deleted. Delete it, or snap it onto the pin end.
Unconnected wire endpoint
unconnected_wire_endpoint
warningA wire end that connects to nothing, usually a leftover stub. Delete or complete it; a net label clears it only if anchored on the free endpoint.
Wires not connected to anything
wire_dangling
errorA run of wires that touches no pin, label, or sheet pin anywhere. Usually a leftover stub or a wire that stops short of its pin; reconnect or delete it.

Labels

ErrorDefault severitySummary
Global label not connected anywhere else in the schematic KiCad 9 only (removed in 10)
global_label_dangling
warningKiCad 9 warns when a global label's net reaches no other pin. Usually the matching label elsewhere is missing or misspelled; make the names match.
Global label only appears once in the schematic
single_global_label
ignoreERC counts global labels by name; a name that appears once connects nothing. Usually a typo'd or missing counterpart label. Off (Ignore) by default.
Label connected to only one pin KiCad 10 only
isolated_pin_label
warningThis label's net reaches exactly one pin, so it connects nothing. Usually the matching label is missing or misspelled; fix the name or wire the other end.
Label not connected
label_dangling
errorThe label's anchor point is not on a wire or pin, or its net reaches no pins. Move the label so its anchor square sits on the wire, then re-run ERC.
Labels are similar (lower/upper case difference only)
similar_labels
warningNet names are case-sensitive: DATA and Data are two nets that never connect. Retype the odd label to the other's exact spelling to merge them.
Local and global labels have same name
same_local_global_label
warningA local label and a global label share the same name. On one sheet they connect; across sheets they silently don't. Make both global or rename one.
More than one name given to this bus or net
multiple_net_names
warningTwo different names sit on one net — usually a second label or a power symbol — and KiCad keeps only one. Delete the extra name or split the net.
Power pin and label are similar (lower/upper case difference only)
similar_label_and_power
warningA label and a power symbol name one rail with different letter case (Vcc vs VCC), leaving two unconnected nets. Retype the label to match exactly.

Conflicts

ErrorDefault severitySummary
Buses are graphically connected but share no bus members
bus_to_bus_conflict
errorA bus crosses a sheet boundary with a different global bus label on each side and no members in common. Make the names agree or delete the extra label.
Conflict between bus alias definitions across schematic sheets
bus_definition_conflict
errorTwo sheet files define the same bus alias with different members. Delete or align the stale copy in Schematic Setup → Project → Bus Alias Definitions.
Conflict problem between pins
pin_to_pin
error/warning (pin matrix)Two driver pins share one net — often a PWR_FLAG landing on a net a regulator already drives. Remove the extra driver or fix the symbol's pin type.
Duplicate pins with different nets
duplicate_pins
errorOne symbol has two pins with the same number on different nets. Same-numbered pins land on one footprint pad, so wire every drawn copy to the same net.
Duplicate reference designators (coming soon)
duplicate_reference
error
Invalid connection between bus and net items
bus_to_net_conflict
errorA bus and a single net are tied together: usually a sheet pin or label without bus syntax on a bus, or a bus-syntax label on a wire. Rename one side.
Net is graphically connected to a bus but not a bus member
net_not_bus_member
warningThe wire's net name isn't a member of the bus. Rename the label to a real member (D[0..7] expands to D0–D7, no zero padding) or fix the bus label.

Symbol units

ErrorDefault severitySummary
Different footprint assigned in another unit of the symbol
different_unit_footprint
errorUnits of one symbol carry different Footprint fields. Pick the right footprint and assign it once per reference, e.g. in Tools → Assign Footprints.
Different net assigned to a shared pin in another unit of the symbol
different_unit_net
errorOne physical pin drawn in two units of a symbol sits on two different nets. Wire every drawn copy of the shared pin — usually a power pin — to one net.
Symbol has bidirectional pins that are not placed
missing_bidi_pin
warningA unit of this symbol with bidirectional pins was never placed. Place it under the same reference, or repair a reference split by reannotation.
Symbol has input pins that are not placed
missing_input_pin
warningAn unplaced unit of this symbol contains input pins, which float on the real chip. Place the unit and tie its inputs off, or fix a split reference.
Symbol has more units than are defined (coming soon)
extra_units
error
Symbol has units that are not placed
missing_unit
warningA multi-unit symbol has fewer placed units than its library entry defines. Place the missing unit under the same reference, then wire or tie it off.
Units of same symbol have different values (coming soon)
unit_value_mismatch
error

Symbols & libraries

ErrorDefault severitySummary
Assigned footprint doesn't match footprint filters
footprint_filter
ignoreOpt-in check: the Footprint field matches none of the symbol's footprint filter patterns. Usually the filter list is stale — widen it or re-assign.
Footprint link issue
footprint_link_issues
warningThe symbol's Footprint field names a library or footprint your library table can't resolve. Fix the row in Preferences → Manage Footprint Libraries.
Library symbol issue
lib_symbol_issues
warningThe symbol's library nickname isn't in your symbol library tables. Add the library under Preferences → Manage Symbol Libraries and re-run ERC.
SPICE model issue
simulation_model_issue
ignoreFires when a symbol's SPICE model fails to load, usually a stale Sim.Library path. Off by default in KiCad 9/10; fix the path or delete the Sim fields.
Symbol doesn't match copy in library
lib_symbol_mismatch
warningThe cached symbol in your schematic differs from the library version, usually because the library changed. Fix: Tools → Update Symbols from Library.

Hierarchy & sheets

ErrorDefault severitySummary
Duplicate sheet names within a given sheet
duplicate_sheet_names
errorTwo subsheets on the same parent sheet share a name; the comparison ignores case. Rename one in Sheet Properties. Sheet files may repeat, names may not.
Mismatch between hierarchical labels and sheet pins
hier_label_mismatch
errorA sheet pin and the hierarchical label inside the subsheet must have identical names, case included. Rename one side or run Sync Sheet Pins.

Miscellaneous

ErrorDefault severitySummary
Field name has leading or trailing whitespace (coming soon) KiCad 10 only
field_name_whitespace
warning
Symbol is not annotated (coming soon)
unannotated
error
Undefined netclass
undefined_netclass
errorA label or directive names a net class the project doesn't define, so it falls back to Default. Define the class in Schematic Setup or fix the typo.
Unresolved text variable (coming soon)
unresolved_variable
error

How ERC works in KiCad

ERC (Electrical Rules Check) runs after KiCad builds the netlist from your schematic. It walks every net and every symbol and applies two kinds of checks: structural ones (dangling wires, unconnected pins, labels that connect to nothing, annotation problems) and electrical ones driven by the pin conflict matrix, which compares the electrical type of every pin sharing a net — two outputs on one net is an error, an input with nothing driving it is another.

Each violation type has a default severity — error, warning, or ignore — and every one of them is configurable in Schematic Setup → Electrical Rules → Violation Severity. Individual violations can also be excluded from the ERC dialog (right-click → Exclude), which keeps them recorded in the schematic but out of your face. The severity defaults documented on this site are the ones shipped in KiCad 9 and 10, extracted from KiCad’s source code rather than copied from forum posts; where a check exists in only one of the two, or changed between them, the error’s page says so.

You can run ERC without opening the schematic editor: kicad-cli sch erc your-design.kicad_sch writes a plain text report, and --format json emits a machine-readable one — both formats are what the analyzer above understands. For the official documentation, see the Electrical Rules Checking chapter of the KiCad Schematic Editor manual for KiCad 9 or KiCad 10.