kicad-source/pcbnew/dialogs/panel_setup_rules_help_2constraints.md

Constraints

Constraint type	Argument type	Description
annular_width	min/opt/max	Checks the width of annular rings on vias.
assertion	"<expression>"	Checks the given expression.
clearance	min	Specifies the electrical clearance between copper objects of different nets. (See physical_clearance if you wish to specify clearance between objects regardless of net.) To allow copper objects to overlap (collide), create a clearance constraint with the min value less than zero (for example, -1).
courtyard_clearance	min	Checks the clearance between footprint courtyards and generates an error if any two courtyards are closer than the min distance. If a footprint does not have a courtyard shape, no errors will be generated from this constraint.
creepage	min	Specifies the creepage distance between copper objects of different nets.
diff_pair_gap	min/opt/max	Checks the gap between coupled tracks in a differential pair. Coupled tracks are segments that are parallel to each other. Differential pair gap is not tested on uncoupled portions of a differential pair (for example, the fanout from a component).
diff_pair_uncoupled	max	Checks the distance that a differential pair track is routed uncoupled from the other polarity track in the pair (for example, where the pair fans out from a component, or becomes uncoupled to pass around another object such as a via).
disallow	track via micro_via buried_via pad zone text graphic hole footprint	Specify one or more object types to disallow, separated by spaces. For example, (constraint disallow track) or (constraint disallow track via pad). If an object of this type matches the rule condition, a DRC error will be created. This constraint is essentially the same as a keepout rule area, but can be used to create more specific keepout restrictions.
edge_clearance	min/opt/max	Checks the clearance between objects and the board edge. This can also be thought of as the "milling tolerance" as the board edge will include all graphical items on the Edge.Cuts layer as well as any oval pad holes. (See physical_hole_clearance for the drilling tolerance.)
length	min/max	Checks the total routed length for the nets that match the rule condition and generates an error for each net that is below the min value (if specified) or above the max value (if specified) of the constraint.
hole	min/max	Checks the size (diameter) of a drilled hole in a pad or via. For oval holes, the smaller (minor) diameter will be tested against the min value (if specified) and the larger (major) diameter will be tested against the max value (if specified).
hole_clearance	min	Checks the clearance between a drilled hole in a pad or via and copper objects on a different net. The clearance is measured from the diameter of the hole, not its center.
hole_to_hole	min	Checks the clearance between mechanically-drilled holes in pads and vias. The clearance is measured between the diameters of the holes, not between their centers. This constraint is soley for the protection of drill bits. The clearance between laser-drilled (microvias) and other non-mechanically-drilled holes is not checked, nor is the clearance between milled (oval-shaped) and other non-mechanically-drilled holes.
physical_clearance	min	Checks the clearance between two objects on a given layer (including non-copper layers). While this can perform more general-purpose checks than clearance, it is much slower. Use clearance where possible.
physical_hole_clearance	min	Checks the clearance between a drilled hole in a pad or via and another object, regardless of net. The clearance is measured from the diameter of the hole, not its center. This can also be thought of as the "drilling tolerance" as it only includes round holes (see edge_clearance for the milling tolerance).
silk_clearance	min/opt/max	Checks the clearance between objects on silkscreen layers and other objects.
skew	max	Checks the total skew for the nets that match the rule condition, that is, the difference between the length of each net and the average of all the lengths of each net that is matched by the rule. If the absolute value of the difference between that average and the length of any one net is above the constraint max value, an error will be generated.
solder_mask_expansion	opt	Specifies the solder mask expansion for pads, shapes and tracks.
solder_paste_abs_margin	opt	Specifies the absolute solder paste clearance for pads. Usually negative to inset the paste. The final solder paste clearance will be the absolute clearance plus the relative clearance.
solder_paste_rel_margin	opt	Specifies the relative solder paste clearance for pads. Usually negative to inset the paste. The final solder paste clearance will be the absolute clearance plus the relative clearance.
thermal_relief_gap	min	Specifies the width of the gap between a pad and a zone with a thermal-relief connection.
thermal_spoke_width	opt	Specifies the width of the spokes connecting a pad to a zone with a thermal-relief connection.
track_width	min/opt/max	Checks the width of track and arc segments. An error will be generated for each segment that has a width below the min value (if specified) or above the max value (if specified).
track_angle	min/opt/max	Checks the angle between two connected track segments. An error will be generated for each connected pair with an angle below the min value (if specified) or above the max value (if specified).
track_segment_length	min/max	Checks the length of track and arc segments. An error will be generated for each segment that has a length below the min value (if specified) or above the max value (if specified).
pad_fanout_ratio	max	Checks the width of the fanout for a pad stated as a percentage. An error will be generated for each connected track with a width above the max value (if specified).
via_count	max	Counts the number of vias on every net matched by the rule condition. If that number exceeds the constraint max value on any matched net, an error will be generated for that net.
via_dangling		Checks for vias that are unconnected or connected on only one layer. This constraint does not take a min/opt/max value. In combination with a severity clause, this constraint can be used to allow or disallow dangling vias in various conditions.
zone_connection	solid thermal_reliefs none	Specifies the connection to be made between a zone and a pad.