Classes
struct	UnionFind
struct	Connectivity
struct	ItemGraph
	KiCad 10's item graph (pcbnew/connectivity, CN_VISITOR): items of any nets are linked when their copper touches on a common layer, except two items that cannot change net (pads, zone fills, free vias) on different nets. More...
struct	ZoneFills
	Edge buckets of every zone fill (geom::PolygonIndex), so the zone questions below cost the nearby edges only. More...
struct	CopperItem
struct	Hole
struct	CopperModel
struct	Flashing
	The copper layers of each via (vias) and pad (pads) as KiCad 10.0.6 flashes them (PCB_VIA::FlashLayer, PAD::FlashLayer): a layer keeps its copper unless the padstack removes unconnected copper there and neither a zone connection (zone_layers) nor a track, arc, via or pad of the net (not of the pad's own footprint) touches it. More...
struct	Coupling
struct	ViolationItem
struct	Violation
struct	DrcOptions
struct	DrcReport
struct	ViaHeights
	The length a via adds to its net in KiCad's length calculation (KiCad 10, BOARD_STACKUP::GetLayerDistance): the stackup between the two copper layers the via joins, with the copper of an outer layer in full and of an inner layer by half. More...
struct	LengthItems
	The items of one net that a length or skew rule matched: indices into the board's pads, tracks, arcs and vias. More...
struct	NetLength
	KiCad's LENGTH_DELAY_STATS. Lengths in nm, delays in attoseconds. More...
struct	RefillResult
struct	StarvedThermal
	A thermal relief KiCad's DRC reports as starved_thermal (DRC_TEST_PROVIDER_ZONE_CONNECTIONS::testZoneLayer): fewer spokes reach the zone's fill than the board's minimum (min_resolved_spokes, 2 by default), counting tracks that run from the pad into the fill; spokes into a fill island that touches nothing but this pad do not count unless the pad has no other. More...
struct	DpSuffix
	compiled custom-rule condition More...
class	RuleEngine
struct	CourtyardRegion
struct	CourtyardEntry
struct	CourtyardCache

Enumerations
enum class	ItemKind : std::uint8_t { Pad , Track , Arc , Via , Zone , Graphic }

Functions
Connectivity	compute_connectivity (const model::Board &b, const CopperModel &cm, index::UniformGrid &grid, bool overlap_links=false, const ZoneFills *fills=nullptr)
bool	in_item_graph (const CopperItem &it)
bool	can_change_net (const CopperItem &it)
ItemGraph	item_graph (const model::Board &b, const CopperModel &cm, index::UniformGrid &grid)
std::vector< int >	zones_touching (const CopperModel &cm, const ZoneFills &zf, index::UniformGrid &grid, const geom::Shape &s, model::LayerMask layers, Coord clearance=0)
	Zone-fill items on layers whose copper is closer than clearance to s (0, the default: overlap only, as KiCad's SHAPE::Collide; 1: touching counts), ascending item indices.
std::vector< model::NetId >	propagate_nets (const CopperModel &cm, const ItemGraph &g, const ZoneFills &zf, index::UniformGrid &grid)
	The nets KiCad's DRC sees after loading a board (CN_CONNECTIVITY_ALGO::PropagateNets, run by every connectivity build): a via touching only zone fills takes a zone's net (its own if one of the zones has it, else the lowest); then in every cluster of the graph without zones whose pads carry one net only, tracks, arcs, vias and board graphics take that net (a stray via on a track joins the track's net; a track bridging two nets keeps its own).
const char *	kind_name (ItemKind k)
	KiCad expression type names: Pad, Track, Arc, Via, Zone, Graphic.
std::vector< geom::Shape >	pad_shapes (const model::Pad &pad)
	Pad copper shape in absolute coordinates.
CopperModel	build_copper (const model::Board &b)
model::LayerMask	conditional_layers (const model::Via &v)
	KiCad's ConditionallyFlashed: the layers of a via, or of a plated through-hole pad on a board of copper_count layers, whose copper depends on what connects there.
model::LayerMask	conditional_layers (const model::Pad &p, int copper_count)
Flashing	flash_layers (const model::Board &b)
std::vector< std::vector< model::Point > >	edge_loops (const std::vector< geom::Shape > &edges, Coord tol=2 '000, bool *all_closed=nullptr)
	Closed loops chained from Edge.Cuts pieces whose ends meet within tol; pieces that close no loop are dropped (all_closed, if given, tells whether any was).
std::optional< Coupling >	couple (model::Point p0, model::Point p1, Coord wp, model::Point n0, model::Point n1, Coord wn)
	The two centrelines (a P track from p0 to p1 of width wp, an N track likewise) coupled as KiCad couples them, or nothing: both longer than about 1 nm, exactly parallel (a zero cross product) and not collinear, with overlapping projections.
DrcReport	run_drc (const model::Board &b, const model::DesignRules &r, const DrcOptions &opt={})
void	write_drc_json (const DrcReport &rep, const std::string &path)
	Writes the report in kicad-cli's JSON layout (violations, unconnected_items; positions in mm).
ViaHeights	via_heights (const model::Board &b, const model::DesignRules &rules)
NetLength	net_length (const model::Board &b, const model::DesignRules &rules, const ViaHeights &vh, const LengthItems &items, const model::TuningProfile *profile)
	Length and delay of items, all of one net.
RefillResult	refill_zones (const model::Board &b, const model::DesignRules &r)
	Follows ZONE_FILLER::fillCopperZone: outline within the board, thermal gaps around same-net pads, every other item knocked out at its clearance, spokes that reach the fill, minimum-width pruning, then islands without a pad removed by each zone's island_removal_mode.
std::vector< StarvedThermal >	starved_thermals (const model::Board &filled, const model::DesignRules &r)
	On a board whose fills are current (refill_zones' board): every pad KiCad would report, in pad then zone order.
std::vector< geom::Ring >	thermal_spokes (const model::Pad &pad, const model::Zone &zone)
	The four spoke polygons of a pad's thermal relief to a zone, as the zone filler draws them (buildThermalSpokes).
DpSuffix	match_dp_suffix (std::string_view name)
bool	area_matches (const CopperItem &item, const model::Zone &area, bool enclosed)
	Requires a common copper layer.
CourtyardCache	build_courtyards (const model::Board &board)
	Build once per board; invalid/unclosed contours leave the corresponding side empty and marked unreadable.
bool	footprint_selected (const std::string &selector, const std::string &reference, const std::string &lib_id)
	KiCad's footprint selector (testFootprintSelector): a reference wildcard, or, when the selector contains ':', a library-id wildcard.
bool	courtyard_matches (const CopperItem &item, const CourtyardCache &courtyards, const std::string &selector, const std::string &function)
	Function is intersectsCourtyard/intersectsFrontCourtyard/intersectsBackCourtyard.
std::vector< int >	courtyard_entries (const CourtyardCache &courtyards, const std::string &selector)
	The entries a footprint selector picks, in entry order, and the same test against them.
bool	courtyard_matches (const CopperItem &item, const CourtyardCache &courtyards, const std::vector< int > &entries, const std::string &function)

Enumeration Type Documentation

◆ ItemKind

enum class tmk::drc::ItemKind : std::uint8_t

strong

Enumerator
Pad
Track
Arc
Via
Zone
Graphic

Definition at line 11 of file copper.hpp.

Function Documentation

◆ area_matches()

bool tmk::drc::area_matches	(	const CopperItem &	item,
		const model::Zone &	area,
		bool	enclosed )

Requires a common copper layer.

Outline rings use even/odd filling (holes and disjoint contours); enclosed requires every copper shape to be wholly inside. The caller selects/caches zones; insideArea and intersectsArea both pass false.

◆ build_copper()

CopperModel tmk::drc::build_copper ( const model::Board & b )

◆ build_courtyards()

CourtyardCache tmk::drc::build_courtyards ( const model::Board & board )

Build once per board; invalid/unclosed contours leave the corresponding side empty and marked unreadable.

◆ can_change_net()

bool tmk::drc::can_change_net ( const CopperItem & it )

◆ compute_connectivity()

Connectivity tmk::drc::compute_connectivity	(	const model::Board &	b,
		const CopperModel &	cm,
		index::UniformGrid &	grid,
		bool	overlap_links = false,
		const ZoneFills *	fills = nullptr )

◆ conditional_layers() [1/2]

model::LayerMask tmk::drc::conditional_layers	(	const model::Pad &	p,
		int	copper_count )

◆ conditional_layers() [2/2]

model::LayerMask tmk::drc::conditional_layers ( const model::Via & v )

KiCad's ConditionallyFlashed: the layers of a via, or of a plated through-hole pad on a board of copper_count layers, whose copper depends on what connects there.

◆ couple()

std::optional< Coupling > tmk::drc::couple	(	model::Point	p0,
		model::Point	p1,
		Coord	wp,
		model::Point	n0,
		model::Point	n1,
		Coord	wn )

The two centrelines (a P track from p0 to p1 of width wp, an N track likewise) coupled as KiCad couples them, or nothing: both longer than about 1 nm, exactly parallel (a zero cross product) and not collinear, with overlapping projections.

◆ courtyard_entries()

std::vector< int > tmk::drc::courtyard_entries	(	const CourtyardCache &	courtyards,
		const std::string &	selector )

The entries a footprint selector picks, in entry order, and the same test against them.

The rule engine resolves each selector once when the rules are compiled (Condition::bind): a rule is evaluated for every pair of items the DRC compares and for every lattice point the router visits, and matching the selector against every footprint each time made a courtyard clearance rule dominate the DRC of a large board.

◆ courtyard_matches() [1/2]

bool tmk::drc::courtyard_matches	(	const CopperItem &	item,
		const CourtyardCache &	courtyards,
		const std::string &	selector,
		const std::string &	function )

Function is intersectsCourtyard/intersectsFrontCourtyard/intersectsBackCourtyard.

Front and back are the footprint's own sides (KiCad: GetCourtyard(fp->IsFlipped() ? B_Cu : F_Cu)): the front courtyard of a flipped footprint is its B.CrtYd outline. The item's copper side does not matter. This overload matches the selector against every footprint for each query: the reference path.

◆ courtyard_matches() [2/2]

bool tmk::drc::courtyard_matches	(	const CopperItem &	item,
		const CourtyardCache &	courtyards,
		const std::vector< int > &	entries,
		const std::string &	function )

◆ edge_loops()

std::vector< std::vector< model::Point > > tmk::drc::edge_loops	(	const std::vector< geom::Shape > &	edges,
		Coord	tol = 2 '000,
		bool *	all_closed = nullptr )

Closed loops chained from Edge.Cuts pieces whose ends meet within tol; pieces that close no loop are dropped (all_closed, if given, tells whether any was).

◆ flash_layers()

Flashing tmk::drc::flash_layers ( const model::Board & b )

◆ footprint_selected()

bool tmk::drc::footprint_selected	(	const std::string &	selector,
		const std::string &	reference,
		const std::string &	lib_id )

KiCad's footprint selector (testFootprintSelector): a reference wildcard, or, when the selector contains ':', a library-id wildcard.

Case-sensitive, like wxString::Matches.

◆ in_item_graph()

bool tmk::drc::in_item_graph ( const CopperItem & it )

◆ item_graph()

ItemGraph tmk::drc::item_graph	(	const model::Board &	b,
		const CopperModel &	cm,
		index::UniformGrid &	grid )

◆ kind_name()

const char * tmk::drc::kind_name ( ItemKind k )

KiCad expression type names: Pad, Track, Arc, Via, Zone, Graphic.

◆ match_dp_suffix()

DpSuffix tmk::drc::match_dp_suffix ( std::string_view name )

◆ net_length()

NetLength tmk::drc::net_length	(	const model::Board &	b,
		const model::DesignRules &	rules,
		const ViaHeights &	vh,
		const LengthItems &	items,
		const model::TuningProfile *	profile )

Length and delay of items, all of one net.

profile is the tuning profile of the net's class (null: every delay is 0, as in KiCad).

◆ pad_shapes()

std::vector< geom::Shape > tmk::drc::pad_shapes ( const model::Pad & pad )

Pad copper shape in absolute coordinates.

◆ propagate_nets()

std::vector< model::NetId > tmk::drc::propagate_nets	(	const CopperModel &	cm,
		const ItemGraph &	g,
		const ZoneFills &	zf,
		index::UniformGrid &	grid )

The nets KiCad's DRC sees after loading a board (CN_CONNECTIVITY_ALGO::PropagateNets, run by every connectivity build): a via touching only zone fills takes a zone's net (its own if one of the zones has it, else the lowest); then in every cluster of the graph without zones whose pads carry one net only, tracks, arcs, vias and board graphics take that net (a stray via on a track joins the track's net; a track bridging two nets keeps its own).

Clusters without pads take the net of their first item with a net. Returns one net per copper item.

◆ refill_zones()

RefillResult tmk::drc::refill_zones	(	const model::Board &	b,
		const model::DesignRules &	r )

Follows ZONE_FILLER::fillCopperZone: outline within the board, thermal gaps around same-net pads, every other item knocked out at its clearance, spokes that reach the fill, minimum-width pruning, then islands without a pad removed by each zone's island_removal_mode.

Teardrop zones lose their fill: kicad-cli's refill first rebuilds teardrops (TEARDROP_MANAGER::UpdateTeardrops), and a rebuilt teardrop joins a pad to a track that already touches it. Hatched zones are not redrawn: their stored fill is kept where the new solid fill still is (warning).

◆ run_drc()

DrcReport tmk::drc::run_drc	(	const model::Board &	b,
		const model::DesignRules &	r,
		const DrcOptions &	opt = {} )

◆ starved_thermals()

std::vector< StarvedThermal > tmk::drc::starved_thermals	(	const model::Board &	filled,
		const model::DesignRules &	r )

On a board whose fills are current (refill_zones' board): every pad KiCad would report, in pad then zone order.

Not covered: custom-pad spoke primitives and min_resolved_spokes constraints in custom rules (the board setup's applies).

◆ thermal_spokes()

std::vector< geom::Ring > tmk::drc::thermal_spokes	(	const model::Pad &	pad,
		const model::Zone &	zone )

The four spoke polygons of a pad's thermal relief to a zone, as the zone filler draws them (buildThermalSpokes).

◆ via_heights()

ViaHeights tmk::drc::via_heights	(	const model::Board &	b,
		const model::DesignRules &	rules )

◆ write_drc_json()

void tmk::drc::write_drc_json	(	const DrcReport &	rep,
		const std::string &	path )

Writes the report in kicad-cli's JSON layout (violations, unconnected_items; positions in mm).

◆ zones_touching()

std::vector< int > tmk::drc::zones_touching	(	const CopperModel &	cm,
		const ZoneFills &	zf,
		index::UniformGrid &	grid,
		const geom::Shape &	s,
		model::LayerMask	layers,
		Coord	clearance = 0 )

Zone-fill items on layers whose copper is closer than clearance to s (0, the default: overlap only, as KiCad's SHAPE::Collide; 1: touching counts), ascending item indices.

Classes

Enumerations

Functions