devbisme
can ‘Disconnect airwires from pads’ also act as a split-net command
Request: can ‘Disconnect airwires from pads’ also act as a split-net command, where someone selects N segments of a NET, but not the whole net. Usually one split keeps the old net name, and a new net name is assigned to now isolated connection set. PADS and Vias touched would have that new net name applied.
One use case, is in manual duplicate of a cell array, where currently that slavish clones all net names where exact clones may not be desired. Being able to split some routed nets, after clone, would be useful. eg keep GND +3V, but make some local by removing the rats-connection due to same-net-name.
Code example below collects selected TRACK items, and then collects PADS of that Netname, and tests for PADs touching selected segments. End outcome is a selected set (trk/via/PAD), ready for NET split rename.
Other issue - I've raised a BUG report in KiCad PCB as to work best, this will need a fix made to Select Copper Connection. https://bugs.launchpad.net/kicad/+bug/1789807
Currently, KiCad menu Select Copper Connection 'travels over' & selects vias in the sub-group, and can travel-over a PAD but fails if entry/exit traces are on different layers. My thinking here, is Select Copper Connection should work like a multimeter, and via is the same as a pad.
I did find a workaround, which is to manually Shft-Clk select one segment in each PAD fragmented sub-net, and then 'I' will collect all the Select Copper Connections. A little klunky and error prone.
# PcbNew_Select_Track_Pad.py Derived from PcbNew_Export_PcbNew_NET
# eg Usage - in KiCad PcbNew Python Console paste after >>>
# >>> execfile("C:\KiCad_Python\Check_Footprint_Attr\PcbNew_Select_Track_Pad.py")
#
# Purposes :
# Select.CopperConnection picks Vias and Tracks, but does not pick PADS.
# It also has a BUG in that it fails IF a layerchange occurs at the pad.
# Workaround: Shift-clk any ONE segment in each pad-fractured subset, and then 'I' will select all copper connects
#
# This simple script collects sets of selectd traces, and same-net pads, and then cross checks those sets, for selected-trace-end at pad
#
# V1.0 first pass
# V1.01 added pad radius to tolerate slight alignment errors
import pcbnew # ok on fresh start
pcb = pcbnew.GetBoard() # Works on Loaded Design file
print '# PcbNew_Select_Track_Pad.py V1.01 start'
SetCount = 0
tPadCount = 0
sPadCount = 0
trks = pcb.GetTracks() # Via is a case of track
trkcnt = trks.GetCount()
SelTrackSet = [] # clear set
PossiblePadSet = [] # clear set
AddSelectPadSet = [] # clear set
print '# Found %s Total Track Segments '%(trkcnt)
TagNetName = '?????' # some default
for ftrk in trks:
if ftrk.IsSelected():
TagNetName = ftrk.GetNetname() # get name
SelTrackSet.append(ftrk) # Collect a list of selected tracks - this includes Vias
SetCount = SetCount + 1
print '# Tag Net name is: %s , Selected Segments & Vias : %s '%(TagNetName, SetCount)
pads = pcb.GetPads()
for pad in pads:
pad.ClearSelected() # debug, clear last pass selects
if pad.GetNetname() == TagNetName:
tPadCount = tPadCount + 1
PossiblePadSet.append(pad) # Collect a list of SAME NET pads in the design
print '# PossiblePadSet count : %s '%(tPadCount)
for strk in SelTrackSet: # Now scan for PAD XY on selected trace end. This does not catch fly-over traces, or not-snapped trace ends
if strk.GetClass() != "VIA": # skip vias
sS = strk.GetStart()
sE = strk.GetEnd()
for spad in PossiblePadSet:
if not spad.IsSelected(): # Skip if already have earlier track end causing select
sP = spad.GetPosition()
mR = min(spad.GetSize()) / 2 # get min radii (rough) - tolerates allows small errors in trace ends.
if ((abs(sS.x-sP.x) < mR) and (abs(sS.y-sP.y) < mR)) or ((abs(sE.x-sP.x) < mR) and (abs(sE.y-sP.y) < mR)): # test trace END inside PAD O
spad.SetSelected() # show and tag as done
sPadCount = sPadCount + 1
AddSelectPadSet.append(spad) # collect these added pads
print '# Copper Connect & Selected Pads count : %s '%(sPadCount)
for spad in AddSelectPadSet: # list those selected
PinName = spad.GetPadName()
PadSize = min(spad.GetSize())
Module = spad.GetParent()
RefDes = Module.GetReference()
Module.SetSelected() # TEST PART - for move checks
print '# Ref %s Pin %s Size %s' %(RefDes,PinName,pcbnew.ToMM(PadSize)) # show list
# if Module.IsSelected():
# Module.Move(pcbnew.wxPoint(pcbnew.FromMM(-0.25),pcbnew.FromMM(-0.35))) #debug, walk selects away from ideal centre
pcbnew.Refresh()
# Null run gives expected
# PcbNew_Select_Track_Pad.py start
# Found 1169 Total Track Segments
# Tag Net name is: ??? , Selected Segments: 0
# PossiblePadSet count : 0
# Copper Connect found Pads count : 0
# PcbNew_Select_Track_Pad.py V1.01 start
# Found 1169 Total Track Segments
# Tag Net name is: GND , Selected Segments & Vias : 29
# PossiblePadSet count : 39
# Copper Connect & Selected Pads count : 9
# Ref U2 Pin 5 Size 1.6
# Ref J11 Pin 1 Size 2.5
# Ref J12 Pin 1 Size 2.5
# Ref J13 Pin 1 Size 2.5
# Ref MIDI_OUT1 Pin 3 Size 1.7
# Ref J14 Pin 1 Size 2.5
# Ref J15 Pin 1 Size 2.5
# Ref J16 Pin 1 Size 2.5
# Ref J4 Pin 2 Size 1.7
# Workaround test : Shift-clk ONE segment in each pad-fractured subset, and then 'I' will select all copper connects
# PcbNew_Select_Track_Pad.py V1.01 start
# Found 1176 Total Track Segments
# Tag Net name is: GND , Selected Segments & Vias : 79
# PossiblePadSet count : 39
# Copper Connect & Selected Pads count : 21
# Ref EXT_FSW_IN1 Pin S Size 2.0
# Ref EXPR_SW_IN1 Pin S Size 2.0
# Ref EXPR_PEDAL_IN1 Pin S Size 2.0
# Ref J9 Pin 1 Size 2.5
# Ref J10 Pin 1 Size 2.5
# Ref U1 Pin 4 Size 1.6
# Ref R10 Pin 2 Size 1.6
# Ref J8 Pin 1 Size 2.5
# Ref J7 Pin 1 Size 2.5
# Ref R6 Pin 1 Size 1.6
# Ref U2 Pin 5 Size 1.6
# Ref J11 Pin 1 Size 2.5
# Ref J12 Pin 1 Size 2.5
# Ref J13 Pin 1 Size 2.5
# Ref MIDI_OUT1 Pin 3 Size 1.7
# Ref J14 Pin 1 Size 2.5
# Ref J15 Pin 1 Size 2.5
# Ref J16 Pin 1 Size 2.5
# Ref J4 Pin 2 Size 1.7
# Ref MIDI_IN1 Pin 3 Size 1.7
# Ref J17 Pin 1 Size 2.5
`
This rough code works around the Select Copper Connection issue, which is awaiting a fix. It can get slow on large datasets, as it sweeps 2 axes, multiple times.
# Select Copper Connection fails to follow-over PADS where LAYER changes, so add a fix to walk along the nets
for ftrk in trks:
if TagNetName == ftrk.GetNetname():
NetTrackSet.append(ftrk) # Collect a list of ALL nets tracks - this includes Vias
NetCount = NetCount + 1
print '# Net name : %s , Possible Seg/Via : %s '%(TagNetName, NetCount)
LastPass = -1
TstCount = 0
while NewCount != LastPass: # repeat until no more found, ie NewCounts stops increasing
LastPass = NewCount
for ntrk in NetTrackSet: # some selected, some not..
if ntrk.IsSelected(): # seed tree expansion by Selected flag
sS = ntrk.GetStart() # Get this selected Start,End co-ordinates
sE = ntrk.GetEnd()
for mtrk in NetTrackSet: # Scan all other nodes
TstCount = TstCount + 1 # this number can eget large very quickly eg Net name : GND , Possible Seg/Via : 144 Track Segs Added 30 tests 48384
if not mtrk.IsSelected(): # Skip if selected already
mS = mtrk.GetStart()
mE = mtrk.GetEnd()
if (mS == sS) or (mS == sE) or (mE == sS) or (mE == sE) :
NewCount = NewCount + 1
mtrk.SetSelected() # join new touch
print '#Track Segs Added %s tests %s '%(NewCount,TstCount)
.. and the good news, is the bug reported https://bugs.launchpad.net/kicad/+bug/1789807 where Select Copper Connection failed to 'follow over' a pad where layer changed, is now fixed.
Fixed in revision 9eec296b0a0d9e9ff6a152aa1ef91d7ae92920dc https://git.launchpad.net/kicad/patch/?id=9eec296b0a0d9e9ff6a152aa1ef91d7ae92920dc Changed in kicad: status: Triaged → Fix Committed assignee: nobody → Seth Hillbrand (sethh)
So that last slower code is not strictly needed, unless you want to allow any single segment select, to be enough to seed the selection ? (or want it to work on older KiCads )
With a properly working Select Copper Connection, that code should exit with nothing to do, after 1 x 2 axis pass.