kicad/pcbnew/dialogs/panel_setup_rules_help.txt

# ---- Top-level Clauses

(version <number>)
(rule <rule_name> <rule_clause> ...)


# ---- Rule Clauses

(constraint <constraint_type> ...)
(condition "<expression>")
(layer "<layer_name>")


# ---- Constraint Types

clearance    annulus_width   track_width     hole     dissallow


# ---- Item Types

track        via         micro_via       buried_via
pad          hole        graphic         text             zone


# ---- Examples

(rule "copper keepout"
   (constraint disallow track via zone)
   (condition "A.insideArea('zone3')"))

(rule "BGA neckdown"
   (constraint track_width (min 0.2mm) (opt 0.25mm))
   (constraint clearance (min 0.05) (opt 0.08mm))
   (condition "A.insideCourtyard('U3')"))

(rule HV
   (constraint clearance (min 1.5mm))
   (condition "A.netclass == 'HV'"))

(rule HV_HV
   # wider clearance between HV tracks
   (constraint clearance (min "1.5mm + 2.0mm"))
   (condition "A.netclass == 'HV' && B.netclass == 'HV'"))


# ---- Notes
#
# Version clause must be first clause in file.
#
# Use Ctrl+/ to comment or uncomment line(s).
#


# ---- Expression functions
#
# All function parameters support simple wildcards ('*' and '?').
#

# True if any part of A lies within the given footprint's courtyard.

A.insideCourtyard('<footprint_refdes>')


# True if any part of A lies within the given zone's outline.

A.insideArea('<zone_name>')


# True if A has a hole which is plated.

A.isPlated()


# True if A exists on the given layer.  The layer name can be
# either the name assigned in Board Setup > Board Editor Layers or
# the canonical name (ie: F.Cu).

A.onLayer('<layer_name>')