Advanced Usage

The goal of circuitpainter is to make the most common parts of PCB generation easy, and you might want to do things that this API doesn’t directly support.

Note that the underlying pcbnew API is not finished, and will likely be different between even minor KiCad versions. Using the python help() function on these object references is a good way to explore their options, though it gets complicated because they are themselves thin wrappers over the C-language pcbnew library. Eventually, you’ll need to dig through the KiCad source to figure out how things are supposed to work, and don’t forget to check the bug tracker if things aren’t working correctly, because it probably is a bug and there might be a workaround / fix.

Extended object properties

Circuit painter aims to keep circuit creation simple, but there are extra configuration settings on many objects that you might want access to. To facilitate this, all functions that create a PCB object will also return a reference to that object, so that you can modify it.

For example, create a rectangular zone, and save the reference to it:

p = CircuitPainter()
p.layer("F_Cu")
zone = p.rect_zone(0,0,10,10)

Then, modify the zone properties using the pcbnew api:

zone.SetIsRuleArea(True)
zone.SetDoNotAllowCopperPour(True)
zone.SetDoNotAllowVias(False)
zone.SetDoNotAllowTracks(False)
zone.SetDoNotAllowPads(False)

Board configuration

Many of the board configuration options (stackup, DRC rules, etc) are stored in the board design settings. For example, to create a 4-layer board with some different DRC settings:

import pcbnew
settings = p.pcb.GetDesignSettings()
settings.SetCopperLayerCount(4) # Change to a 4-layer board design
settings.m_CopperEdgeClearance = pcbnew.FromMM(0.1) # Set the copper-to-edge spacing to 0.1mm

Note that we are importing ‘pcbnew’ here, in order to use the FromMM() function to convert a measurement from mm to KiCad’s internal units.

Updating boards / adding manual edits

Circuit Painter is great for automating parts of designs that are highly repetitive, but is less effective for more mundane tasks such as wiring up a fancy LED array to a microcontroller. On this end, everything that CircuitPainter creates is placed into a single group. When you make manual additions to the board, be sure not to put your changes into the auto-generated group. Later, if you want to re-generate the automated portion of your design, you should be able to just delete that group, then start Circuit Painter by passing it the file name:

p = CircuitPainter('my_file.kicad_pcb')

New objects will then be added to that board, in a new group.