Python - iterate through selected parts (replicate layout)

Layout
1

How to use Python script / console to iterate through selected footprint elements on Pcbnew? Is it possible?

I just started with:

import pcbnew

board_handle = pcbnew.LoadBoard('foo.kicad_pcb')
board = board_handle.GetBoard()

board.GetFoorprint
board.GetFoorprints
2

Foorprint?
Did you copy & paste that Python snippet?

[Edit] Foo R print.
(I don’t know much about scripting in KiCad, so can’t help there.)

3

My intention is copy a part of a layout, rename some REF and update the link with Eeschema (F8).

Something less automatic than https://github.com/MitjaNemec/Kicad_action_plugins/issues/102, that I could not complete fix it.

4

You don’t say what version of KiCad you are using.

def SetText(Filename = None):
    if Filename: 
        my_board = pcbnew.LoadBoard (Filename)
    else:
        my_board = pcbnew.GetBoard()

    for module in my_board.GetModules():
        print ("module ref %s %s" % ( module.GetReference(), my_board.GetLayerName(module.Reference().GetLayer())))

        # set layer
        module.Value().SetLayer (pcbnew.F_Fab)

This used to work, but the Great Renaming Event of 2020 may have scuppered it.

5 
board = pcbnew.GetBoard()
for fp in board.Footprints():
  if fp.IsSelected():
    # do the deed
    pass

That is for nightly. For 5.1 do board.GetModules()

1 Like
6

I got. Yes, @qu1ck I just wrote the same code here. Thanks!

7

For future references, my final algorithm (I just realized that have to for change the tracks net also, before re-sync):

import pcbnew
import re

#board = pcbnew.LoadBoard(file_name)
board = pcbnew.GetBoard()

# Number used to offset the reference number to macth with news hierarchical block.
offset_ref = -800

for f in board.GetFootprints():
	if f.IsSelected():
		old_ref =  f.GetReference()
		ref_parts = re.findall(r'([A-Z]+)([0-9]+)', old_ref)[0]
		new_ref = ref_parts[0] + str( int(ref_parts[1]) + offset_ref )
		f.SetReference(new_ref)
		print('Changed ref: "%s" -> "%s"' % (old_ref, new_ref))

for t in board.GetTracks():
	if t.IsSelected():
		old_net = t.GetNetname()
		net_parts = re.findall(r'Net\-\(([A-Z]+)([0-9]+)\-Pad[0-9]+\)', old_net)
		if net_parts:#Net-(R1606-Pad1)
			print(ref_parts)
			net_parts = net_parts[0]
			new_net = net_parts[0] + str( int(net_parts[1]) + offset_ref )
			new_net = old_net.replace(''.join(net_parts), new_net)
			t.SetNet(new_net)
			print('Changed net: "%s" -> "%s"' % (old_net, new_net))

Just missing fix the t.SetNet(new_net) method use. Some ideas?

8

No idea what new_ref is supposed to be but if you meant new_net then it will not work because SetNet() takes a NETINFO_ITEM object, not a string
image

9

Right @qu1ck about the variable (just a mistake here). I update the code above.

I am right now trying to understand how to get the NETINFO_ITEM from my intended net name.

I could not fix the above mentioned (link) Pcbnew python plugin (my first intention). There was some wx issues that I could make.

10

The way you generate net name is not the right approach. Net names are not deterministic in kicad, they may change when you add/remove components to the net.
You can get list of nets from pcb by doing board.GetNetsByName() which returns a map that you can index like a dictionary or iterate over using items() method.
Now to find which net you need depends on what you are trying to achieve maybe looking at pads and their GetNet() and GetNetname() will help.

11

Thanks @qu1ck. At the end, the “net rename” wasn’t need. Only the references change and re-sync by reference was enough.

My mistake was just some difference in the Nightly behavior that allow me different unit sequence on OA at hierarchical pages.

12

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.