fix more layers

1 files changed, 0 insertions, 114 deletions

diff --git a/fix-layer-4.py b/fix-layer-4.py
deleted file mode 100755
index 78f851c..0000000
--- a/fix-layer-4.py
+++ /dev/null
@@ -1,114 +0,0 @@
-#!/usr/bin/python
-"""
-
-Layer 4 is a layer with large polygons (GND and Power). In Altium, this was made
-like an inverted layer with drawn lines separating polygons. Issues were with
-line thickness in Kicad, clearance parameters preventing copper to flow in between
-pins under the FPGA and the fact that KiCAD doesn't do inverted layers so the
-lines had to be removed and zone clearances adjusted to create the same result.
-
-Compare with
-
-  $ gerbv 'rev03-KiCad/GerberOutput/Cryptech Alpha-In4.Cu.gbr' /path/to/CrypTech.GP3
-
-"""
-
-import sys
-import pcbnew
-
-
-def remove_tracks(board, layer):
-    """
-    The tracks on Layer four are actually where there *should not* be copper.
-    L4 is an inverted layer, but that information actually isn't in the files -
-    it is specified in an excel sheet sent to the PCB house.
-
-    By removing them and then setting some parameters carefully on the zones
-    on that layer, we get a close-to-perfect (but no longer inverted) result
-    in KiCAD.
-    """
-    for this in [x for x in board.GetTracks() if x.GetLayerName() == layer]:
-        print('Removing track {}'.format(this))
-        board.Delete(this)
-
-#def set_tracks_width(board, layer, width):
-#    for this in [x for x in board.GetTracks() if x.GetLayerName() == layer]:
-#        this.SetWidth(width)
-#
-#def move_tracks(board, from_layer, to_layer):
-#    for this in [x for x in board.GetTracks() if x.GetLayerName() == from_layer]:
-#        this.SetLayer(board.GetLayerID(to_layer))
-
-
-def layer_zone_fixes(board, layer):
-    for i in range(board.GetAreaCount()):
-        area = board.GetArea(i)
-        if area.GetLayerName() != layer:
-            continue
-        print('Area {} {}'.format(area, area.GetNetname()))
-        # This makes sharp edges matching Altium Designer
-        # 0.0255 is the minimum KiCad wants in order to allow changes to the zone inside KiCad
-        area.SetMinThickness(int(2 * 0.0255 * 1000000))
-        # 0.25 works better for the distance between zones in the bottom half of layer 4,
-        # but does not allow copper between the vias under the FPGA
-        #area.SetZoneClearance(int(0.25 * 1000000))
-        #
-        # Values below 0.15 or somewhere there does not seem to make a difference at all
-        area.SetZoneClearance(int(0.15 * 1000000))
-        if area.GetNetname() == 'GND':
-            area.SetPriority(50)
-            # 0.25 clearance on the 'background' GND zone keeps the distance to the island
-            # zones in the bottom half of layer 4, matching the clearance between the areas
-            # but creating a bit more clearance around vias in KiCAD plot than in Altium
-            area.SetZoneClearance(int(0.25 * 1000000))
-            area.SetThermalReliefCopperBridge(int(0.5 * 1000000))
-            #help(area)
-
-
-def hide_layers_except(board, layers):
-    """
-    As a convenience when working on getting a particular layer right, hide other layers.
-    """
-    lset = board.GetVisibleLayers()
-    print('Layer set: {} / {}'.format(lset, lset.FmtHex()))
-    #help(lset)
-    mask = 0
-    for x in lset.Seq():
-        name = board.GetLayerName(x)
-        print('  {} {}'.format(x, name))
-        if name in layers:
-            mask |= 1 << x
-    hexset = '{0:013x}'.format(mask)
-    visible_set = pcbnew.LSET()
-    visible_set.ParseHex(hexset, len(hexset))
-    board.SetVisibleLayers(visible_set)
-
-
-def main(in_fn='rev03-KiCad/convert.kicad_pcb', out_fn='rev03-KiCad/Cryptech Alpha.kicad_pcb'):
-    board = pcbnew.LoadBoard(in_fn)
-    pcbnew.SaveBoard(in_fn + '.before-fix-layer-4', board)
-
-    remove_tracks(board, 'In4.Cu')
-    #set_tracks_width(board, 'In4.Cu', int(0.15 * 1000000))
-    #move_tracks(board, 'In4.Cu', 'Eco2.User')
-    layer_zone_fixes(board, 'In4.Cu')
-
-    hide_layers_except(board, ['In4.Cu'])
-
-    # Only show Through Via while working on Layer 4
-    board.SetVisibleElements(0x7FFC0009)
-
-    pcbnew.SaveBoard(out_fn, board)
-    return True
-
-if __name__ == '__main__':
-    try:
-        if len(sys.argv) != 3:
-            sys.stderr.write('Syntax: fix-layer-4.py infile.kicad_pcb outfile.kicad_pcb\n')
-            sys.exit(1)
-        res = main(sys.argv[1], sys.argv[2])
-        if res:
-            sys.exit(0)
-        sys.exit(1)
-    except KeyboardInterrupt:
-        pass