~/cmos $ CMOS Foundry_

kicad-druid: Fab House Design Rules, Generated and Tested

Simon Maddison / October 2026 (546 Words, 4 Minutes)

kicad kicad-dru design-rules drc jlcpcb pcbway ci-cd pcb

View on GitHub

Table of contents

Overview

kicad-druid is a set of KiCad custom design rules (.kicad_dru) that match what JLCPCB and PCBWay can actually make. Drop the file for your order into your project and KiCad’s DRC flags anything the fab would bounce, on your screen instead of in their review queue.

It replaces my earlier KiCad Custom Design Rules repo, which is now in the archive. Same idea, rebuilt properly: the rules are generated rather than hand-edited, every variant is checked by KiCad in CI, and there is a new set of rules that works for either fab. MIT-licensed, works on KiCad 8, 9 and 10.

What changed from the old rules

  Old repo kicad-druid
Rule files hand-edited generated
Variants comment blocks one file per build
Fabs JLCPCB, PCBWay + Generic (both)
CI lint lint + full DRC
Silent failures possible sentinel rule

One source of truth per fab

Each fab’s published capabilities live in one TOML file (capabilities/JLCPCB.toml, capabilities/PCBWay.toml). A small Python script generates every .kicad_dru from it, plus a side-by-side comparison table of the two fabs. CI regenerates the files and fails if anyone hand-edits the output, so the rules can’t drift away from the capability table they came from.

That also killed the old “uncomment the right block for your layer count” step, which was the easiest way to get these files wrong. You now pick the whole file that matches what you’re ordering:

File Layers Copper
<FAB>.kicad_dru 4 (default) 1 oz
<FAB>-2L-1oz.kicad_dru 1–2 1 oz
<FAB>-4L-2oz.kicad_dru 4 2 oz
<FAB>-6L-1oz.kicad_dru 6 1 oz

PCBWay files also ship impedance net classes (50 Ω single-ended, 60–120 Ω differential) as starting points for the fab’s default stackup.

Generic: design before you pick a fab

Plenty of boards get designed before anyone has decided where they’ll be built. The Generic/ rules take the stricter of the two fabs for every limit: the larger minimum, the smaller maximum, and any rule either fab needs. A board that passes Generic passes at both. Once the fab is settled, switch to that fab’s file and the limits relax. Generic is derived in code from the two fab files, so it follows any capability update automatically.

The green DRC that checked nothing

This is the part I’m happiest with. If KiCad can’t compile a rules file (one typo, one unknown layer name), it drops the rules, and kicad-cli pcb drc reports a clean run with exit code 0. No warning, empty stderr. Your CI goes green while not a single custom rule ran.

kicad-druid’s CI guards against that. It runs KiCad’s DRC on a paired test board for every one of the twelve rule files, and before each run it appends a sentinel rule that must always fire. If the sentinel isn’t in the report, the file didn’t compile, and the job fails. It goes at the end of the file because some errors drop only the rule they’re in and everything after it, while others drop the whole file. Either way, the sentinel goes missing.

The linter also catches the quieter mistakes: lowercase item types like 'track' that KiCad silently never matches, and layer display names like F.Silkscreen that stop resolving the moment a board is imported from Altium or renamed.

Using it

  1. Copy the .kicad_dru matching your order from JLCPCB/, PCBWay/ or Generic/ into your project folder.
  2. Rename it to match the project: your-project.kicad_dru.
  3. Run DRC (F8). Check Board Setup > Design Rules > Custom Rules once for errors, since KiCad won’t tell you otherwise.

Releases and the full rule comparison are on GitHub. It started as a fork of labtroll/KiCad-DesignRules by Morten Hattesen, with that history kept.

-SM

Related