pns_kicad_iface.cpp

Go to the documentation of this file.

/*
 * KiRouter - a push-and-(sometimes-)shove PCB router
 *
 * Copyright (C) 2013-2016 CERN
 * Copyright (C) 2016-2024 KiCad Developers, see AUTHORS.txt for contributors.
 * Author: Tomasz Wlostowski <[email protected]>
 *
 * This program is free software: you can redistribute it and/or modify it
 * under the terms of the GNU General Public License as published by the
 * Free Software Foundation, either version 3 of the License, or (at your
 * option) any later version.
 *
 * This program is distributed in the hope that it will be useful, but
 * WITHOUT ANY WARRANTY; without even the implied warranty of
 * MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE. See the GNU
 * General Public License for more details.
 *
 * You should have received a copy of the GNU General Public License along
 * with this program. If not, see <http://www.gnu.org/licenses/>.
 */
 
#include <board.h>
#include <board_connected_item.h>
#include <board_design_settings.h>
#include <netinfo.h>
#include <footprint.h>
#include <layer_range.h>
#include <pad.h>
#include <pcb_track.h>
#include <zone.h>
#include <pcb_shape.h>
#include <pcb_generator.h>
#include <pcb_text.h>
#include <board_commit.h>
#include <layer_ids.h>
#include <kidialog.h>
#include <tools/pcb_tool_base.h>
#include <tool/tool_manager.h>
#include <settings/app_settings.h>
 
#include <gal/graphics_abstraction_layer.h>
#include <pcb_painter.h>
 
#include <geometry/shape.h>
#include <geometry/shape_line_chain.h>
#include <geometry/shape_arc.h>
#include <geometry/shape_simple.h>
 
#include <drc/drc_rule.h>
#include <drc/drc_engine.h>
 
#include <connectivity/connectivity_data.h>
 
#include <wx/log.h>
 
#include <memory>
 
#include <advanced_config.h>
#include <pcbnew_settings.h>
#include <macros.h>
 
#include "pns_kicad_iface.h"
#include "pns_arc.h"
#include "pns_sizes_settings.h"
#include "pns_item.h"
#include "pns_layerset.h"
#include "pns_line.h"
#include "pns_solid.h"
#include "pns_segment.h"
#include "pns_node.h"
#include "pns_router.h"
#include "pns_debug_decorator.h"
#include "router_preview_item.h"
 
typedef VECTOR2I::extended_type ecoord;
 
 
struct CLEARANCE_CACHE_KEY
{
 const PNS::ITEM* A;
 const PNS::ITEM* B;
 bool Flag;
 
 bool operator==(const CLEARANCE_CACHE_KEY& other) const
 {
 return A == other.A && B == other.B && Flag == other.Flag;
 }
};
 
namespace std
{
 template <>
 struct hash<CLEARANCE_CACHE_KEY>
 {
 std::size_t operator()( const CLEARANCE_CACHE_KEY& k ) const
 {
 size_t retval = 0xBADC0FFEE0DDF00D;
 hash_combine( retval, hash<const void*>()( k.A ), hash<const void*>()( k.B ), hash<int>()( k.Flag ) );
 return retval;
 }
 };
}
 
 
class PNS_PCBNEW_RULE_RESOLVER : public PNS::RULE_RESOLVER
{
public:
 PNS_PCBNEW_RULE_RESOLVER( BOARD* aBoard, PNS::ROUTER_IFACE* aRouterIface );
 virtual ~PNS_PCBNEW_RULE_RESOLVER();
 
 int Clearance( const PNS::ITEM* aA, const PNS::ITEM* aB,
 bool aUseClearanceEpsilon = true ) override;
 
 PNS::NET_HANDLE DpCoupledNet( PNS::NET_HANDLE aNet ) override;
 int DpNetPolarity( PNS::NET_HANDLE aNet ) override;
 bool DpNetPair( const PNS::ITEM* aItem, PNS::NET_HANDLE& aNetP,
 PNS::NET_HANDLE& aNetN ) override;
 
 int NetCode( PNS::NET_HANDLE aNet ) override;
 wxString NetName( PNS::NET_HANDLE aNet ) override;
 
 bool IsInNetTie( const PNS::ITEM* aA ) override;
 bool IsNetTieExclusion( const PNS::ITEM* aItem, const VECTOR2I& aCollisionPos,
 const PNS::ITEM* aCollidingItem ) override;
 
 bool IsDrilledHole( const PNS::ITEM* aItem ) override;
 bool IsNonPlatedSlot( const PNS::ITEM* aItem ) override;
 
 bool IsKeepout( const PNS::ITEM* aObstacle, const PNS::ITEM* aItem, bool* aEnforce ) override;
 
 bool QueryConstraint( PNS::CONSTRAINT_TYPE aType, const PNS::ITEM* aItemA,
 const PNS::ITEM* aItemB, int aLayer,
 PNS::CONSTRAINT* aConstraint ) override;
 
 int ClearanceEpsilon() const override { return m_clearanceEpsilon; }
 
 void ClearCacheForItems( std::vector<const PNS::ITEM*>& aItems ) override;
 void ClearCaches() override;
 void ClearTemporaryCaches() override;
 
private:
 BOARD_ITEM* getBoardItem( const PNS::ITEM* aItem, PCB_LAYER_ID aBoardLayer, int aIdx = 0 );
 
private:
 PNS::ROUTER_IFACE* m_routerIface;
 BOARD* m_board;
 PCB_TRACK m_dummyTracks[2];
 PCB_ARC m_dummyArcs[2];
 PCB_VIA m_dummyVias[2];
 int m_clearanceEpsilon;
 
 std::unordered_map<CLEARANCE_CACHE_KEY, int> m_clearanceCache;
 std::unordered_map<CLEARANCE_CACHE_KEY, int> m_tempClearanceCache;
};
 
 
PNS_PCBNEW_RULE_RESOLVER::PNS_PCBNEW_RULE_RESOLVER( BOARD* aBoard,
 PNS::ROUTER_IFACE* aRouterIface ) :
 m_routerIface( aRouterIface ),
 m_board( aBoard ),
 m_dummyTracks{ { aBoard }, { aBoard } },
 m_dummyArcs{ { aBoard }, { aBoard } },
 m_dummyVias{ { aBoard }, { aBoard } }
{
 for( PCB_TRACK& track : m_dummyTracks )
 track.SetFlags( ROUTER_TRANSIENT );
 
 for( PCB_ARC& arc : m_dummyArcs )
 arc.SetFlags( ROUTER_TRANSIENT );
 
 for ( PCB_VIA& via : m_dummyVias )
 via.SetFlags( ROUTER_TRANSIENT );
 
 if( aBoard )
 m_clearanceEpsilon = aBoard->GetDesignSettings().GetDRCEpsilon();
 else
 m_clearanceEpsilon = 0;
}
 
 
PNS_PCBNEW_RULE_RESOLVER::~PNS_PCBNEW_RULE_RESOLVER()
{
}
 
 
bool PNS_PCBNEW_RULE_RESOLVER::IsInNetTie( const PNS::ITEM* aA )
{
 BOARD_ITEM* item = aA->BoardItem();
 
 return item && item->GetParentFootprint() && item->GetParentFootprint()->IsNetTie();
}
 
 
bool PNS_PCBNEW_RULE_RESOLVER::IsNetTieExclusion( const PNS::ITEM* aItem,
 const VECTOR2I& aCollisionPos,
 const PNS::ITEM* aCollidingItem )
{
 if( !aItem || !aCollidingItem )
 return false;
 
 std::shared_ptr<DRC_ENGINE> drcEngine = m_board->GetDesignSettings().m_DRCEngine;
 BOARD_ITEM* item = aItem->BoardItem();
 BOARD_ITEM* collidingItem = aCollidingItem->BoardItem();
 
 FOOTPRINT* collidingFp = collidingItem->GetParentFootprint();
 FOOTPRINT* itemFp = item ? item->GetParentFootprint() : nullptr;
 
 if( collidingFp && itemFp && ( collidingFp == itemFp ) && itemFp->IsNetTie() )
 {
 // Two items colliding from the same net tie footprint are not checked
 return true;
 }
 
 if( drcEngine )
 {
 return drcEngine->IsNetTieExclusion( NetCode( aItem->Net() ),
 m_routerIface->GetBoardLayerFromPNSLayer( aItem->Layer() ),
 aCollisionPos, collidingItem );
 }
 
 return false;
}
 
 
bool PNS_PCBNEW_RULE_RESOLVER::IsKeepout( const PNS::ITEM* aObstacle, const PNS::ITEM* aItem,
 bool* aEnforce )
{
 auto checkKeepout =
 []( const ZONE* aKeepout, const BOARD_ITEM* aOther )
 {
 if( !aOther )
 return false;
 
 if( aKeepout->GetDoNotAllowTracks() && aOther->IsType( { PCB_ARC_T, PCB_TRACE_T } ) )
 return true;
 
 if( aKeepout->GetDoNotAllowVias() && aOther->Type() == PCB_VIA_T )
 return true;
 
 if( aKeepout->GetDoNotAllowPads() && aOther->Type() == PCB_PAD_T )
 return true;
 
 // Incomplete test, but better than nothing:
 if( aKeepout->GetDoNotAllowFootprints() && aOther->Type() == PCB_PAD_T )
 {
 return !aKeepout->GetParentFootprint()
 || aKeepout->GetParentFootprint() != aOther->GetParentFootprint();
 }
 
 return false;
 };
 
 if( aObstacle->Parent() && aObstacle->Parent()->Type() == PCB_ZONE_T )
 {
 const ZONE* zone = static_cast<ZONE*>( aObstacle->Parent() );
 
 if( zone->GetIsRuleArea() && zone->HasKeepoutParametersSet() )
 {
 *aEnforce = checkKeepout( zone,
 getBoardItem( aItem, m_routerIface->GetBoardLayerFromPNSLayer(
 aObstacle->Layer() ) ) );
 return true;
 }
 }
 
 return false;
}
 
 
static bool isCopper( const PNS::ITEM* aItem )
{
 if ( !aItem )
 return false;
 
 const BOARD_ITEM *parent = aItem->Parent();
 
 return !parent || parent->IsOnCopperLayer();
}
 
 
static bool isHole( const PNS::ITEM* aItem )
{
 if ( !aItem )
 return false;
 
 return aItem->OfKind( PNS::ITEM::HOLE_T );
}
 
 
static bool isEdge( const PNS::ITEM* aItem )
{
 if ( !aItem )
 return false;
 
 const PCB_SHAPE *parent = dynamic_cast<PCB_SHAPE*>( aItem->BoardItem() );
 
 return parent && ( parent->IsOnLayer( Edge_Cuts ) || parent->IsOnLayer( Margin ) );
}
 
 
bool PNS_PCBNEW_RULE_RESOLVER::IsDrilledHole( const PNS::ITEM* aItem )
{
 if( isHole( aItem ) && aItem->Parent() )
 return aItem->Parent()->HasDrilledHole();
 
 return false;
}
 
 
bool PNS_PCBNEW_RULE_RESOLVER::IsNonPlatedSlot( const PNS::ITEM* aItem )
{
 if( !isHole( aItem ) )
 return false;
 
 BOARD_ITEM* parent = aItem->Parent();
 
 if( !parent && aItem->ParentPadVia() )
 parent = aItem->ParentPadVia()->Parent();
 
 if( parent )
 {
 if( parent->Type() == PCB_PAD_T )
 {
 PAD* pad = static_cast<PAD*>( parent );
 
 return pad->GetAttribute() == PAD_ATTRIB::NPTH
 && pad->GetDrillSizeX() != pad->GetDrillSizeY();
 }
 
 // Via holes are (currently) always round, and always plated
 }
 
 return false;
}
 
 
BOARD_ITEM* PNS_PCBNEW_RULE_RESOLVER::getBoardItem( const PNS::ITEM* aItem, PCB_LAYER_ID aBoardLayer, int aIdx )
{
 switch( aItem->Kind() )
 {
 case PNS::ITEM::ARC_T:
 m_dummyArcs[aIdx].SetLayer( aBoardLayer );
 m_dummyArcs[aIdx].SetNet( static_cast<NETINFO_ITEM*>( aItem->Net() ) );
 m_dummyArcs[aIdx].SetStart( aItem->Anchor( 0 ) );
 m_dummyArcs[aIdx].SetEnd( aItem->Anchor( 1 ) );
 return &m_dummyArcs[aIdx];
 
 case PNS::ITEM::VIA_T:
 case PNS::ITEM::HOLE_T:
 m_dummyVias[aIdx].SetLayer( aBoardLayer );
 m_dummyVias[aIdx].SetNet( static_cast<NETINFO_ITEM*>( aItem->Net() ) );
 m_dummyVias[aIdx].SetStart( aItem->Anchor( 0 ) );
 return &m_dummyVias[aIdx];
 
 case PNS::ITEM::SEGMENT_T:
 case PNS::ITEM::LINE_T:
 m_dummyTracks[aIdx].SetLayer( aBoardLayer );
 m_dummyTracks[aIdx].SetNet( static_cast<NETINFO_ITEM*>( aItem->Net() ) );
 m_dummyTracks[aIdx].SetStart( aItem->Anchor( 0 ) );
 m_dummyTracks[aIdx].SetEnd( aItem->Anchor( 1 ) );
 return &m_dummyTracks[aIdx];
 
 default:
 return nullptr;
 }
}
 
 
bool PNS_PCBNEW_RULE_RESOLVER::QueryConstraint( PNS::CONSTRAINT_TYPE aType,
 const PNS::ITEM* aItemA, const PNS::ITEM* aItemB,
 int aPNSLayer, PNS::CONSTRAINT* aConstraint )
{
 std::shared_ptr<DRC_ENGINE> drcEngine = m_board->GetDesignSettings().m_DRCEngine;
 
 if( !drcEngine )
 return false;
 
 DRC_CONSTRAINT_T hostType;
 
 switch ( aType )
 {
 case PNS::CONSTRAINT_TYPE::CT_CLEARANCE: hostType = CLEARANCE_CONSTRAINT; break;
 case PNS::CONSTRAINT_TYPE::CT_WIDTH: hostType = TRACK_WIDTH_CONSTRAINT; break;
 case PNS::CONSTRAINT_TYPE::CT_DIFF_PAIR_GAP: hostType = DIFF_PAIR_GAP_CONSTRAINT; break;
 case PNS::CONSTRAINT_TYPE::CT_LENGTH: hostType = LENGTH_CONSTRAINT; break;
 case PNS::CONSTRAINT_TYPE::CT_DIFF_PAIR_SKEW: hostType = SKEW_CONSTRAINT; break;
 case PNS::CONSTRAINT_TYPE::CT_MAX_UNCOUPLED: hostType = MAX_UNCOUPLED_CONSTRAINT; break;
 case PNS::CONSTRAINT_TYPE::CT_VIA_DIAMETER: hostType = VIA_DIAMETER_CONSTRAINT; break;
 case PNS::CONSTRAINT_TYPE::CT_VIA_HOLE: hostType = HOLE_SIZE_CONSTRAINT; break;
 case PNS::CONSTRAINT_TYPE::CT_HOLE_CLEARANCE: hostType = HOLE_CLEARANCE_CONSTRAINT; break;
 case PNS::CONSTRAINT_TYPE::CT_EDGE_CLEARANCE: hostType = EDGE_CLEARANCE_CONSTRAINT; break;
 case PNS::CONSTRAINT_TYPE::CT_HOLE_TO_HOLE: hostType = HOLE_TO_HOLE_CONSTRAINT; break;
 case PNS::CONSTRAINT_TYPE::CT_PHYSICAL_CLEARANCE: hostType = PHYSICAL_CLEARANCE_CONSTRAINT; break;
 default: return false; // should not happen
 }
 
 BOARD_ITEM* parentA = aItemA ? aItemA->BoardItem() : nullptr;
 BOARD_ITEM* parentB = aItemB ? aItemB->BoardItem() : nullptr;
 PCB_LAYER_ID board_layer = m_routerIface->GetBoardLayerFromPNSLayer( aPNSLayer );
 DRC_CONSTRAINT hostConstraint;
 
 // A track being routed may not have a BOARD_ITEM associated yet.
 if( aItemA && !parentA )
 parentA = getBoardItem( aItemA, board_layer, 0 );
 
 if( aItemB && !parentB )
 parentB = getBoardItem( aItemB, board_layer, 1 );
 
 if( parentA )
 hostConstraint = drcEngine->EvalRules( hostType, parentA, parentB, board_layer );
 
 if( hostConstraint.IsNull() )
 return false;
 
 if( hostConstraint.GetSeverity() == RPT_SEVERITY_IGNORE )
 {
 aConstraint->m_Value.SetMin( -1 );
 aConstraint->m_RuleName = hostConstraint.GetName();
 aConstraint->m_Type = aType;
 return true;
 }
 
 switch ( aType )
 {
 case PNS::CONSTRAINT_TYPE::CT_CLEARANCE:
 case PNS::CONSTRAINT_TYPE::CT_WIDTH:
 case PNS::CONSTRAINT_TYPE::CT_DIFF_PAIR_GAP:
 case PNS::CONSTRAINT_TYPE::CT_VIA_DIAMETER:
 case PNS::CONSTRAINT_TYPE::CT_VIA_HOLE:
 case PNS::CONSTRAINT_TYPE::CT_HOLE_CLEARANCE:
 case PNS::CONSTRAINT_TYPE::CT_EDGE_CLEARANCE:
 case PNS::CONSTRAINT_TYPE::CT_HOLE_TO_HOLE:
 case PNS::CONSTRAINT_TYPE::CT_LENGTH:
 case PNS::CONSTRAINT_TYPE::CT_DIFF_PAIR_SKEW:
 case PNS::CONSTRAINT_TYPE::CT_MAX_UNCOUPLED:
 case PNS::CONSTRAINT_TYPE::CT_PHYSICAL_CLEARANCE:
 aConstraint->m_Value = hostConstraint.GetValue();
 aConstraint->m_RuleName = hostConstraint.GetName();
 aConstraint->m_Type = aType;
 return true;
 
 default:
 return false;
 }
}
 
 
void PNS_PCBNEW_RULE_RESOLVER::ClearCacheForItems( std::vector<const PNS::ITEM*>& aItems )
{
 int n_pruned = 0;
 std::set<const PNS::ITEM*> remainingItems( aItems.begin(), aItems.end() );
 
/* We need to carefully check both A and B item pointers in the cache against dirty/invalidated
 items in the set, as the clearance relation is commutative ( CL[a,b] == CL[b,a] ). The code
 below is a bit ugly, but works in O(n*log(m)) and is run once or twice during ROUTER::Move() call
 - so I hope it still gets better performance than no cache at all */
 for( auto it = m_clearanceCache.begin(); it != m_clearanceCache.end(); )
 {
 bool dirty = remainingItems.find( it->first.A ) != remainingItems.end();
 dirty |= remainingItems.find( it->first.B) != remainingItems.end();
 
 if( dirty )
 {
 it = m_clearanceCache.erase( it );
 n_pruned++;
 } else
 it++;
 }
#if 0
 printf("ClearCache : n_pruned %d\n", n_pruned );
#endif
}
 
 
void PNS_PCBNEW_RULE_RESOLVER::ClearCaches()
{
 m_clearanceCache.clear();
 m_tempClearanceCache.clear();
}
 
 
void PNS_PCBNEW_RULE_RESOLVER::ClearTemporaryCaches()
{
 m_tempClearanceCache.clear();
}
 
 
int PNS_PCBNEW_RULE_RESOLVER::Clearance( const PNS::ITEM* aA, const PNS::ITEM* aB,
 bool aUseClearanceEpsilon )
{
 CLEARANCE_CACHE_KEY key = { aA, aB, aUseClearanceEpsilon };
 
 // Search cache (used for actual board items)
 auto it = m_clearanceCache.find( key );
 
 if( it != m_clearanceCache.end() )
 return it->second;
 
 // Search cache (used for temporary items within an algorithm)
 it = m_tempClearanceCache.find( key );
 
 if( it != m_tempClearanceCache.end() )
 return it->second;
 
 PNS::CONSTRAINT constraint;
 int rv = 0;
 PNS_LAYER_RANGE layers;
 
 if( !aB )
 layers = aA->Layers();
 else if( isEdge( aA ) )
 layers = aB->Layers();
 else if( isEdge( aB ) )
 layers = aA->Layers();
 else
 layers = aA->Layers().Intersection( aB->Layers() );
 
 // Normalize layer range (no -1 magic numbers)
 layers = layers.Intersection( PNS_LAYER_RANGE( PCBNEW_LAYER_ID_START, PCB_LAYER_ID_COUNT - 1 ) );
 
 for( int layer = layers.Start(); layer <= layers.End(); ++layer )
 {
 if( IsDrilledHole( aA ) && IsDrilledHole( aB ) )
 {
 if( QueryConstraint( PNS::CONSTRAINT_TYPE::CT_HOLE_TO_HOLE, aA, aB, layer, &constraint ) )
 {
 if( constraint.m_Value.Min() > rv )
 rv = constraint.m_Value.Min();
 }
 }
 else if( isHole( aA ) || isHole( aB ) )
 {
 if( QueryConstraint( PNS::CONSTRAINT_TYPE::CT_HOLE_CLEARANCE, aA, aB, layer, &constraint ) )
 {
 if( constraint.m_Value.Min() > rv )
 rv = constraint.m_Value.Min();
 }
 }
 
 // No 'else'; plated holes get both HOLE_CLEARANCE and CLEARANCE
 if( isCopper( aA ) && ( !aB || isCopper( aB ) ) )
 {
 if( QueryConstraint( PNS::CONSTRAINT_TYPE::CT_CLEARANCE, aA, aB, layer, &constraint ) )
 {
 if( constraint.m_Value.Min() > rv )
 rv = constraint.m_Value.Min();
 }
 }
 
 // No 'else'; non-plated milled holes get both HOLE_CLEARANCE and EDGE_CLEARANCE
 if( isEdge( aA ) || IsNonPlatedSlot( aA ) || isEdge( aB ) || IsNonPlatedSlot( aB ) )
 {
 if( QueryConstraint( PNS::CONSTRAINT_TYPE::CT_EDGE_CLEARANCE, aA, aB, layer, &constraint ) )
 {
 if( constraint.m_Value.Min() > rv )
 rv = constraint.m_Value.Min();
 }
 }
 
 if( QueryConstraint( PNS::CONSTRAINT_TYPE::CT_PHYSICAL_CLEARANCE, aA, aB, layer, &constraint ) )
 {
 if( constraint.m_Value.Min() > rv )
 rv = constraint.m_Value.Min();
 }
 }
 
 if( aUseClearanceEpsilon && rv > 0 )
 rv = std::max( 0, rv - m_clearanceEpsilon );
 
 /*
 * It makes no sense to put items that have no owning NODE in the cache - they can be
 * allocated on stack and we can't really invalidate them in the cache when they are
 * destroyed. Probably a better idea would be to use a static unique counter in PNS::ITEM
 * constructor to generate the cache keys.
 *
 * However, algorithms DO greatly benefit from using the cache, so ownerless items need to be
 * cached. In order to easily clear those only, a temporary cache is created. If this doesn't
 * seem nice, an alternative is clearing the full cache once it reaches a certain size. Also
 * not pretty, but VERY effective to keep things interactive.
 */
 if( aA && aB )
 {
 if ( aA->Owner() && aB->Owner() )
 m_clearanceCache[ key ] = rv;
 else
 m_tempClearanceCache[ key ] = rv;
 }
 
 return rv;
}
 
 
bool PNS_KICAD_IFACE_BASE::inheritTrackWidth( PNS::ITEM* aItem, int* aInheritedWidth )
{
 VECTOR2I p;
 
 assert( aItem->Owner() != nullptr );
 
 auto tryGetTrackWidth =
 []( PNS::ITEM* aPnsItem ) -> int
 {
 switch( aPnsItem->Kind() )
 {
 case PNS::ITEM::SEGMENT_T: return static_cast<PNS::SEGMENT*>( aPnsItem )->Width();
 case PNS::ITEM::ARC_T: return static_cast<PNS::ARC*>( aPnsItem )->Width();
 default: return -1;
 }
 };
 
 int itemTrackWidth = tryGetTrackWidth( aItem );
 
 if( itemTrackWidth > 0 )
 {
 *aInheritedWidth = itemTrackWidth;
 return true;
 }
 
 switch( aItem->Kind() )
 {
 case PNS::ITEM::VIA_T: p = static_cast<PNS::VIA*>( aItem )->Pos(); break;
 case PNS::ITEM::SOLID_T: p = static_cast<PNS::SOLID*>( aItem )->Pos(); break;
 default: return false;
 }
 
 const PNS::JOINT* jt = static_cast<const PNS::NODE*>( aItem->Owner() )->FindJoint( p, aItem );
 
 assert( jt != nullptr );
 
 int mval = INT_MAX;
 
 PNS::ITEM_SET linkedSegs( jt->CLinks() );
 linkedSegs.ExcludeItem( aItem ).FilterKinds( PNS::ITEM::SEGMENT_T | PNS::ITEM::ARC_T );
 
 for( PNS::ITEM* item : linkedSegs.Items() )
 {
 int w = tryGetTrackWidth( item );
 
 if( w > 0 )
 mval = std::min( w, mval );
 }
 
 if( mval == INT_MAX )
 return false;
 
 *aInheritedWidth = mval;
 return true;
}
 
 
bool PNS_KICAD_IFACE_BASE::ImportSizes( PNS::SIZES_SETTINGS& aSizes, PNS::ITEM* aStartItem,
 PNS::NET_HANDLE aNet, VECTOR2D aStartPosition )
{
 BOARD_DESIGN_SETTINGS& bds = m_board->GetDesignSettings();
 PNS::CONSTRAINT constraint;
 
 if( aStartItem && m_startLayer < 0 )
 m_startLayer = aStartItem->Layer();
 
 aSizes.SetClearance( bds.m_MinClearance );
 aSizes.SetMinClearance( bds.m_MinClearance );
 aSizes.SetClearanceSource( _( "board minimum clearance" ) );
 
 int startAnchor = 0;
 VECTOR2I startPosInt( aStartPosition.x, aStartPosition.y );
 
 if( aStartItem && aStartItem->Kind() == PNS::ITEM::SEGMENT_T )
 {
 // Find the start anchor which is closest to the start mouse location
 double anchor0Distance = startPosInt.Distance( aStartItem->Anchor( 0 ) );
 double anchor1Distance = startPosInt.Distance( aStartItem->Anchor( 1 ) );
 
 if( anchor1Distance < anchor0Distance )
 startAnchor = 1;
 }
 
 if( aStartItem )
 {
 PNS::SEGMENT dummyTrack;
 dummyTrack.SetEnds( aStartItem->Anchor( startAnchor ), aStartItem->Anchor( startAnchor ) );
 dummyTrack.SetLayer( m_startLayer );
 dummyTrack.SetNet( static_cast<NETINFO_ITEM*>( aStartItem->Net() ) );
 
 if( m_ruleResolver->QueryConstraint( PNS::CONSTRAINT_TYPE::CT_CLEARANCE, &dummyTrack,
 nullptr, m_startLayer, &constraint ) )
 {
 if( constraint.m_Value.Min() >= bds.m_MinClearance )
 {
 aSizes.SetClearance( constraint.m_Value.Min() );
 aSizes.SetClearanceSource( constraint.m_RuleName );
 }
 }
 }
 
 int trackWidth = bds.m_TrackMinWidth;
 bool found = false;
 aSizes.SetWidthSource( _( "board minimum track width" ) );
 
 if( bds.m_UseConnectedTrackWidth && !bds.m_TempOverrideTrackWidth && aStartItem != nullptr )
 {
 found = inheritTrackWidth( aStartItem, &trackWidth );
 
 if( found )
 aSizes.SetWidthSource( _( "existing track" ) );
 }
 
 if( !found && bds.UseNetClassTrack() && aStartItem )
 {
 PNS::SEGMENT dummyTrack;
 dummyTrack.SetEnds( aStartItem->Anchor( startAnchor ), aStartItem->Anchor( startAnchor ) );
 dummyTrack.SetLayer( m_startLayer );
 dummyTrack.SetNet( static_cast<NETINFO_ITEM*>( aStartItem->Net() ) );
 
 if( m_ruleResolver->QueryConstraint( PNS::CONSTRAINT_TYPE::CT_WIDTH, &dummyTrack, nullptr,
 m_startLayer, &constraint ) )
 {
 trackWidth = std::max( trackWidth, constraint.m_Value.Opt() );
 found = true;
 
 if( trackWidth == constraint.m_Value.Opt() )
 aSizes.SetWidthSource( constraint.m_RuleName );
 }
 }
 
 if( !found )
 {
 trackWidth = std::max( trackWidth, bds.GetCurrentTrackWidth() );
 
 if( bds.UseNetClassTrack() )
 aSizes.SetWidthSource( _( "netclass 'Default'" ) );
 else if( trackWidth == bds.GetCurrentTrackWidth() )
 aSizes.SetWidthSource( _( "user choice" ) );
 }
 
 aSizes.SetTrackWidth( trackWidth );
 aSizes.SetBoardMinTrackWidth( bds.m_TrackMinWidth );
 aSizes.SetTrackWidthIsExplicit( !bds.m_UseConnectedTrackWidth || bds.m_TempOverrideTrackWidth );
 
 int viaDiameter = bds.m_ViasMinSize;
 int viaDrill = bds.m_MinThroughDrill;
 
 PNS::VIA dummyVia, coupledVia;
 
 if( aStartItem )
 {
 dummyVia.SetNet( aStartItem->Net() );
 coupledVia.SetNet( m_ruleResolver->DpCoupledNet( aStartItem->Net() ) );
 }
 
 if( bds.UseNetClassVia() && aStartItem ) // netclass value
 {
 if( m_ruleResolver->QueryConstraint( PNS::CONSTRAINT_TYPE::CT_VIA_DIAMETER, &dummyVia,
 nullptr, m_startLayer, &constraint ) )
 {
 viaDiameter = std::max( viaDiameter, constraint.m_Value.Opt() );
 }
 
 if( m_ruleResolver->QueryConstraint( PNS::CONSTRAINT_TYPE::CT_VIA_HOLE, &dummyVia,
 nullptr, m_startLayer, &constraint ) )
 {
 viaDrill = std::max( viaDrill, constraint.m_Value.Opt() );
 }
 }
 else
 {
 viaDiameter = bds.GetCurrentViaSize();
 viaDrill = bds.GetCurrentViaDrill();
 }
 
 aSizes.SetViaDiameter( viaDiameter );
 aSizes.SetViaDrill( viaDrill );
 
 int diffPairWidth = bds.m_TrackMinWidth;
 int diffPairGap = bds.m_MinClearance;
 int diffPairViaGap = bds.m_MinClearance;
 
 aSizes.SetDiffPairWidthSource( _( "board minimum track width" ) );
 aSizes.SetDiffPairGapSource( _( "board minimum clearance" ) );
 
 found = false;
 
 // First try to pick up diff pair width from starting track, if enabled
 if( bds.m_UseConnectedTrackWidth && aStartItem )
 found = inheritTrackWidth( aStartItem, &diffPairWidth );
 
 // Next, pick up gap from netclass, and width also if we didn't get a starting width above
 if( bds.UseNetClassDiffPair() && aStartItem )
 {
 PNS::NET_HANDLE coupledNet = m_ruleResolver->DpCoupledNet( aStartItem->Net() );
 
 PNS::SEGMENT dummyTrack;
 dummyTrack.SetEnds( aStartItem->Anchor( 0 ), aStartItem->Anchor( 0 ) );
 dummyTrack.SetLayer( m_startLayer );
 dummyTrack.SetNet( static_cast<NETINFO_ITEM*>( aStartItem->Net() ) );
 
 PNS::SEGMENT coupledTrack;
 dummyTrack.SetEnds( aStartItem->Anchor( 0 ), aStartItem->Anchor( 0 ) );
 dummyTrack.SetLayer( m_startLayer );
 dummyTrack.SetNet( static_cast<NETINFO_ITEM*>( coupledNet ) );
 
 if( !found
 && m_ruleResolver->QueryConstraint( PNS::CONSTRAINT_TYPE::CT_WIDTH, &dummyTrack,
 &coupledTrack, m_startLayer, &constraint ) )
 {
 diffPairWidth = std::max( diffPairWidth, constraint.m_Value.Opt() );
 
 if( diffPairWidth == constraint.m_Value.Opt() )
 aSizes.SetDiffPairWidthSource( constraint.m_RuleName );
 }
 
 if( m_ruleResolver->QueryConstraint( PNS::CONSTRAINT_TYPE::CT_DIFF_PAIR_GAP, &dummyTrack,
 &coupledTrack, m_startLayer, &constraint ) )
 {
 diffPairGap = std::max( diffPairGap, constraint.m_Value.Opt() );
 diffPairViaGap = std::max( diffPairViaGap, constraint.m_Value.Opt() );
 
 if( diffPairGap == constraint.m_Value.Opt() )
 aSizes.SetDiffPairGapSource( constraint.m_RuleName );
 }
 }
 else
 {
 diffPairWidth = bds.GetCurrentDiffPairWidth();
 diffPairGap = bds.GetCurrentDiffPairGap();
 diffPairViaGap = bds.GetCurrentDiffPairViaGap();
 
 aSizes.SetDiffPairWidthSource( _( "user choice" ) );
 aSizes.SetDiffPairGapSource( _( "user choice" ) );
 }
 
 aSizes.SetDiffPairWidth( diffPairWidth );
 aSizes.SetDiffPairGap( diffPairGap );
 aSizes.SetDiffPairViaGap( diffPairViaGap );
 aSizes.SetDiffPairViaGapSameAsTraceGap( false );
 
 int holeToHoleMin = bds.m_HoleToHoleMin;
 
 if( m_ruleResolver->QueryConstraint( PNS::CONSTRAINT_TYPE::CT_HOLE_TO_HOLE, &dummyVia,
 &dummyVia, UNDEFINED_LAYER, &constraint ) )
 {
 holeToHoleMin = constraint.m_Value.Min();
 }
 
 aSizes.SetHoleToHole( holeToHoleMin );
 
 if( m_ruleResolver->QueryConstraint( PNS::CONSTRAINT_TYPE::CT_HOLE_TO_HOLE, &dummyVia,
 &coupledVia, UNDEFINED_LAYER, &constraint ) )
 {
 holeToHoleMin = constraint.m_Value.Min();
 }
 
 aSizes.SetDiffPairHoleToHole( holeToHoleMin );
 
 return true;
}
 
 
int PNS_KICAD_IFACE_BASE::StackupHeight( int aFirstLayer, int aSecondLayer ) const
{
 if( !m_board || !m_board->GetDesignSettings().m_UseHeightForLengthCalcs )
 return 0;
 
 BOARD_STACKUP& stackup = m_board->GetDesignSettings().GetStackupDescriptor();
 
 return stackup.GetLayerDistance( GetBoardLayerFromPNSLayer( aFirstLayer ),
 GetBoardLayerFromPNSLayer( aSecondLayer ) );
}
 
 
PNS::NET_HANDLE PNS_PCBNEW_RULE_RESOLVER::DpCoupledNet( PNS::NET_HANDLE aNet )
{
 return m_board->DpCoupledNet( static_cast<NETINFO_ITEM*>( aNet ) );
}
 
 
int PNS_PCBNEW_RULE_RESOLVER::NetCode( PNS::NET_HANDLE aNet )
{
 return m_routerIface->GetNetCode( aNet );
}
 
 
wxString PNS_PCBNEW_RULE_RESOLVER::NetName( PNS::NET_HANDLE aNet )
{
 return m_routerIface->GetNetName( aNet );
}
 
 
int PNS_PCBNEW_RULE_RESOLVER::DpNetPolarity( PNS::NET_HANDLE aNet )
{
 wxString refName;
 
 if( NETINFO_ITEM* net = static_cast<NETINFO_ITEM*>( aNet ) )
 refName = net->GetNetname();
 
 wxString dummy1;
 
 return m_board->MatchDpSuffix( refName, dummy1 );
}
 
 
bool PNS_PCBNEW_RULE_RESOLVER::DpNetPair( const PNS::ITEM* aItem, PNS::NET_HANDLE& aNetP,
 PNS::NET_HANDLE& aNetN )
{
 if( !aItem || !aItem->Net() )
 return false;
 
 wxString netNameP = static_cast<NETINFO_ITEM*>( aItem->Net() )->GetNetname();
 wxString netNameN, netNameCoupled;
 
 int r = m_board->MatchDpSuffix( netNameP, netNameCoupled );
 
 if( r == 0 )
 {
 return false;
 }
 else if( r == 1 )
 {
 netNameN = netNameCoupled;
 }
 else
 {
 netNameN = netNameP;
 netNameP = netNameCoupled;
 }
 
 PNS::NET_HANDLE netInfoP = m_board->FindNet( netNameP );
 PNS::NET_HANDLE netInfoN = m_board->FindNet( netNameN );
 
 if( !netInfoP || !netInfoN )
 return false;
 
 aNetP = netInfoP;
 aNetN = netInfoN;
 
 return true;
}
 
 
class PNS_PCBNEW_DEBUG_DECORATOR: public PNS::DEBUG_DECORATOR
{
public:
 PNS_PCBNEW_DEBUG_DECORATOR( PNS::ROUTER_IFACE* aIface ) :
 PNS::DEBUG_DECORATOR(),
 m_iface( aIface ),
 m_view( nullptr ),
 m_items( nullptr ),
 m_depth( 0 )
 {}
 
 ~PNS_PCBNEW_DEBUG_DECORATOR()
 {
 PNS_PCBNEW_DEBUG_DECORATOR::Clear();
 delete m_items;
 }
 
 void SetView( KIGFX::VIEW* aView )
 {
 Clear();
 delete m_items;
 m_items = nullptr;
 m_view = aView;
 
 if( m_view == nullptr )
 return;
 
 if( m_view->GetGAL() )
 m_depth = m_view->GetGAL()->GetMinDepth();
 
 m_items = new KIGFX::VIEW_GROUP( m_view );
 m_items->SetLayer( LAYER_SELECT_OVERLAY ) ;
 m_view->Add( m_items );
 }
 
 void AddPoint( const VECTOR2I& aP, const KIGFX::COLOR4D& aColor, int aSize,
 const wxString& aName = wxT( "" ),
 const SRC_LOCATION_INFO& aSrcLoc = SRC_LOCATION_INFO() ) override
 
 {
 SHAPE_LINE_CHAIN sh;
 
 sh.SetWidth( 10000 );
 
 sh.Append( aP.x - aSize, aP.y - aSize );
 sh.Append( aP.x + aSize, aP.y + aSize );
 sh.Append( aP.x, aP.y );
 sh.Append( aP.x - aSize, aP.y + aSize );
 sh.Append( aP.x + aSize, aP.y - aSize );
 
 AddShape( &sh, aColor, sh.Width(), aName, aSrcLoc );
 }
 
 void AddItem( const PNS::ITEM* aItem, const KIGFX::COLOR4D& aColor, int aOverrideWidth = 0,
 const wxString& aName = wxT( "" ),
 const SRC_LOCATION_INFO& aSrcLoc = SRC_LOCATION_INFO() ) override
 {
 if( !m_view || !aItem )
 return;
 
 ROUTER_PREVIEW_ITEM* pitem = new ROUTER_PREVIEW_ITEM( aItem, m_iface, m_view );
 
 pitem->SetColor( aColor.WithAlpha( 0.5 ) );
 pitem->SetWidth( aOverrideWidth );
 pitem->SetDepth( nextDepth() );
 
 m_items->Add( pitem );
 m_view->Update( m_items );
 }
 
 void AddShape( const BOX2I& aBox, const KIGFX::COLOR4D& aColor, int aOverrideWidth = 0,
 const wxString& aName = wxT( "" ),
 const SRC_LOCATION_INFO& aSrcLoc = SRC_LOCATION_INFO() ) override
 {
 SHAPE_LINE_CHAIN l;
 l.SetWidth( aOverrideWidth );
 
 VECTOR2I o = aBox.GetOrigin();
 VECTOR2I s = aBox.GetSize();
 
 l.Append( o );
 l.Append( o.x + s.x, o.y );
 l.Append( o.x + s.x, o.y + s.y );
 l.Append( o.x, o.y + s.y );
 l.Append( o );
 
 AddShape( &l, aColor, aOverrideWidth, aName, aSrcLoc );
 }
 
 void AddShape( const SHAPE* aShape, const KIGFX::COLOR4D& aColor, int aOverrideWidth = 0,
 const wxString& aName = wxT( "" ),
 const SRC_LOCATION_INFO& aSrcLoc = SRC_LOCATION_INFO() ) override
 {
 if( !m_view || !aShape )
 return;
 
 ROUTER_PREVIEW_ITEM* pitem = new ROUTER_PREVIEW_ITEM( *aShape, m_iface, m_view );
 
 pitem->SetColor( aColor.WithAlpha( 0.5 ) );
 pitem->SetWidth( aOverrideWidth );
 pitem->SetDepth( nextDepth() );
 
 m_items->Add( pitem );
 m_view->Update( m_items );
 }
 
 void Clear() override
 {
 if( m_view && m_items )
 {
 m_items->FreeItems();
 m_view->Update( m_items );
 
 if( m_view->GetGAL() )
 m_depth = m_view->GetGAL()->GetMinDepth();
 }
 }
 
private:
 double nextDepth()
 {
 // Use different depths so that the transculent shapes won't overwrite each other.
 
 m_depth++;
 
 if( m_depth >= 0 && m_view->GetGAL() )
 m_depth = m_view->GetGAL()->GetMinDepth();
 
 return m_depth;
 }
 
 PNS::ROUTER_IFACE* m_iface;
 KIGFX::VIEW* m_view;
 KIGFX::VIEW_GROUP* m_items;
 
 double m_depth;
};
 
 
PNS::DEBUG_DECORATOR* PNS_KICAD_IFACE_BASE::GetDebugDecorator()
{
 return m_debugDecorator;
}
 
 
PNS_KICAD_IFACE_BASE::PNS_KICAD_IFACE_BASE()
{
 m_ruleResolver = nullptr;
 m_board = nullptr;
 m_world = nullptr;
 m_debugDecorator = nullptr;
 m_startLayer = -1;
}
 
 
PNS_KICAD_IFACE::PNS_KICAD_IFACE()
{
 m_tool = nullptr;
 m_view = nullptr;
 m_previewItems = nullptr;
 m_commitFlags = 0;
}
 
 
PNS_KICAD_IFACE_BASE::~PNS_KICAD_IFACE_BASE()
{
 delete m_ruleResolver;
 delete m_debugDecorator;
}
 
 
PNS_KICAD_IFACE::~PNS_KICAD_IFACE()
{
 if( m_previewItems )
 {
 m_previewItems->FreeItems();
 delete m_previewItems;
 }
}
 
 
std::vector<std::unique_ptr<PNS::SOLID>> PNS_KICAD_IFACE_BASE::syncPad( PAD* aPad )
{
 std::vector<std::unique_ptr<PNS::SOLID>> solids;
 PNS_LAYER_RANGE layers( 0, aPad->BoardCopperLayerCount() );
 LSEQ lmsk = aPad->GetLayerSet().CuStack();
 
 // ignore non-copper pads except for those with holes
 if( lmsk.empty() && aPad->GetDrillSize().x == 0 )
 return solids;
 
 switch( aPad->GetAttribute() )
 {
 case PAD_ATTRIB::PTH:
 case PAD_ATTRIB::NPTH:
 break;
 
 case PAD_ATTRIB::CONN:
 case PAD_ATTRIB::SMD:
 {
 bool is_copper = false;
 
 if( !lmsk.empty() && aPad->GetAttribute() != PAD_ATTRIB::NPTH )
 {
 layers = SetLayersFromPCBNew( lmsk.front(), lmsk.front() );
 is_copper = true;
 }
 
 if( !is_copper )
 return solids;
 
 break;
 }
 
 default:
 wxLogTrace( wxT( "PNS" ), wxT( "unsupported pad type 0x%x" ), aPad->GetAttribute() );
 return solids;
 }
 
 auto makeSolidFromPadLayer =
 [&]( PCB_LAYER_ID aLayer )
 {
 std::unique_ptr<PNS::SOLID> solid = std::make_unique<PNS::SOLID>();
 
 if( aPad->GetAttribute() == PAD_ATTRIB::NPTH )
 solid->SetRoutable( false );
 
 if( aPad->Padstack().Mode() == PADSTACK::MODE::CUSTOM )
 {
 solid->SetLayers( GetPNSLayerFromBoardLayer( aLayer ) );
 }
 else if( aPad->Padstack().Mode() == PADSTACK::MODE::FRONT_INNER_BACK )
 {
 if( aLayer == F_Cu || aLayer == B_Cu )
 solid->SetLayers( GetPNSLayerFromBoardLayer( aLayer ) );
 else
 solid->SetLayers( PNS_LAYER_RANGE( 1, aPad->BoardCopperLayerCount() - 1 ) );
 }
 else
 {
 solid->SetLayers( layers );
 }
 
 solid->SetNet( aPad->GetNet() );
 solid->SetParent( aPad );
 solid->SetPadToDie( aPad->GetPadToDieLength() );
 solid->SetOrientation( aPad->GetOrientation() );
 
 if( aPad->IsFreePad() )
 solid->SetIsFreePad();
 
 VECTOR2I wx_c = aPad->ShapePos( aLayer );
 VECTOR2I offset = aPad->GetOffset( aLayer );
 
 VECTOR2I c( wx_c.x, wx_c.y );
 
 RotatePoint( offset, aPad->GetOrientation() );
 
 solid->SetPos( VECTOR2I( c.x - offset.x, c.y - offset.y ) );
 solid->SetOffset( VECTOR2I( offset.x, offset.y ) );
 
 if( aPad->GetDrillSize().x > 0 )
 solid->SetHole( new PNS::HOLE( aPad->GetEffectiveHoleShape()->Clone() ) );
 
 // We generate a single SOLID for a pad, so we have to treat it as ALWAYS_FLASHED and
 // then perform layer-specific flashing tests internally.
 const std::shared_ptr<SHAPE>& shape =
 aPad->GetEffectiveShape( aLayer, FLASHING::ALWAYS_FLASHED );
 
 if( shape->HasIndexableSubshapes() && shape->GetIndexableSubshapeCount() == 1 )
 {
 std::vector<const SHAPE*> subshapes;
 shape->GetIndexableSubshapes( subshapes );
 
 solid->SetShape( subshapes[0]->Clone() );
 }
 // For anything that's not a single shape we use a polygon. Multiple shapes have a tendency
 // to confuse the hull generator. https://gitlab.com/kicad/code/kicad/-/issues/15553
 else
 {
 const std::shared_ptr<SHAPE_POLY_SET>& poly =
 aPad->GetEffectivePolygon( aLayer, ERROR_OUTSIDE );
 
 if( poly->OutlineCount() )
 solid->SetShape( new SHAPE_SIMPLE( poly->Outline( 0 ) ) );
 }
 
 solids.emplace_back( std::move( solid ) );
 };
 
 aPad->Padstack().ForEachUniqueLayer( makeSolidFromPadLayer );
 
 return solids;
}
 
 
std::unique_ptr<PNS::SEGMENT> PNS_KICAD_IFACE_BASE::syncTrack( PCB_TRACK* aTrack )
{
 auto segment = std::make_unique<PNS::SEGMENT>( SEG( aTrack->GetStart(), aTrack->GetEnd() ),
 aTrack->GetNet() );
 
 segment->SetWidth( aTrack->GetWidth() );
 segment->SetLayer( GetPNSLayerFromBoardLayer( aTrack->GetLayer() ) );
 segment->SetParent( aTrack );
 
 if( aTrack->IsLocked() )
 segment->Mark( PNS::MK_LOCKED );
 
 if( PCB_GENERATOR* generator = dynamic_cast<PCB_GENERATOR*>( aTrack->GetParentGroup() ) )
 {
 if( !generator->HasFlag( IN_EDIT ) )
 segment->Mark( PNS::MK_LOCKED );
 }
 
 return segment;
}
 
 
std::unique_ptr<PNS::ARC> PNS_KICAD_IFACE_BASE::syncArc( PCB_ARC* aArc )
{
 auto arc = std::make_unique<PNS::ARC>( SHAPE_ARC( aArc->GetStart(), aArc->GetMid(),
 aArc->GetEnd(), aArc->GetWidth() ),
 aArc->GetNet() );
 
 arc->SetLayer( GetPNSLayerFromBoardLayer( aArc->GetLayer() ) );
 arc->SetParent( aArc );
 
 if( aArc->IsLocked() )
 arc->Mark( PNS::MK_LOCKED );
 
 if( PCB_GENERATOR* generator = dynamic_cast<PCB_GENERATOR*>( aArc->GetParentGroup() ) )
 {
 if( !generator->HasFlag( IN_EDIT ) )
 arc->Mark( PNS::MK_LOCKED );
 }
 
 return arc;
}
 
 
std::vector<std::unique_ptr<PNS::VIA>> PNS_KICAD_IFACE_BASE::syncVia( PCB_VIA* aVia )
{
 std::vector<std::unique_ptr<PNS::VIA>> vias;
 PCB_LAYER_ID top, bottom;
 aVia->LayerPair( &top, &bottom );
 
 aVia->Padstack().ForEachUniqueLayer(
 [&]( PCB_LAYER_ID aLayer )
 {
 auto via = std::make_unique<PNS::VIA>( aVia->GetPosition(),
 SetLayersFromPCBNew( aVia->TopLayer(), aVia->BottomLayer() ),
 aVia->GetWidth( aLayer ),
 aVia->GetDrillValue(),
 aVia->GetNet(),
 aVia->GetViaType() );
 
 via->SetParent( aVia );
 
 if( aVia->IsLocked() )
 via->Mark( PNS::MK_LOCKED );
 
 if( PCB_GENERATOR* generator = dynamic_cast<PCB_GENERATOR*>( aVia->GetParentGroup() ) )
 {
 if( !generator->HasFlag( IN_EDIT ) )
 via->Mark( PNS::MK_LOCKED );
 }
 
 via->SetIsFree( aVia->GetIsFree() );
 via->SetHole( PNS::HOLE::MakeCircularHole( aVia->GetPosition(),
 aVia->GetDrillValue() / 2 ) );
 vias.emplace_back( std::move( via ) );
 } );
 
 return vias;
}
 
 
bool PNS_KICAD_IFACE_BASE::syncZone( PNS::NODE* aWorld, ZONE* aZone, SHAPE_POLY_SET* aBoardOutline )
{
 static wxString msg;
 SHAPE_POLY_SET* poly;
 
 if( !aZone->GetIsRuleArea() || !aZone->HasKeepoutParametersSet() )
 return false;
 
 LSET layers = aZone->GetLayerSet();
 
 poly = aZone->Outline();
 poly->CacheTriangulation( false );
 
 if( !poly->IsTriangulationUpToDate() )
 {
 UNITS_PROVIDER unitsProvider( pcbIUScale, GetUnits() );
 msg.Printf( _( "%s is malformed." ), aZone->GetItemDescription( &unitsProvider, true ) );
 
 KIDIALOG dlg( nullptr, msg, KIDIALOG::KD_WARNING );
 dlg.ShowDetailedText( _( "This zone cannot be handled by the router.\n"
 "Please verify it is not a self-intersecting polygon." ) );
 dlg.DoNotShowCheckbox( __FILE__, __LINE__ );
 dlg.ShowModal();
 
 return false;
 }
 
 for( PCB_LAYER_ID layer : LAYER_RANGE( F_Cu, B_Cu, m_board->GetCopperLayerCount() ) )
 {
 if( !layers[ layer ] )
 continue;
 
 for( int polyId = 0; polyId < poly->TriangulatedPolyCount(); polyId++ )
 {
 const SHAPE_POLY_SET::TRIANGULATED_POLYGON* tri = poly->TriangulatedPolygon( polyId );
 
 for( size_t i = 0; i < tri->GetTriangleCount(); i++)
 {
 VECTOR2I a, b, c;
 tri->GetTriangle( i, a, b, c );
 SHAPE_SIMPLE* triShape = new SHAPE_SIMPLE;
 
 triShape->Append( a );
 triShape->Append( b );
 triShape->Append( c );
 
 std::unique_ptr<PNS::SOLID> solid = std::make_unique<PNS::SOLID>();
 
 solid->SetLayer( GetPNSLayerFromBoardLayer( layer ) );
 solid->SetNet( nullptr );
 solid->SetParent( aZone );
 solid->SetShape( triShape );
 solid->SetIsCompoundShapePrimitive();
 solid->SetRoutable( false );
 
 aWorld->Add( std::move( solid ) );
 }
 }
 }
 
 return true;
}
 
 
bool PNS_KICAD_IFACE_BASE::syncTextItem( PNS::NODE* aWorld, PCB_TEXT* aText, PCB_LAYER_ID aLayer )
{
 if( !IsKicadCopperLayer( aLayer ) )
 return false;
 
 std::unique_ptr<PNS::SOLID> solid = std::make_unique<PNS::SOLID>();
 SHAPE_SIMPLE* shape = new SHAPE_SIMPLE;
 
 solid->SetLayer( GetPNSLayerFromBoardLayer( aLayer ) );
 solid->SetNet( nullptr );
 solid->SetParent( aText );
 solid->SetShape( shape ); // takes ownership
 solid->SetRoutable( false );
 
 SHAPE_POLY_SET cornerBuffer;
 
 aText->TransformShapeToPolygon( cornerBuffer, aText->GetLayer(), 0,
 m_board->GetDesignSettings().m_MaxError, ERROR_OUTSIDE );
 
 if( !cornerBuffer.OutlineCount() )
 return false;
 
 for( const VECTOR2I& pt : cornerBuffer.Outline( 0 ).CPoints() )
 shape->Append( pt );
 
 aWorld->Add( std::move( solid ) );
 
 return true;
}
 
 
bool PNS_KICAD_IFACE_BASE::syncGraphicalItem( PNS::NODE* aWorld, PCB_SHAPE* aItem )
{
 if( aItem->GetLayer() == Edge_Cuts
 || aItem->GetLayer() == Margin
 || IsKicadCopperLayer( aItem->GetLayer() ) )
 {
 std::vector<SHAPE*> shapes = aItem->MakeEffectiveShapes();
 
 for( SHAPE* shape : shapes )
 {
 std::unique_ptr<PNS::SOLID> solid = std::make_unique<PNS::SOLID>();
 
 if( aItem->GetLayer() == Edge_Cuts || aItem->GetLayer() == Margin )
 {
 solid->SetLayers( PNS_LAYER_RANGE( 0, m_board->GetCopperLayerCount() ) );
 solid->SetRoutable( false );
 }
 else
 {
 solid->SetLayer( GetPNSLayerFromBoardLayer( aItem->GetLayer() ) );
 }
 
 if( aItem->GetLayer() == Edge_Cuts )
 {
 switch( shape->Type() )
 {
 case SH_SEGMENT: static_cast<SHAPE_SEGMENT*>( shape )->SetWidth( 0 ); break;
 case SH_ARC: static_cast<SHAPE_ARC*>( shape )->SetWidth( 0 ); break;
 case SH_LINE_CHAIN: static_cast<SHAPE_LINE_CHAIN*>( shape )->SetWidth( 0 ); break;
 default: /* remaining shapes don't have width */ break;
 }
 }
 
 solid->SetAnchorPoints( aItem->GetConnectionPoints() );
 solid->SetNet( aItem->GetNet() );
 solid->SetParent( aItem );
 solid->SetShape( shape ); // takes ownership
 
 if( shapes.size() > 1 )
 solid->SetIsCompoundShapePrimitive();
 
 aWorld->Add( std::move( solid ) );
 }
 
 return true;
 }
 
 return false;
}
 
 
void PNS_KICAD_IFACE_BASE::SetBoard( BOARD* aBoard )
{
 m_board = aBoard;
 wxLogTrace( wxT( "PNS" ), wxT( "m_board = %p" ), m_board );
}
 
 
bool PNS_KICAD_IFACE_BASE::IsPNSCopperLayer( int aPNSLayer ) const
{
 return ::IsCopperLayer( GetBoardLayerFromPNSLayer( aPNSLayer ) );
}
 
 
 
bool PNS_KICAD_IFACE_BASE::IsKicadCopperLayer( PCB_LAYER_ID aKicadLayer ) const
{
 return ::IsCopperLayer( aKicadLayer );
}
 
 
bool PNS_KICAD_IFACE::IsAnyLayerVisible( const PNS_LAYER_RANGE& aLayer ) const
{
 if( !m_view )
 return false;
 
 for( int i = aLayer.Start(); i <= aLayer.End(); i++ )
 {
 if( m_view->IsLayerVisible( GetBoardLayerFromPNSLayer( i ) ) )
 return true;
 }
 
 return false;
}
 
 
bool PNS_KICAD_IFACE_BASE::IsFlashedOnLayer( const PNS::ITEM* aItem, int aLayer ) const
{
 if( aLayer < 0 )
 return true;
 
 if( aItem->Parent() )
 {
 switch( aItem->Parent()->Type() )
 {
 case PCB_VIA_T:
 {
 const PCB_VIA* via = static_cast<const PCB_VIA*>( aItem->Parent() );
 
 return via->FlashLayer( GetBoardLayerFromPNSLayer( aLayer ) );
 }
 
 case PCB_PAD_T:
 {
 const PAD* pad = static_cast<const PAD*>( aItem->Parent() );
 
 return pad->FlashLayer( GetBoardLayerFromPNSLayer( aLayer ) );
 }
 
 default:
 break;
 }
 }
 
 return aItem->Layers().Overlaps( aLayer );
}
 
 
bool PNS_KICAD_IFACE_BASE::IsFlashedOnLayer( const PNS::ITEM* aItem,
 const PNS_LAYER_RANGE& aLayer ) const
{
 PNS_LAYER_RANGE test = aItem->Layers().Intersection( aLayer );
 
 if( aItem->Parent() )
 {
 switch( aItem->Parent()->Type() )
 {
 case PCB_VIA_T:
 {
 const PCB_VIA* via = static_cast<const PCB_VIA*>( aItem->Parent() );
 
 for( int layer = test.Start(); layer <= test.End(); ++layer )
 {
 if( via->FlashLayer( GetBoardLayerFromPNSLayer( layer ) ) )
 return true;
 }
 
 return false;
 }
 
 case PCB_PAD_T:
 {
 const PAD* pad = static_cast<const PAD*>( aItem->Parent() );
 
 for( int layer = test.Start(); layer <= test.End(); ++layer )
 {
 if( pad->FlashLayer( GetBoardLayerFromPNSLayer( layer ) ) )
 return true;
 }
 
 return false;
 }
 
 default:
 break;
 }
 }
 
 return test.Start() <= test.End();
}
 
 
bool PNS_KICAD_IFACE::IsItemVisible( const PNS::ITEM* aItem ) const
{
 // by default, all items are visible (new ones created by the router have parent == NULL
 // as they have not been committed yet to the BOARD)
 if( !m_view || !aItem->Parent() )
 return true;
 
 BOARD_ITEM* item = aItem->Parent();
 bool isOnVisibleLayer = true;
 RENDER_SETTINGS* settings = m_view->GetPainter()->GetSettings();
 
 if( settings->GetHighContrast() )
 isOnVisibleLayer = item->IsOnLayer( settings->GetPrimaryHighContrastLayer() );
 
 if( m_view->IsVisible( item ) && isOnVisibleLayer )
 {
 for( PCB_LAYER_ID layer : item->GetLayerSet().Seq() )
 {
 if( item->ViewGetLOD( layer, m_view ) < m_view->GetScale() )
 return true;
 }
 }
 
 // Items hidden in the router are not hidden on the board
 if( m_hiddenItems.find( item ) != m_hiddenItems.end() )
 return true;
 
 return false;
}
 
 
void PNS_KICAD_IFACE_BASE::SyncWorld( PNS::NODE *aWorld )
{
 if( !m_board )
 {
 wxLogTrace( wxT( "PNS" ), wxT( "No board attached, aborting sync." ) );
 return;
 }
 
 int worstClearance = m_board->GetMaxClearanceValue();
 
 m_world = aWorld;
 
 for( BOARD_ITEM* gitem : m_board->Drawings() )
 {
 if ( gitem->Type() == PCB_SHAPE_T || gitem->Type() == PCB_TEXTBOX_T )
 {
 syncGraphicalItem( aWorld, static_cast<PCB_SHAPE*>( gitem ) );
 }
 else if( gitem->Type() == PCB_TEXT_T )
 {
 syncTextItem( aWorld, static_cast<PCB_TEXT*>( gitem ), gitem->GetLayer() );
 }
 }
 
 SHAPE_POLY_SET buffer;
 SHAPE_POLY_SET* boardOutline = nullptr;
 
 if( m_board->GetBoardPolygonOutlines( buffer ) )
 boardOutline = &buffer;
 
 for( ZONE* zone : m_board->Zones() )
 {
 syncZone( aWorld, zone, boardOutline );
 }
 
 for( FOOTPRINT* footprint : m_board->Footprints() )
 {
 for( PAD* pad : footprint->Pads() )
 {
 std::vector<std::unique_ptr<PNS::SOLID>> solids = syncPad( pad );
 
 for( std::unique_ptr<PNS::SOLID>& solid : solids )
 aWorld->Add( std::move( solid ) );
 
 std::optional<int> clearanceOverride = pad->GetClearanceOverrides( nullptr );
 
 if( clearanceOverride.has_value() )
 worstClearance = std::max( worstClearance, clearanceOverride.value() );
 
 if( pad->GetProperty() == PAD_PROP::CASTELLATED )
 {
 std::unique_ptr<SHAPE> hole;
 hole.reset( pad->GetEffectiveHoleShape()->Clone() );
 aWorld->AddEdgeExclusion( std::move( hole ) );
 }
 }
 
 syncTextItem( aWorld, &footprint->Reference(), footprint->Reference().GetLayer() );
 syncTextItem( aWorld, &footprint->Value(), footprint->Value().GetLayer() );
 
 for( ZONE* zone : footprint->Zones() )
 syncZone( aWorld, zone, boardOutline );
 
 for( PCB_FIELD* field : footprint->Fields() )
 syncTextItem( aWorld, static_cast<PCB_TEXT*>( field ), field->GetLayer() );
 
 for( BOARD_ITEM* item : footprint->GraphicalItems() )
 {
 if( item->Type() == PCB_SHAPE_T || item->Type() == PCB_TEXTBOX_T )
 {
 syncGraphicalItem( aWorld, static_cast<PCB_SHAPE*>( item ) );
 }
 else if( item->Type() == PCB_TEXT_T )
 {
 syncTextItem( aWorld, static_cast<PCB_TEXT*>( item ), item->GetLayer() );
 }
 }
 }
 
 for( PCB_TRACK* t : m_board->Tracks() )
 {
 KICAD_T type = t->Type();
 
 if( type == PCB_TRACE_T )
 {
 if( std::unique_ptr<PNS::SEGMENT> segment = syncTrack( t ) )
 aWorld->Add( std::move( segment ) );
 }
 else if( type == PCB_ARC_T )
 {
 if( std::unique_ptr<PNS::ARC> arc = syncArc( static_cast<PCB_ARC*>( t ) ) )
 aWorld->Add( std::move( arc ) );
 }
 else if( type == PCB_VIA_T )
 {
 std::vector<std::unique_ptr<PNS::VIA>> vias = syncVia( static_cast<PCB_VIA*>( t ) );
 
 for( std::unique_ptr<PNS::VIA>& via : vias )
 aWorld->Add( std::move( via ) );
 }
 }
 
 // NB: if this were ever to become a long-lived object we would need to dirty its
 // clearance cache here....
 delete m_ruleResolver;
 m_ruleResolver = new PNS_PCBNEW_RULE_RESOLVER( m_board, this );
 
 aWorld->SetRuleResolver( m_ruleResolver );
 aWorld->SetMaxClearance( worstClearance + m_ruleResolver->ClearanceEpsilon() );
}
 
 
void PNS_KICAD_IFACE::EraseView()
{
 for( BOARD_ITEM* item : m_hiddenItems )
 m_view->SetVisible( item, true );
 
 m_hiddenItems.clear();
 
 if( m_previewItems )
 {
 m_previewItems->FreeItems();
 m_view->Update( m_previewItems );
 }
 
 if( m_debugDecorator )
 m_debugDecorator->Clear();
}
 
 
void PNS_KICAD_IFACE_BASE::SetDebugDecorator( PNS::DEBUG_DECORATOR *aDec )
{
 m_debugDecorator = aDec;
}
 
 
void PNS_KICAD_IFACE::DisplayItem( const PNS::ITEM* aItem, int aClearance, bool aEdit, int aFlags )
{
 if( aItem->IsVirtual() )
 return;
 
 if( ZONE* zone = dynamic_cast<ZONE*>( aItem->Parent() ) )
 {
 if( zone->GetIsRuleArea() )
 aFlags |= PNS_SEMI_SOLID;
 }
 
 ROUTER_PREVIEW_ITEM* pitem = new ROUTER_PREVIEW_ITEM( aItem, this, m_view, aFlags );
 
 // Note: SEGMENT_T is used for placed tracks; LINE_T is used for the routing head
 static int tracks = PNS::ITEM::SEGMENT_T | PNS::ITEM::ARC_T | PNS::ITEM::LINE_T;
 static int tracksOrVias = tracks | PNS::ITEM::VIA_T;
 
 if( aClearance >= 0 )
 {
 pitem->SetClearance( aClearance );
 
 auto* settings = static_cast<PCBNEW_SETTINGS*>( m_tool->GetManager()->GetSettings() );
 
 switch( settings->m_Display.m_TrackClearance )
 {
 case SHOW_WITH_VIA_ALWAYS:
 case SHOW_WITH_VIA_WHILE_ROUTING_OR_DRAGGING:
 pitem->ShowClearance( aItem->OfKind( tracksOrVias ) );
 break;
 
 case SHOW_WITH_VIA_WHILE_ROUTING:
 pitem->ShowClearance( aItem->OfKind( tracksOrVias ) && !aEdit );
 break;
 
 case SHOW_WHILE_ROUTING:
 pitem->ShowClearance( aItem->OfKind( tracks ) && !aEdit );
 break;
 
 default:
 pitem->ShowClearance( false );
 break;
 }
 }
 
 m_previewItems->Add( pitem );
 m_view->Update( m_previewItems );
}
 
 
void PNS_KICAD_IFACE::DisplayPathLine( const SHAPE_LINE_CHAIN& aLine, int aImportance )
{
 ROUTER_PREVIEW_ITEM* pitem = new ROUTER_PREVIEW_ITEM( aLine, this, m_view );
 pitem->SetDepth( pitem->GetOriginDepth() - ROUTER_PREVIEW_ITEM::PathOverlayDepth );
 
 COLOR4D color;
 
 if( aImportance >= 1 )
 color = COLOR4D( 1.0, 1.0, 0.0, 0.6 );
 else if( aImportance == 0 )
 color = COLOR4D( 0.7, 0.7, 0.7, 0.6 );
 
 pitem->SetColor( color );
 
 m_previewItems->Add( pitem );
 m_view->Update( m_previewItems );
}
 
 
void PNS_KICAD_IFACE::DisplayRatline( const SHAPE_LINE_CHAIN& aRatline, PNS::NET_HANDLE aNet )
{
 ROUTER_PREVIEW_ITEM* pitem = new ROUTER_PREVIEW_ITEM( aRatline, this, m_view );
 
 KIGFX::RENDER_SETTINGS* renderSettings = m_view->GetPainter()->GetSettings();
 KIGFX::PCB_RENDER_SETTINGS* rs = static_cast<KIGFX::PCB_RENDER_SETTINGS*>( renderSettings );
 bool colorByNet = rs->GetNetColorMode() != NET_COLOR_MODE::OFF;
 COLOR4D defaultColor = rs->GetColor( nullptr, LAYER_RATSNEST );
 COLOR4D color = defaultColor;
 
 std::shared_ptr<CONNECTIVITY_DATA> connectivity = m_board->GetConnectivity();
 std::set<int> highlightedNets = rs->GetHighlightNetCodes();
 std::map<int, KIGFX::COLOR4D>& netColors = rs->GetNetColorMap();
 int netCode = -1;
 
 if( NETINFO_ITEM* net = static_cast<NETINFO_ITEM*>( aNet ) )
 netCode = net->GetNetCode();
 
 const NETCLASS* nc = nullptr;
 const NET_SETTINGS* netSettings = connectivity->GetNetSettings();
 
 if( connectivity->HasNetNameForNetCode( netCode ) )
 {
 const wxString& netName = connectivity->GetNetNameForNetCode( netCode );
 
 if( netSettings && netSettings->HasEffectiveNetClass( netName ) )
 nc = netSettings->GetCachedEffectiveNetClass( netName ).get();
 }
 
 if( colorByNet && netColors.count( netCode ) )
 color = netColors.at( netCode );
 else if( colorByNet && nc && nc->HasPcbColor() )
 color = nc->GetPcbColor();
 else
 color = defaultColor;
 
 if( color == COLOR4D::UNSPECIFIED )
 color = defaultColor;
 
 pitem->SetColor( color.Brightened( 0.5 ).WithAlpha( std::min( 1.0, color.a + 0.4 ) ) );
 
 m_previewItems->Add( pitem );
 m_view->Update( m_previewItems );
}
 
 
void PNS_KICAD_IFACE::HideItem( PNS::ITEM* aItem )
{
 BOARD_ITEM* parent = aItem->Parent();
 
 if( parent )
 {
 if( m_view->IsVisible( parent ) )
 m_hiddenItems.insert( parent );
 
 m_view->SetVisible( parent, false );
 m_view->Update( parent, KIGFX::APPEARANCE );
 
 for( ZONE* td : m_board->Zones() )
 {
 if( td->IsTeardropArea()
 && td->GetBoundingBox().Intersects( aItem->Parent()->GetBoundingBox() )
 && td->Outline()->Collide( aItem->Shape() ) )
 {
 m_view->SetVisible( td, false );
 m_view->Update( td, KIGFX::APPEARANCE );
 }
 }
 }
}
 
 
void PNS_KICAD_IFACE_BASE::RemoveItem( PNS::ITEM* aItem )
{
}
 
 
void PNS_KICAD_IFACE::RemoveItem( PNS::ITEM* aItem )
{
 BOARD_ITEM* parent = aItem->Parent();
 
 if( aItem->OfKind( PNS::ITEM::SOLID_T ) )
 {
 PAD* pad = static_cast<PAD*>( parent );
 VECTOR2I pos = static_cast<PNS::SOLID*>( aItem )->Pos();
 
 m_fpOffsets[ pad ].p_old = pos;
 return;
 }
 
 if( parent )
 {
 m_commit->Remove( parent );
 }
}
 
 
void PNS_KICAD_IFACE_BASE::UpdateItem( PNS::ITEM* aItem )
{
}
 
 
void PNS_KICAD_IFACE::modifyBoardItem( PNS::ITEM* aItem )
{
 BOARD_ITEM* board_item = aItem->Parent();
 
 switch( aItem->Kind() )
 {
 case PNS::ITEM::ARC_T:
 {
 PNS::ARC* arc = static_cast<PNS::ARC*>( aItem );
 PCB_ARC* arc_board = static_cast<PCB_ARC*>( board_item );
 const SHAPE_ARC* arc_shape = static_cast<const SHAPE_ARC*>( arc->Shape() );
 
 m_commit->Modify( arc_board );
 
 arc_board->SetStart( VECTOR2I( arc_shape->GetP0() ) );
 arc_board->SetEnd( VECTOR2I( arc_shape->GetP1() ) );
 arc_board->SetMid( VECTOR2I( arc_shape->GetArcMid() ) );
 arc_board->SetWidth( arc->Width() );
 break;
 }
 
 case PNS::ITEM::SEGMENT_T:
 {
 PNS::SEGMENT* seg = static_cast<PNS::SEGMENT*>( aItem );
 PCB_TRACK* track = static_cast<PCB_TRACK*>( board_item );
 const SEG& s = seg->Seg();
 
 m_commit->Modify( track );
 
 track->SetStart( VECTOR2I( s.A.x, s.A.y ) );
 track->SetEnd( VECTOR2I( s.B.x, s.B.y ) );
 track->SetWidth( seg->Width() );
 break;
 }
 
 case PNS::ITEM::VIA_T:
 {
 PCB_VIA* via_board = static_cast<PCB_VIA*>( board_item );
 PNS::VIA* via = static_cast<PNS::VIA*>( aItem );
 
 m_commit->Modify( via_board );
 
 via_board->SetPosition( VECTOR2I( via->Pos().x, via->Pos().y ) );
 via_board->SetWidth( PADSTACK::ALL_LAYERS, via->Diameter() );
 via_board->SetDrill( via->Drill() );
 via_board->SetNet( static_cast<NETINFO_ITEM*>( via->Net() ) );
 via_board->SetViaType( via->ViaType() ); // MUST be before SetLayerPair()
 via_board->SetIsFree( via->IsFree() );
 via_board->SetLayerPair( GetBoardLayerFromPNSLayer( via->Layers().Start() ),
 GetBoardLayerFromPNSLayer( via->Layers().End() ) );
 break;
 }
 
 case PNS::ITEM::SOLID_T:
 {
 PAD* pad = static_cast<PAD*>( aItem->Parent() );
 VECTOR2I pos = static_cast<PNS::SOLID*>( aItem )->Pos();
 
 // Don't add to commit; we'll add the parent footprints when processing the m_fpOffsets
 
 m_fpOffsets[pad].p_old = pad->GetPosition();
 m_fpOffsets[pad].p_new = pos;
 break;
 }
 
 default:
 m_commit->Modify( aItem->Parent() );
 break;
 }
}
 
 
void PNS_KICAD_IFACE::UpdateItem( PNS::ITEM* aItem )
{
 modifyBoardItem( aItem );
}
 
 
void PNS_KICAD_IFACE_BASE::AddItem( PNS::ITEM* aItem )
{
}
 
 
BOARD_CONNECTED_ITEM* PNS_KICAD_IFACE::createBoardItem( PNS::ITEM* aItem )
{
 BOARD_CONNECTED_ITEM* newBoardItem = nullptr;
 NETINFO_ITEM* net = static_cast<NETINFO_ITEM*>( aItem->Net() );
 
 if( !net )
 net = NETINFO_LIST::OrphanedItem();
 
 switch( aItem->Kind() )
 {
 case PNS::ITEM::ARC_T:
 {
 PNS::ARC* arc = static_cast<PNS::ARC*>( aItem );
 PCB_ARC* new_arc = new PCB_ARC( m_board, static_cast<const SHAPE_ARC*>( arc->Shape() ) );
 new_arc->SetWidth( arc->Width() );
 new_arc->SetLayer( GetBoardLayerFromPNSLayer( arc->Layers().Start() ) );
 new_arc->SetNet( net );
 newBoardItem = new_arc;
 break;
 }
 
 case PNS::ITEM::SEGMENT_T:
 {
 PNS::SEGMENT* seg = static_cast<PNS::SEGMENT*>( aItem );
 PCB_TRACK* track = new PCB_TRACK( m_board );
 const SEG& s = seg->Seg();
 track->SetStart( VECTOR2I( s.A.x, s.A.y ) );
 track->SetEnd( VECTOR2I( s.B.x, s.B.y ) );
 track->SetWidth( seg->Width() );
 track->SetLayer( GetBoardLayerFromPNSLayer( seg->Layers().Start() ) );
 track->SetNet( net );
 newBoardItem = track;
 break;
 }
 
 case PNS::ITEM::VIA_T:
 {
 PCB_VIA* via_board = new PCB_VIA( m_board );
 PNS::VIA* via = static_cast<PNS::VIA*>( aItem );
 via_board->SetPosition( VECTOR2I( via->Pos().x, via->Pos().y ) );
 via_board->SetWidth( PADSTACK::ALL_LAYERS, via->Diameter() );
 via_board->SetDrill( via->Drill() );
 via_board->SetNet( net );
 via_board->SetViaType( via->ViaType() ); // MUST be before SetLayerPair()
 via_board->SetIsFree( via->IsFree() );
 via_board->SetLayerPair( GetBoardLayerFromPNSLayer( via->Layers().Start() ),
 GetBoardLayerFromPNSLayer( via->Layers().End() ) );
 newBoardItem = via_board;
 break;
 }
 
 case PNS::ITEM::SOLID_T:
 {
 PAD* pad = static_cast<PAD*>( aItem->Parent() );
 VECTOR2I pos = static_cast<PNS::SOLID*>( aItem )->Pos();
 
 m_fpOffsets[pad].p_new = pos;
 return nullptr;
 }
 
 default:
 return nullptr;
 }
 
 if( net->GetNetCode() <= 0 )
 {
 NETINFO_ITEM* newNetInfo = newBoardItem->GetNet();
 
 newNetInfo->SetParent( m_board );
 newNetInfo->SetNetClass( m_board->GetDesignSettings().m_NetSettings->GetDefaultNetclass() );
 }
 
 return newBoardItem;
}
 
 
void PNS_KICAD_IFACE::AddItem( PNS::ITEM* aItem )
{
 BOARD_CONNECTED_ITEM* boardItem = createBoardItem( aItem );
 
 if( boardItem )
 {
 aItem->SetParent( boardItem );
 boardItem->ClearFlags();
 
 m_commit->Add( boardItem );
 }
}
 
 
void PNS_KICAD_IFACE::Commit()
{
 std::set<FOOTPRINT*> processedFootprints;
 
 EraseView();
 
 for( const auto& [ pad, fpOffset ] : m_fpOffsets )
 {
 VECTOR2I offset = fpOffset.p_new - fpOffset.p_old;
 FOOTPRINT* footprint = pad->GetParentFootprint();
 VECTOR2I p_orig = footprint->GetPosition();
 VECTOR2I p_new = p_orig + offset;
 
 if( processedFootprints.find( footprint ) != processedFootprints.end() )
 continue;
 
 processedFootprints.insert( footprint );
 m_commit->Modify( footprint );
 footprint->SetPosition( p_new );
 }
 
 m_fpOffsets.clear();
 
 m_commit->Push( _( "Routing" ), m_commitFlags );
 m_commit = std::make_unique<BOARD_COMMIT>( m_tool );
}
 
 
EDA_UNITS PNS_KICAD_IFACE::GetUnits() const
{
 return static_cast<EDA_UNITS>( m_tool->GetManager()->GetSettings()->m_System.units );
}
 
 
void PNS_KICAD_IFACE::SetView( KIGFX::VIEW* aView )
{
 wxLogTrace( wxT( "PNS" ), wxT( "SetView %p" ), aView );
 
 if( m_previewItems )
 {
 m_previewItems->FreeItems();
 delete m_previewItems;
 }
 
 m_view = aView;
 m_previewItems = new KIGFX::VIEW_GROUP( m_view );
 m_previewItems->SetLayer( LAYER_SELECT_OVERLAY ) ;
 
 if(m_view)
 m_view->Add( m_previewItems );
 
 delete m_debugDecorator;
 
 auto dec = new PNS_PCBNEW_DEBUG_DECORATOR( this );
 m_debugDecorator = dec;
 
 dec->SetDebugEnabled( ADVANCED_CFG::GetCfg().m_ShowRouterDebugGraphics );
 
 if( ADVANCED_CFG::GetCfg().m_ShowRouterDebugGraphics )
 dec->SetView( m_view );
}
 
 
int PNS_KICAD_IFACE::GetNetCode( PNS::NET_HANDLE aNet ) const
{
 if( aNet )
 return static_cast<NETINFO_ITEM*>( aNet )->GetNetCode();
 else
 return -1;
}
 
 
wxString PNS_KICAD_IFACE::GetNetName( PNS::NET_HANDLE aNet ) const
{
 if( aNet )
 return static_cast<NETINFO_ITEM*>( aNet )->GetNetname();
 else
 return wxEmptyString;
}
 
 
void PNS_KICAD_IFACE::UpdateNet( PNS::NET_HANDLE aNet )
{
 wxLogTrace( wxT( "PNS" ), wxT( "Update-net %s" ), GetNetName( aNet ) );
}
 
 
PNS::NET_HANDLE PNS_KICAD_IFACE_BASE::GetOrphanedNetHandle()
{
 return NETINFO_LIST::OrphanedItem();
}
 
 
PNS::RULE_RESOLVER* PNS_KICAD_IFACE_BASE::GetRuleResolver()
{
 return m_ruleResolver;
}
 
 
void PNS_KICAD_IFACE::SetHostTool( PCB_TOOL_BASE* aTool )
{
 m_tool = aTool;
 m_commit = std::make_unique<BOARD_COMMIT>( m_tool );
}
 
 
PCB_LAYER_ID PNS_KICAD_IFACE_BASE::GetBoardLayerFromPNSLayer( int aLayer ) const
{
 if( aLayer < 0 )
 return PCB_LAYER_ID::UNDEFINED_LAYER;
 
 if( aLayer == 0 )
 return F_Cu;
 
 if( aLayer == m_board->GetCopperLayerCount() - 1 )
 return B_Cu;
 
 return static_cast<PCB_LAYER_ID>( ( aLayer + 1 ) * 2 );
}
 
 
int PNS_KICAD_IFACE_BASE::GetPNSLayerFromBoardLayer( PCB_LAYER_ID aLayer ) const
{
 if( aLayer < 0 )
 return -1;
 
 if( aLayer == F_Cu )
 return 0;
 
 if( aLayer == B_Cu )
 return m_board->GetCopperLayerCount() - 1;
 
 return ( aLayer / 2 ) - 1;
}
 
 
void PNS_KICAD_IFACE_BASE::SetStartLayerFromPCBNew( PCB_LAYER_ID aLayer )
{
 m_startLayer = GetPNSLayerFromBoardLayer( aLayer );
}
 
 
PNS_LAYER_RANGE PNS_KICAD_IFACE_BASE::SetLayersFromPCBNew( PCB_LAYER_ID aStartLayer, PCB_LAYER_ID aEndLayer )
{
 return PNS_LAYER_RANGE( GetPNSLayerFromBoardLayer( aStartLayer ),
 GetPNSLayerFromBoardLayer( aEndLayer ) );
}