Replicating pcbnew new for arrayed sheets

Many circuit designs can have repeated structures. Sadly, pcbnew doesn’t have any features to make the placement and routing any more productive.
Here is a demo of a script I wrote to help:

If you have X copies of the same sheet in eeschema, the script will allow you to place and route one of them and them apply that to the other sheets.

How’s it work?

If you call GetPath() on the modules in your design, you’ll get values like these (note the the path is only the /number/number part):

mod Q1 path /587DA765/58758821
mod Q2 path /5875D13C/58758821
mod Q3 path /5875D13D/58758821
mod Q4 path /5875D13E/58758821
mod R1 path /587DA765/5875882F
mod R2 path /587DA765/5875883D
mod R3 path /5875D13C/5875882F
mod R4 path /5875D13C/5875883D

The first number tells you which sheet instance the module belongs to. The second is an identifier for the module. So from the information above we can tell that these are all in the same sheet:

mod Q1 path /587DA765/58758821
mod R1 path /587DA765/5875882F
mod R2 path /587DA765/5875883D

Similarly, we know that these are the same transistor, just in different instances of the sheet:

mod Q1 path /587DA765/58758821
mod Q2 path /5875D13C/58758821
mod Q3 path /5875D13D/58758821
mod Q4 path /5875D13E/58758821

So if I have placed and routed sheet 587DA765, the script just needs to find all of the members of 5875D13C and simply adjust their positions by some constant increment.…

Querying pcbnew to generate a basic svg file

In a previous post, I gave some basic query capabilies in pcbnew. In this post, I’ll use that to generate a simple svg file.
The result looks like this:

Not the most interesting layout and a bunch of detail is missing, but I was happy to get this far. The code is hopefully self-explanatory. After the last post, I don’t really know what I can add.
The code can be found in my github


I need to get each of pcbnew’s layer colors. Some of the color names are modified to match svr colors. The real answer is to get the rgb values from colorrefs, but those aren’t exposed in python today
Edit Nov 15, 2017 RGB values are now available in the form of the COLOR4D structure.
colors = board.Colors()
c4 = colors.GetLayerColor(track.GetLayer())
r = int(round(c4.r*255)
g = int(round(c4.g*255)),
b = int(round(c4.b*255))
The colornames map below won’t work anymore.
End edit

colornames = {
 pcbnew.BLACK: 'BLACK',
 pcbnew.WHITE: 'WHITE',
 pcbnew.BLUE: 'BLUE',
 pcbnew.GREEN: 'GREEN',
 pcbnew.CYAN: 'CYAN',
 pcbnew.RED: 'RED',
 pcbnew.BROWN: 'BROWN',

modifying pcbnew layout from python

I my previous post, I talked about querying for information about your layout. In this one I’ll show you how to create your own wires/vias from python. I also cover moving modules. Most of the code is self-explanatory but I find it helpful to have sample “cookbook” code.
The main thing to keep in mind when creating new objects is that even though you have to pass a board pointer to the constructors, you still have to call board.Add(obj). Also, you have to add it before setting the net. If you try to set the net before, it’ll do nothing.
Remember that the units are 1E-6mm. So if you have a mm value multiply it by a million.


First, let’s generate our layer mapping

layertable = {}
numlayers = pcbnew.LAYER_ID_COUNT
for i in range(numlayers):
 layertable[i] = board.GetLayerName(i)
 print("{} {}".format(i, board.GetLayerName(i)))

Add a track

track = pcbnew.TRACK(board)
track.SetStart(pcbnew.wxPoint(136144000, 95504000))
track.SetEnd(pcbnew.wxPoint(176144000, 95504000))

Add a via

In this case, I’m going to copy an existing via. Note that there is also the clone method, but doing it this way you’ll know how to generate a via from scratch.
There isn’t yet a direct way to query a via for its layers.…

The basics of scripting in pcbnew

I’ve found that, so far, I’m able to do all of the layout queries and manipulations I’ve wanted to do.
Edit April 3, 2018 The comment below about 4.0.5 is not true. Even the most recent 4.0.7 is missing a ton of python related stuff. Until kicad 5.0 comes out, I recommend using one of the nightly builds from the kicad downloads page. End Edit
Note that these examples don’t work on the latest release as of Feb 2017 (4.0.5). You want one of the nightly builds, also in the kicad download area. Or you can build it
The interface is lacking some consistency but it’s fine if you have a map of the classes (click for a larger version or download it from here):

In this post, I’ll focus on querying a board for information about it’s contents. The code can be found in this github repo.

Getting started

To invoke any of these examples, you’ll want pcbnew’s scripting window. Tools->scripting console
You’ll probably want these in your scripts

import pcbnew
# most queries start with a board
board = pcbnew.GetBoard()


Want to know all of the nets in your board?
Nets can be looked up in two ways:

  • by name
  • by netcode – a unique integer identifier for your net.