

Mcu board
KiCad diff view tool
- Size
- 80 × 50 mm
- Copper layers
- 2
- Thickness
- 1.6 mm
- Parts
- 15
- Nets
- 9
- Pads
- 40
- Tracks, vias
- 54, 8
- Pours
- 1
- Routed
- Yes
- KiCad
- KiCad 10.0 (file 20260206)
- Created
- 10 May 2026
- Updated
- 5 Nov 2026
Overview
Mcu board is an open-source printed circuit board by sksat, from the sksat/kicadiff repository on GitHub, published under the MIT licence. It is a 2-layer board of 80 × 50 mm with 15 parts on 9 nets, routed with 54 tracks and 8 vias.
It is built around the AMS1117-3.3. Its parts include 3 capacitors, 2 resistors, 2 ICs, 2 connectors and 1 diode. It belongs with the microcontroller boards boards of this library.
Main components
1README
README.mdkicadiff
Visual diff tool for KiCad projects — see what changed between two
states of a .kicad_pcb / .kicad_sch / .kicad_sym / .kicad_mod
file in your browser, or as a markdown report you can paste into a PR.

What you get
-
HTML viewer with side-by-side / overlay / swipe modes, layer toggles for PCBs, page navigation for hierarchical schematics, wheel-to-zoom and right-click-drag-to-pan, and an amber tab marker on files / pages whose rendered output actually changed.
-
Markdown report (
--md) with side-by-side image tables and a structural component diff (added / removed / changed by reference designator), plus — for PCBs — aNetssubsection that lists added / removed nets and pads that were rewired (R1.2: GND → /VCC). Pad transitions to or from the unconnected net are surfaced too (R7.1: (unconnected) → +3V3). Both legacy ((net id "name")) and KiCad 10 ((net "name"), no top-level net table) shapes are supported. Good for PR descriptions and commit messages. -
Text-only structural diff (
--text-only) — fast, no image rendering, prints to stdout. Includes the sameNetssubsection for PCBs so routing changes show up in CI logs and grep:text blink.kicad_pcb (pcb): +0 -0 ~1 =3 ~ R1 value: 330 → 470 Nets: +1 -0 ~2 + /LED_OUT ~ R1.2: GND → /LED_OUT ~ R7.1: (unconnected) → +3V3 -
DRC / ERC violation diff (
kicadiff check) — runs design-rule and electrical-rule checks on both sides and reports the delta as+N new / -M fixed / =K unchanged. Exits 1 when the target side introduces NEW violations (non-zero on operational failures too — missingkicad-cli, git errors, JSON parse errors), so it makes a good PR gate that fails on regressions while ignoring pre-existing findings.
Requirements
kicad-cli9.x or later (rendering engine).- Bun — runs the TypeScript CLI directly via shebang. Bun also compiles the standalone binary, so no separate Node install is needed for any workflow. Standalone binary users skip this.
The render pipeline (SVG → PNG, tri-colour pixel diff highlight) used to
need rsvg-convert and ImageMagick; both are now in-process
(@resvg/resvg-js for rasterisation, a small custom classifier on top
of pngjs for the diff overlay).
Install
Three ways depending on what's already on your machine:
# 1. One-shot via Bun's package runner (no install)
bunx kicadiff [args...]
# 2. Global install (puts `kicadiff` on PATH)
pnpm add -g kicadiff
# or with `bun add -g kicadiff` / `npm install -g kicadiff`
# 3. Standalone binary — single file, no Bun runtime needed.
# Drops `kicadiff` into ~/.local/bin (override with KICADIFF_INSTALL_DIR).
curl -fsSL https://raw.githubusercontent.com/sksat/kicadiff/main/install.sh | shkicad-cli (and rsvg-convert / magick) are not bundled — install KiCad 9+
first, then pick whichever kicadiff distribution form fits your workflow.
Usage
kicadiff works on the same positional argument shape as git diff,
plus a few subcommands when you want to scope to one file type.
# Project-level diff (cwd, both PCB and schematic, default = index vs working
# tree — same as `git diff`)
kicadiff
# Pass a project root, a .kicad_pro, or any single KiCad file
kicadiff path/to/project/
kicadiff project.kicad_pro
kicadiff project.kicad_pcb
# Staged changes only (same as `git diff --cached` / `git diff --staged`)
kicadiff --cached project/
kicadiff --staged project/ # alias
# Compare arbitrary refs
kicadiff HEAD path/to/project/ # working tree vs HEAD (includes staged)
kicadiff main path/to/project/ # working tree vs main
kicadiff v1.0 v2.0 board.kicad_pcb # v1.0 vs v2.0
kicadiff main..feat foo.kicad_pcb # range syntax
kicadiff main -- foo.kicad_pcb # explicit `--` separator
kicadiff :0 project/ # explicit index ref (alias: index / staged)
# Subcommands scope to one file type (skip sibling auto-detect)
kicadiff pcb foo.kicad_pcb
kicadiff sch foo.kicad_sch # alias: schematicOutput
By default kicadiff writes to <repo>/.claude/preview/ (next to the git
root) so the directory is easy to find from the project. Override with
--output-dir <dir> for the image directory, and --output <path> to
relocate the HTML / markdown file specifically (image paths in the
file get rewritten to be relative to it, so the file stays portable).
The HTML viewer is a single file with the manifest + image references inline; you can email it, host it as a static asset, or open it locally with VSCode's Live Preview extension.
Render cache
Every per-side render is content-addressed and cached under
$XDG_CACHE_HOME/kicadiff (or ~/.cache/kicadiff). Repeat runs
against unchanged content return in ~1 s vs ~5 s cold. Bypass with
--no-cache or override the location with KICADIFF_CACHE_DIR.
The cache grows monotonically — every kicad-cli version bump and every
content edit adds a new entry, and nothing is evicted automatically.
Inspect and reclaim space with the cache subcommand:
# Show cache directory, entry count, total size, and oldest / newest age
kicadiff cache stats
# Delete entries older than a cutoff (units: s/m/h/d, unit required)
kicadiff cache prune --older-than 30d
kicadiff cache prune --older-than 30d --dry-run # preview, change nothing
# Wipe the whole cache (recursive rm of the cache root — any stray files
# at the root go too, not just registered entries). `--yes` skips the
# confirmation prompt and is required in non-TTY (CI) environments so
# the prompt can never hang a build. As a safety net, `--all` refuses
# to run unless the cache root contains a `.kicadiff-cache` marker
# (auto-dropped on first cache write and on any `cache stats` /
# read) — that way a misconfigured `KICADIFF_CACHE_DIR` can't silently
# wipe an unrelated directory. For a pre-existing cache from before
# this marker was introduced, run `kicadiff cache stats` once to
# install the marker, then retry `--all`. Use `rm -rf` manually if
# you really mean to delete such a directory.
#
# Note: `cache stats` does NOT recurse into foreign top-level
# directories (anything whose name doesn't match the cache layout's
# 2-char hex bucket pattern). Their bytes are excluded from "Total
# size" — a misconfigured `KICADIFF_CACHE_DIR` (e.g. `$HOME`) won't
# make `stats` walk a huge unrelated tree. `--all` will still wipe
# the entire cache root, so it may reclaim more than `stats` reports.
kicadiff cache prune --all --yesGitHub Actions
Drop the action into a workflow to render a visual diff for every PR that touches a KiCad file. The action handles KiCad install, runs kicadiff, and (opt-in) uploads the rendered images as a build artifact, writes a job summary with inline before/after images, upserts a sticky PR comment, and updates a marked section in the PR description.
# .github/workflows/kicad-diff.yml
name: KiCad visual diff
on:
pull_request:
paths: ["**/*.kicad_pcb", "**/*.kicad_sch"]
permissions:
contents: read
pull-requests: write # only needed for pr-comment / pr-description
jobs:
diff:
runs-on: ubuntu-latest
steps:
- uses: actions/checkout@v6
with: { fetch-depth: 0 }
- uses: sksat/kicadiff@v0.2.0
with:
path: hardware/main-board # default: cwd
upload-artifact: 'true'
pr-comment: 'true'
pr-description: 'true'Job summary embeds combined PNGs as base64 data URIs (no extra hosting
needed) up to a 1 MiB cap; if a project's images would overflow, the
action drops the rest, emits ::warning::, and links to the artifact
for the full set. PR comment / description are kept text-only and link
to the artifact for images.
install-kicadiff: bunx (default) pulls the latest published kicadiff
on demand; pin a version with install-kicadiff: <semver>. Pre-installed
on PATH? Use install-kicadiff: skip.
More
DESIGN.md— architecture, render pipeline, cache key shape, manifest schema, viewer mode semanticsexamples/blink/— minimal KiCad project used as the test fixture and a usable starting point. Ships with a.claude/settings.jsonPostToolUse hook (kicadiff hook) that re-renders the diff every time a.kicad_pcb/.kicad_schis Edited / Written.examples/mcu-board/— a more realistic small-board layout: an 8-pin MCU stand-in with the usual stuff around it (5 V → 3.3 V AMS1117 LDO, decoupling caps, reset switch with pull-up, status LED, and a 6-pin programming/breakout header). Hierarchical schematic — root for the power chain and MCU itself,peripherals.kicad_schsub-sheet for the reset/LED/header — so the per-page tabs in the viewer have something to switch between.
Parts
15| Qty | Value | Footprint | References |
|---|---|---|---|
| 4 | M3 | MountingHole:MountingHole_3.2mm_M3 | H1, H2, H3, H4 |
| 2 | 10uF | C_0805_2012Metric | C1, C2 |
| 1 | 100nF | C_0805_2012Metric | C3 |
| 1 | 10k | R_0805_2012Metric | R1 |
| 1 | 1k | R_0805_2012Metric | R2 |
| 1 | 5V_IN | PinHeader_1x02_P2.54mm_Vertical | J1 |
| 1 | AMS1117-3.3 | SOT-223-3_TabPin2 | U2 |
| 1 | Green | LED_0805_2012Metric | D1 |
| 1 | MCU | SOIC-8_3.9x4.9mm_P1.27mm | U1 |
| 1 | PROG/IO | PinHeader_1x06_P2.54mm_Vertical | J2 |
| 1 | Reset | SW_SPST_TL3342 | SW1 |
More from sksat/kicadiff
1- 2 layers50 × 30 mm

Similar boards
- 2 layers290.1 × 130 mm

- 2 layers26.2 × 45.5 mm

PL18 multiprotocol
pascallanger/DIY-Multiprotocol-TX-Module
Multiprotocol TX Module (or MULTI-Module) is a 2.4GHz transmitter module which controls many different receivers and models.
24 parts1.9kGPL-3.0 - 4 layers99 × 53.3 mm

PSLab
fossasia/pslab-hardware
PSLab Hardware Design and Schematics https://pslab.io
199 parts1.7kApache-2.0 - 4 layers85 × 56 mm

- 4 layers100 × 54 mm

32Bit shift register
MaltWhiskey/Mega-Cube
16x16x16 PL9823 Cube with Teensy 4.0 and FlexIO driver
64 parts766 - 2 layers44.2 × 29.3 mm

- 2 layers78 × 60 mm

- 2 layers59.1 × 99.9 mm

Cheap FOCer 2 60mm
shamansystems/Cheap-FOCer-2
Low-Cost Motor Controller based on the VESC 6
193 parts407
Questions
How big is the Mcu board PCB?
It measures 80 × 50 mm and has 2 copper layers, 1.6 mm thick.
What parts does the Mcu board use?
15 parts, built around the AMS1117-3.3. The full list of its parts is on this page, with links to each part's symbol and footprint where PCBKit's library has them.
Where can I download the Mcu board KiCad files?
From the sksat/kicadiff repository on GitHub, at the commit this page was made from: the board is examples/mcu-board/mcu-board.kicad_pcb and its schematic examples/blink/blink.kicad_sch. PCBKit opens the board in the browser, with nothing to install.
Can I use the Mcu board design in my own project?
Its repository publishes it under the MIT licence: you may reuse it on that licence's terms (keep the author's notice, and for a copyleft licence share your changes alike).