Special Strings or Text on PCB

Layout
7

Here is a quick example. I’ve got symbols in the schematic I use for things like PCB logos (these have no pins).

782×468 3.29 KB

I can attach these to different footprints to select where the data goes. In this case the footprints are trivial, they have no graphic items, I’m just using the value. I cheated with the “text on copper” footprint, I had to edit that in a text editor, KiCad deprecates putting text on copper.

The PCB initially looks like this after netlist import:

883×434 2.54 KB

The designators are hidden and don’t appear on PCB, just shown here for reference. Running the script

>>> execfile “test.py”
Setting module M3 Value to 2017-08-08

795×448 2.5 KB

and the script

import sys
from datetime import datetime
import pcbnew

def testfunc():
  my_board = pcbnew.GetBoard()
  for module in my_board.GetModules():
    fpid = module.GetFPID()
    if fpid.GetFootprintName() == "text_auto_date":
      new_text = "{:%Y-%m-%d}".format(datetime.now())
      print ("Setting module %s Value to %s " % ( module.GetReference(), new_text ) )
      module.Value().SetText(new_text)
      
testfunc()

I can’t see how to get to the sch file from the board object, is there another way?
board.GetFileName() should do it…

5 Likes