Project Logs

Collapse

• Comparison to FreeRouting

  haas • 02/04/2026 at 02:13 • 1 comment

  FreeRouting is another KiCad plugin that can do auto-routing. It's not bad, just more limited in scope, slower, and less integrated into KiCad. It has been around for a while though so is solid and reliable. 

  For simple boards, there's not much difference in what it would do vs. this project, except KiCadRoutingTools gives you more control over track widths, power nets, ground/power planes, etc. 

  This is a relatively simple board routed with KiCadRoutingTools:

  And here is FreeRouting on the same board:

  
  But for a more complicated board the differences are more apparent. Here again is the board I posted about recently, with bus routing enabled in KiCadRoutingTools:

  And here is FreeRouting on the same board:

  FreeRouting actually failed to route 4 of the nets here. And it took it ~10 minutes. KiCadRoutingTools took ~1 minute and routed all tracks.

  KiCadRoutingTools gives tracks that are far more natural and organized than the Manhattan-style FreeRouting algorithm.

• Smarter and prettier routes

  haas • 02/02/2026 at 23:32 • 0 comments

  Auto-routers are known for producing ugly tracks. I'm working hard to teach this one how to be smarter and prettier. And it's not just esthetics. It can now route dense boards most auto-routers would choke on!
  
  I've recently added some features that we humans rely on:
  - Preferred direction by layer
  - River routing, with nearby tracks being encouraged to follow a neighboring track on the same layer
  - Rip-up memory: if you needed to rip up a track to route in a new track, try not to block where the old track was, since it is likely going to have to pass through there again when it's re-routed

• A KiCad Plugin GUI

  haas • 01/26/2026 at 20:33 • 0 comments

  I was impressed how easy it was to make a GUI wrapper for the python/rust backend - here it is. 

  There's a tab for basic single-ended routing, an advanced tab with fancier features, another for differential pair routing, one for bga/qfn fanout, one for GND/power plane, and a place to see the logs from each command. 

  Nets can be selected based on component or name, and be filtered in various ways.

  There's a progress bar, close/cancel button, etc.

  All the results are immediately put onto the live kicad pcb board, and can be undo/redo'ed before saving.

  Plus there's a cool icon that gets put on your KiCad toolbar...

• Using AI to figure out power nets

  haas • 01/21/2026 at 19:54 • 0 comments

  Some nets on a PCB will need to be wider because they need to carry more power. We can easily feed in these per-net widths (in mm) like this:

  python route.py input.kicad_pcb output.kicad_pcb --nets "Net*" \
    --power-nets "*GND*" "*VCC*" "+3.3V" \
    --power-nets-widths 1.0 0.5 0.35

  But going through a whole board and figuring out which nets need to carry what amount of current/power and then listing them is tedious, and error-prone. Automating the discovery and categorization is challenging though, because there are so many types of components and situations that arise. For instance, a regulator may output through a fuse, an inductor or ferrite bead, a current shunt resistor, and then eventually get to an IC. Along the way there are various decoupling caps, resistors branching off going to an LED, etc. A script would have a hard time figuring out what nets in this web need to carry large currents. First of all, it would need to understand what each component is and does, more or less. What are the typical currents needed by that kind of IC? How much is used in that LED? 

  An experienced human, even if they're not the original designer, can go through and figure it out pretty well. They know what each component is, and if not they can look it up based on the part number and check the datasheet. And they understand how current flows through a branching circuit like this and what nets will need the larger widths. But again, it's tedious, and transcribing that into a list of net names and widths is error-prone.

  Fortunately, it turns out AI is already very capable of analyzing such a board and doing this job of understanding power flow pretty well! Here's an example of how it works and what it looks like in practice. More details here.

  First, start up a claude code session. Next, we point the provided claude skill at the kicad pcb file: /analyze-power-nets input.kicad_pcb, and it goes to work. First it extracts info from the kicad pcb file about what components are on the board and how they're connected (not routed, but what airwire nets "conenct" what), using a python script. It categorizes all the easy components like resistors, caps, inductors, etc. and then searches the Web for info about each non-trivial component. This all takes about ~15 seconds, since components are researched in parallel. 

  Next, it forms an understanding of what the board is trying to do! Here's it's correctly identified that this is a PIC programmer. It then traces the power flow through the components on the board, and estimates the power/current and voltages in important nets, based on info it learned reading the datasheets. 

  It then reports what it has discovered and surmised, and determines the width of each trace needed based on power requirements and IPC-2152 guidelines. It finally outputs a command in the correct format to be used by the --power-nets --power-nets-widths commands.

  In the end it took just ~20k tokens to do all that for this (simple) board. The result after routing with the --power-nets --power-nets-widths commands given looks pretty reasonable!

View all 4 project logs