haskal
/
kicad
1
0
Fork 0
Code Issues Pull Requests Packages Projects Releases Wiki Activity
kicad/pcbnew/zones_convert_brd_items_to_...

510 lines
20 KiB
C++
Raw Blame History

/**
* @file zones_convert_brd_items_to_polygons_with_Boost.cpp
*/
/*
* This program source code file is part of KiCad, a free EDA CAD application.
*
* Copyright (C) 2012 Jean-Pierre Charras, jean-pierre.charras@ujf-grenoble.fr
* Copyright (C) 1992-2012 KiCad Developers, see AUTHORS.txt for contributors.
*
* 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 2
* 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, you may find one here:
* http://www.gnu.org/licenses/old-licenses/gpl-2.0.html
* or you may search the http://www.gnu.org website for the version 2 license,
* or you may write to the Free Software Foundation, Inc.,
* 51 Franklin Street, Fifth Floor, Boston, MA 02110-1301, USA
*/
/* Functions to convert some board items to polygons
* (pads, tracks ..)
* This is used to calculate filled areas in copper zones.
* Filled areas are areas remainder of the full zone area after removed all polygons
* calculated from these items shapes and the clearance area
*
* Important note:
* Because filled areas must have a minimum thickness to match with Design rule, they are
* draw in 2 step:
* 1 - filled polygons are drawn
* 2 - polygon outlines are drawn with a "minimum thickness width" ( or with a minimum
* thickness pen )
* So outlines of filled polygons are calculated with the constraint they match with clearance,
* taking in account outlines have thickness
* This ensures:
* - areas meet the minimum thickness requirement.
* - shapes are smoothed.
*/
// Polygon calculations can use fast mode or force strickly simple polygons after calculations
// Forcing strickly simple polygons is time consuming, and we have not see issues in fast mode
// so we use fast mode
#define POLY_CALC_MODE SHAPE_POLY_SET::PM_FAST
#include <cmath>
#include <sstream>
#include <fctsys.h>
#include <wxPcbStruct.h>
#include <trigo.h>
#include <class_board.h>
#include <class_module.h>
#include <class_track.h>
#include <class_edge_mod.h>
#include <class_drawsegment.h>
#include <class_pcb_text.h>
#include <class_zone.h>
#include <project.h>
#include <pcbnew.h>
#include <zones.h>
#include <convert_basic_shapes_to_polygon.h>
#include <geometry/shape_poly_set.h>
#include <geometry/shape_file_io.h>
#include <boost/foreach.hpp>
extern void BuildUnconnectedThermalStubsPolygonList( SHAPE_POLY_SET& aCornerBuffer,
BOARD* aPcb, ZONE_CONTAINER* aZone,
double aArcCorrection,
double aRoundPadThermalRotation);
extern void Test_For_Copper_Island_And_Remove( BOARD* aPcb,
ZONE_CONTAINER* aZone_container );
extern void CreateThermalReliefPadPolygon( SHAPE_POLY_SET& aCornerBuffer,
D_PAD& aPad,
int aThermalGap,
int aCopperThickness,
int aMinThicknessValue,
int aCircleToSegmentsCount,
double aCorrectionFactor,
double aThermalRot );
// Local Variables:
static double s_thermalRot = 450; // angle of stubs in thermal reliefs for round pads
void ZONE_CONTAINER::buildFeatureHoleList( BOARD* aPcb, SHAPE_POLY_SET& aFeatures )
{
int segsPerCircle;
double correctionFactor;
// Set the number of segments in arc approximations
if( m_ArcToSegmentsCount == ARC_APPROX_SEGMENTS_COUNT_HIGHT_DEF )
segsPerCircle = ARC_APPROX_SEGMENTS_COUNT_HIGHT_DEF;
else
segsPerCircle = ARC_APPROX_SEGMENTS_COUNT_LOW_DEF;
/* calculates the coeff to compensate radius reduction of holes clearance
* due to the segment approx.
* For a circle the min radius is radius * cos( 2PI / s_CircleToSegmentsCount / 2)
* s_Correction is 1 /cos( PI/s_CircleToSegmentsCount )
*/
correctionFactor = 1.0 / cos( M_PI / (double) segsPerCircle );
aFeatures.RemoveAllContours();
int outline_half_thickness = m_ZoneMinThickness / 2;
int zone_clearance = std::max( m_ZoneClearance, GetClearance() );
zone_clearance += outline_half_thickness;
/* store holes (i.e. tracks and pads areas as polygons outlines)
* in a polygon list
*/
/* items ouside the zone bounding box are skipped
* the bounding box is the zone bounding box + the biggest clearance found in Netclass list
*/
EDA_RECT item_boundingbox;
EDA_RECT zone_boundingbox = GetBoundingBox();
int biggest_clearance = aPcb->GetDesignSettings().GetBiggestClearanceValue();
biggest_clearance = std::max( biggest_clearance, zone_clearance );
zone_boundingbox.Inflate( biggest_clearance );
/*
* First : Add pads. Note: pads having the same net as zone are left in zone.
* Thermal shapes will be created later if necessary
*/
int item_clearance;
/* Use a dummy pad to calculate hole clerance when a pad is not on all copper layers
* and this pad has a hole
* This dummy pad has the size and shape of the hole
* Therefore, this dummy pad is a circle or an oval.
* A pad must have a parent because some functions expect a non null parent
* to find the parent board, and some other data
*/
MODULE dummymodule( aPcb ); // Creates a dummy parent
D_PAD dummypad( &dummymodule );
for( MODULE* module = aPcb->m_Modules; module; module = module->Next() )
{
D_PAD* nextpad;
for( D_PAD* pad = module->Pads(); pad != NULL; pad = nextpad )
{
nextpad = pad->Next(); // pad pointer can be modified by next code, so
// calculate the next pad here
if( !pad->IsOnLayer( GetLayer() ) )
{
/* Test for pads that are on top or bottom only and have a hole.
* There are curious pads but they can be used for some components that are
* inside the board (in fact inside the hole. Some photo diodes and Leds are
* like this)
*/
if( pad->GetDrillSize().x == 0 && pad->GetDrillSize().y == 0 )
continue;
// Use a dummy pad to calculate a hole shape that have the same dimension as
// the pad hole
dummypad.SetSize( pad->GetDrillSize() );
dummypad.SetOrientation( pad->GetOrientation() );
dummypad.SetShape( pad->GetDrillShape() == PAD_DRILL_SHAPE_OBLONG ?
PAD_SHAPE_OVAL : PAD_SHAPE_CIRCLE );
dummypad.SetPosition( pad->GetPosition() );
pad = &dummypad;
}
// Note: netcode <=0 means not connected item
if( ( pad->GetNetCode() != GetNetCode() ) || ( pad->GetNetCode() <= 0 ) )
{
item_clearance = pad->GetClearance() + outline_half_thickness;
item_boundingbox = pad->GetBoundingBox();
item_boundingbox.Inflate( item_clearance );
if( item_boundingbox.Intersects( zone_boundingbox ) )
{
int clearance = std::max( zone_clearance, item_clearance );
pad->TransformShapeWithClearanceToPolygon( aFeatures,
clearance,
segsPerCircle,
correctionFactor );
}
continue;
}
if( GetPadConnection( pad ) == PAD_ZONE_CONN_NONE )
{
int gap = zone_clearance;
int thermalGap = GetThermalReliefGap( pad );
gap = std::max( gap, thermalGap );
item_boundingbox = pad->GetBoundingBox();
if( item_boundingbox.Intersects( zone_boundingbox ) )
{
pad->TransformShapeWithClearanceToPolygon( aFeatures,
gap,
segsPerCircle,
correctionFactor );
}
}
}
}
/* Add holes (i.e. tracks and vias areas as polygons outlines)
* in cornerBufferPolysToSubstract
*/
for( TRACK* track = aPcb->m_Track; track; track = track->Next() )
{
if( !track->IsOnLayer( GetLayer() ) )
continue;
if( track->GetNetCode() == GetNetCode() && (GetNetCode() != 0) )
continue;
item_clearance = track->GetClearance() + outline_half_thickness;
item_boundingbox = track->GetBoundingBox();
if( item_boundingbox.Intersects( zone_boundingbox ) )
{
int clearance = std::max( zone_clearance, item_clearance );
track->TransformShapeWithClearanceToPolygon( aFeatures,
clearance,
segsPerCircle,
correctionFactor );
}
}
/* Add module edge items that are on copper layers
* Pcbnew allows these items to be on copper layers in microwave applictions
* This is a bad thing, but must be handled here, until a better way is found
*/
for( MODULE* module = aPcb->m_Modules; module; module = module->Next() )
{
for( BOARD_ITEM* item = module->GraphicalItems(); item; item = item->Next() )
{
if( !item->IsOnLayer( GetLayer() ) && !item->IsOnLayer( Edge_Cuts ) )
continue;
if( item->Type() != PCB_MODULE_EDGE_T )
continue;
item_boundingbox = item->GetBoundingBox();
if( item_boundingbox.Intersects( zone_boundingbox ) )
{
( (EDGE_MODULE*) item )->TransformShapeWithClearanceToPolygon(
aFeatures, zone_clearance,
segsPerCircle, correctionFactor );
}
}
}
// Add graphic items (copper texts) and board edges
for( BOARD_ITEM* item = aPcb->m_Drawings; item; item = item->Next() )
{
if( item->GetLayer() != GetLayer() && item->GetLayer() != Edge_Cuts )
continue;
switch( item->Type() )
{
case PCB_LINE_T:
( (DRAWSEGMENT*) item )->TransformShapeWithClearanceToPolygon(
aFeatures,
zone_clearance, segsPerCircle, correctionFactor );
break;
case PCB_TEXT_T:
( (TEXTE_PCB*) item )->TransformBoundingBoxWithClearanceToPolygon(
aFeatures, zone_clearance );
break;
default:
break;
}
}
// Add zones outlines having an higher priority and keepout
for( int ii = 0; ii < GetBoard()->GetAreaCount(); ii++ )
{
ZONE_CONTAINER* zone = GetBoard()->GetArea( ii );
if( zone->GetLayer() != GetLayer() )
continue;
if( !zone->GetIsKeepout() && zone->GetPriority() <= GetPriority() )
continue;
if( zone->GetIsKeepout() && ! zone->GetDoNotAllowCopperPour() )
continue;
// A highter priority zone or keepout area is found: remove this area
item_boundingbox = zone->GetBoundingBox();
if( !item_boundingbox.Intersects( zone_boundingbox ) )
continue;
// Add the zone outline area.
// However if the zone has the same net as the current zone,
// do not add any clearance.
// the zone will be connected to the current zone, but filled areas
// will use different parameters (clearance, thermal shapes )
bool same_net = GetNetCode() == zone->GetNetCode();
bool use_net_clearance = true;
int min_clearance = zone_clearance;
// Do not forget to make room to draw the thick outlines
// of the hole created by the area of the zone to remove
int holeclearance = zone->GetClearance() + outline_half_thickness;
// The final clearance is obviously the max value of each zone clearance
min_clearance = std::max( min_clearance, holeclearance );
if( zone->GetIsKeepout() || same_net )
{
// Just take in account the fact the outline has a thickness, so
// the actual area to substract is inflated to take in account this fact
min_clearance = outline_half_thickness;
use_net_clearance = false;
}
zone->TransformOutlinesShapeWithClearanceToPolygon(
aFeatures,
min_clearance, use_net_clearance );
}
// Remove thermal symbols
for( MODULE* module = aPcb->m_Modules; module; module = module->Next() )
{
for( D_PAD* pad = module->Pads(); pad != NULL; pad = pad->Next() )
{
// Rejects non-standard pads with tht-only thermal reliefs
if( GetPadConnection( pad ) == PAD_ZONE_CONN_THT_THERMAL
&& pad->GetAttribute() != PAD_ATTRIB_STANDARD )
continue;
if( GetPadConnection( pad ) != PAD_ZONE_CONN_THERMAL
&& GetPadConnection( pad ) != PAD_ZONE_CONN_THT_THERMAL )
continue;
if( !pad->IsOnLayer( GetLayer() ) )
continue;
if( pad->GetNetCode() != GetNetCode() )
continue;
item_boundingbox = pad->GetBoundingBox();
int thermalGap = GetThermalReliefGap( pad );
item_boundingbox.Inflate( thermalGap, thermalGap );
if( item_boundingbox.Intersects( zone_boundingbox ) )
{
CreateThermalReliefPadPolygon( aFeatures,
*pad, thermalGap,
GetThermalReliefCopperBridge( pad ),
m_ZoneMinThickness,
segsPerCircle,
correctionFactor, s_thermalRot );
}
}
}
}
/**
* Function AddClearanceAreasPolygonsToPolysList
* Supports a min thickness area constraint.
* Add non copper areas polygons (pads and tracks with clearance)
* to the filled copper area found
* in BuildFilledPolysListData after calculating filled areas in a zone
* Non filled copper areas are pads and track and their clearance areas
* The filled copper area must be computed just before.
* BuildFilledPolysListData() call this function just after creating the
* filled copper area polygon (without clearance areas)
* to do that this function:
* 1 - Creates the main outline (zone outline) using a correction to shrink the resulting area
* with m_ZoneMinThickness/2 value.
* The result is areas with a margin of m_ZoneMinThickness/2
* When drawing outline with segments having a thickness of m_ZoneMinThickness, the
* outlines will match exactly the initial outlines
* 3 - Add all non filled areas (pads, tracks) in group B with a clearance of m_Clearance +
* m_ZoneMinThickness/2
* in a buffer
* - If Thermal shapes are wanted, add non filled area, in order to create these thermal shapes
* 4 - calculates the polygon A - B
* 5 - put resulting list of polygons (filled areas) in m_FilledPolysList
* This zone contains pads with the same net.
* 6 - Remove insulated copper islands
* 7 - If Thermal shapes are wanted, remove unconnected stubs in thermal shapes:
* creates a buffer of polygons corresponding to stubs to remove
* sub them to the filled areas.
* Remove new insulated copper islands
*/
void ZONE_CONTAINER::AddClearanceAreasPolygonsToPolysList_NG( BOARD* aPcb )
{
int segsPerCircle;
double correctionFactor;
int outline_half_thickness = m_ZoneMinThickness / 2;
std::auto_ptr<SHAPE_FILE_IO> dumper( new SHAPE_FILE_IO(
g_DumpZonesWhenFilling ? "zones_dump.txt" : "", SHAPE_FILE_IO::IOM_APPEND ) );
// Set the number of segments in arc approximations
if( m_ArcToSegmentsCount == ARC_APPROX_SEGMENTS_COUNT_HIGHT_DEF )
segsPerCircle = ARC_APPROX_SEGMENTS_COUNT_HIGHT_DEF;
else
segsPerCircle = ARC_APPROX_SEGMENTS_COUNT_LOW_DEF;
/* calculates the coeff to compensate radius reduction of holes clearance
* due to the segment approx.
* For a circle the min radius is radius * cos( 2PI / s_CircleToSegmentsCount / 2)
* s_Correction is 1 /cos( PI/s_CircleToSegmentsCount )
*/
correctionFactor = 1.0 / cos( M_PI / (double) segsPerCircle );
CPOLYGONS_LIST tmp;
if(g_DumpZonesWhenFilling)
dumper->BeginGroup("clipper-zone");
SHAPE_POLY_SET solidAreas = ConvertPolyListToPolySet( m_smoothedPoly->m_CornersList );
solidAreas.Inflate( -outline_half_thickness, segsPerCircle );
solidAreas.Simplify( POLY_CALC_MODE );
SHAPE_POLY_SET holes;
if(g_DumpZonesWhenFilling)
dumper->Write( &solidAreas, "solid-areas" );
tmp.RemoveAllContours();
buildFeatureHoleList( aPcb, holes );
if(g_DumpZonesWhenFilling)
dumper->Write( &holes, "feature-holes" );
holes.Simplify( POLY_CALC_MODE );
if (g_DumpZonesWhenFilling)
dumper->Write( &holes, "feature-holes-postsimplify" );
solidAreas.BooleanSubtract( holes, POLY_CALC_MODE );
if (g_DumpZonesWhenFilling)
dumper->Write( &solidAreas, "solid-areas-minus-holes" );
SHAPE_POLY_SET fractured = solidAreas;
fractured.Fracture( POLY_CALC_MODE );
if (g_DumpZonesWhenFilling)
dumper->Write( &fractured, "fractured" );
m_FilledPolysList = fractured;
// Remove insulated islands:
if( GetNetCode() > 0 )
TestForCopperIslandAndRemoveInsulatedIslands( aPcb );
SHAPE_POLY_SET thermalHoles;
// Test thermal stubs connections and add polygons to remove unconnected stubs.
// (this is a refinement for thermal relief shapes)
if( GetNetCode() > 0 )
BuildUnconnectedThermalStubsPolygonList( thermalHoles, aPcb, this,
correctionFactor, s_thermalRot );
// remove copper areas corresponding to not connected stubs
if( !thermalHoles.IsEmpty() )
{
thermalHoles.Simplify( POLY_CALC_MODE );
// Remove unconnected stubs
solidAreas.BooleanSubtract( thermalHoles, POLY_CALC_MODE );
if( g_DumpZonesWhenFilling )
dumper->Write( &thermalHoles, "thermal-holes" );
// put these areas in m_FilledPolysList
SHAPE_POLY_SET fractured = solidAreas;
fractured.Fracture( POLY_CALC_MODE );
if( g_DumpZonesWhenFilling )
dumper->Write ( &fractured, "fractured" );
m_FilledPolysList = fractured;
if( GetNetCode() > 0 )
TestForCopperIslandAndRemoveInsulatedIslands( aPcb );
}
if(g_DumpZonesWhenFilling)
dumper->EndGroup();
}
void ZONE_CONTAINER::AddClearanceAreasPolygonsToPolysList( BOARD* aPcb )
{
}
Reference in New Issue View Git Blame Copy Permalink