Skip to the content
2 layers25 × 18 mmUsb ldo, the printed circuit board in 3D

A set of skills for Claude Code and Codex (Agent Skills format) plus pcbkit, a toolkit that is copied into each board project at a fixed version. Together they cover the whole KiCad 10 board flow:

Size
25 × 18 mm
Copper layers
2
Thickness
1.6 mm
Parts
9
Nets
6
Pads
28
Tracks, vias
38, 3
Pours
2
Routed
Yes
KiCad
KiCad 10.0 (file 20260206)
Created
11 Oct 2026
Updated
11 Oct 2026

Overview

Usb ldo is an open-source printed circuit board by kfihihc, from the kfihihc/pcb-pipeline repository on GitHub, published under the MIT licence. It is a 2-layer board of 25 × 18 mm with 9 parts on 6 nets, routed with 38 tracks and 3 vias.

It is built around the HT7533-1, CL21A106KAYNNNE and PZ254V-11-03P, with the USB4125-GF-A-0190 and KT-0603R among its other parts. Its parts include 3 resistors, 2 capacitors, 2 connectors, 1 IC and 1 diode.

Main components

5

README

README.md

pcb-pipeline: skills, toolkit and merge gate for open-source PCB design

English | 中文

A set of skills for Claude Code and Codex (Agent Skills format) plus pcbkit, a toolkit that is copied into each board project at a fixed version. Together they cover the whole KiCad 10 board flow:

requirements → parts → datasheet facts → official reference design comparison → schematic as code → simulation → rules, placement, routing → gate → review → release

mermaid
flowchart LR
  classDef agent stroke:#3987e5,stroke-width:2px
  classDef human stroke:#d95926,stroke-width:2px
  classDef tool stroke:#199e70,stroke-width:2px
  S1(Requirements):::agent --> S2(Parts):::agent --> S3(Datasheets):::agent --> S4(Reference design):::agent --> S5(Schematic):::agent --> S6(Simulation):::agent --> S7(Layout):::agent
  S7 --> G{8-check gate}:::tool
  G -- fail --> S7
  G -- pass --> R{{Review}}:::human --> P(Release):::agent --> B{{Bring-up}}:::human
  B -- errata --> S1

The principles:

  • KiCad is the single source of truth for the board.
  • Design intent is kept as text.
  • Every change passes a deterministic gate in Git and CI.
  • Routing uses open routers.
  • Agents change a design only through branches, change notes and pull requests.

Language. The skill instructions and the project documents are written in Chinese. Every skill description includes an English sentence to help agents identify relevant tasks in English; automatic selection has not been systematically evaluated.

  • How to use it: docs/SKILLS.zh-CN.md (Chinese). It has an overview diagram, a quick reference for the ten skills, example prompts, the life cycle of one change, the evidence chain and the data flow.
  • Why it is designed this way and what was verified: PIPELINE.zh-CN.md (Chinese).
  • The diagrams are Mermaid, which GitHub renders directly. For other viewers, SVG copies are in docs/diagrams/.

It grew out of an earlier survey of AI and EDA tools for hardware design (not part of this repository) and the experience of building a KiCad replica of an ESP32-S3 AMOLED board.

Skills

SkillWhat it doesBundled scripts
pcb-pipelineOrchestrator: stages, artifacts, rules for transactional changes; creates or adopts a project; upgrades pcbkitscripts/new_project.py, kit/, assets/template/
pcb-partsOffline search of the JLCPCB/LCSC parts library, alternates, BOM stock and cost, live pricesscripts/jlc_parts.py
pcb-datasheetDatasheet download with provenance, per-page search and rendering, facts.toml with page references, pinout check against KiCadscripts/datasheet.py
pcb-refdesignExport of official reference designs (KiCad, Altium, EAGLE, PDF), chip-centred surroundings, pin-by-pin comparisonscripts/refnet.py
pcb-schematicSKiDL circuit code → readable KiCad schematic; connectivity intent(in the project: pcbkit/sch_gen.py)
pcb-simSPICE benches, corners and assertions (libngspice)(in the project: pcbkit/sim.py)
pcb-layoutBoard outline, rules, net classes, pours, keepouts; sync, placement, pre-routing; transactional routing with KiCadRoutingToolsscripts/setup_krt.sh
pcb-gateThe 8-check gate, declarative metrics, CI, revision diff and change-scope check(in the project: pcbkit/gate.py, metrics.py, board_diff.py)
pcb-reviewReview packet (KiCanvas, interactive BOM, PcbDraw drawings, EMC pre-check leads), reviewer plus devil's-advocate passes, findings turned into gate checksscripts/setup_kicad_happy.sh (in the project: pcbkit/review.py)
pcb-releaseFabrication and review package, JLCPCB BOM/CPL, interactive BOM, panelization (the user decides), pre-order checks, tagging(in the project: pcbkit/release.py, extras.py)

The gate runs these 8 checks:

  1. ERC.
  2. DRC with schematic parity.
  3. A rules canary: a broken .kicad_dru is otherwise dropped silently.
  4. Zone refill.
  5. Netlist checks: connectivity intent, pins against pads, BOM fields and the parts register.
  6. Board metrics.
  7. Simulation assertions.
  8. Reproduction of generated files.

Installing the skills

1. Prerequisites

Needed forRequirement
EverythingLinux with KiCad 10 from your distribution: kicad-cli and KiCad's pcbnew Python module. Tested with Debian's KiCad 10.0.6 and Python 3.14. pcbkit uses the system KiCad and never downloads its own copy
Datasheetspoppler-utils (pdftotext, pdfinfo, pdftoppm)
Simulationlibngspice (Debian: libngspice0, already pulled in by KiCad)
Board projectsuv for the Python dependency groups (SKiDL, router, optional outputs), and git
Tests onlyrsync
The agentClaude Code and/or Codex

On Debian or Ubuntu:

bash
sudo apt install kicad poppler-utils libngspice0 git rsync pipx
pipx install uv          # or the installer from the uv website

2. Get the repository

bash
git clone https://github.com/kfihihc/pcb-pipeline.git
cd pcb-pipeline

Keep the clone: the skills are installed as symbolic links into it.

3. Link the skills

install.sh links every folder under skills/ into the personal skill folders of Claude Code (~/.claude/skills/) and Codex (~/.codex/skills/). It links only into folders that already exist, so create the ones for the agents you use first:

bash
mkdir -p ~/.claude/skills     # Claude Code
mkdir -p ~/.codex/skills      # Codex, only if you use it
./install.sh

Expected output, once per skill and agent:

text
linked  /home/you/.claude/skills/pcb-pipeline
linked  /home/you/.claude/skills/pcb-parts
...
  • skip … (not present) means that agent's skill folder does not exist; create it and run ./install.sh again.
  • CONFLICT … exists and is not a link means a skill of the same name is already installed. The script leaves it untouched; move it away first if you want this one.

Install all ten skills. They refer to each other: the orchestrator hands work to the stage skills, and the release skill uses references from the layout skill.

4. Check the installation

bash
./install.sh --check

This lists every link (ok, missing or CONFLICT) and checks the dependencies: kicad-cli, poppler, uv, git, libngspice, the parts database, the router and kicad-happy.

Then start a new Claude Code session so it loads the skills, and try one of these:

  • type /pcb-pipeline;
  • or just describe the task, for example "Design a small USB-C to 3.3 V board with pcb-pipeline". The agent chooses the skill from its description.

The ten skills have been discovered in both Claude Code and Codex, and their instructions have been read in Codex. This verifies discovery and access, not an end-to-end board design run in both agents.

5. One-time downloads (when a stage first needs them)

All of these go to ~/.cache/pcb-pipeline/, outside the repository:

ForCommandNotes
Parts search (pcb-parts)python3 skills/pcb-parts/scripts/jlc_parts.py fetch --db currentJLCPCB parts database, about 180 MB
Autorouting (pcb-layout)skills/pcb-layout/scripts/setup_krt.shKiCadRoutingTools v0.22.1 with its own uv environment
EMC pre-check (pcb-review, optional)skills/pcb-review/scripts/setup_kicad_happy.shkicad-happy v2.3.1; only its analysis scripts are used, its skills are not installed

The optional outputs (KiKit panel, InteractiveHtmlBom, PcbDraw) are installed per board project, in that project's uv environment: run uv sync --group extras in the project. kicanvas.js ships with pcbkit. docs/external-tools.zh-CN.md (Chinese) explains how these tools were chosen and why KiBot is not used.

Updating and removing

  • Update the skills: git pull in the clone. The links pick up the change at once; start a new agent session.

  • Update a board project's toolkit: each project keeps its own copy of pcbkit, so upgrade it deliberately, on its own branch, then run the gate:

    bash
    python3 <clone>/skills/pcb-pipeline/scripts/new_project.py <board> --update-kit
  • Remove: ./install.sh --uninstall removes only the links that point into this clone.

Other ways to install

  • One project only (Claude Code): link the skill folders into that project's .claude/skills/ instead of ~/.claude/skills/.
  • Copy instead of link: copying skills/* also works, but then git pull no longer updates them.

Quick start

bash
P=$PWD/skills       # run inside the pcb-pipeline clone
python3 "$P/pcb-pipeline/scripts/new_project.py" ~/boards/my-board --name my-board --title "My board" --size 40x30
cd ~/boards/my-board && git init
# then tell Claude Code / Codex: "Design this board with pcb-pipeline. The requirements are ..."
python3 pcbkit/gate.py          # the gate; run it at any time

To adopt an existing KiCad project:

bash
# Run from the pcb-pipeline clone; replace /path/to/existing-board.
python3 skills/pcb-pipeline/scripts/new_project.py /path/to/existing-board \
  --adopt --pcb x.kicad_pcb --sch x.kicad_sch

See examples/s3-adoption/ for a worked case.

Examples

  • examples/usb-ldo/: a small two-layer board taken from nothing to a fabrication package. Its README lists the problems each stage actually caught.
  • examples/s3-adoption/: the gate applied to the S3 AMOLED replica, with its 30 existing thresholds rewritten as declarative metrics.

Tests

bash
tests/run_tests.sh        # about 2 minutes

The suite runs the example's gate and negative tests for each check. It also covers simulation, reference designs, parts search, datasheets, and the optional outputs including panelization. A test whose data or tool is missing is skipped, not failed.

License

MIT, see LICENSE. This covers the skills, pcbkit, the documentation and the example designs.

New board projects default to MIT; use new_project.py --license <identifier> to choose another license. Check the upstream license when adopting or deriving an existing design.

Exceptions:

  • KiCanvas: kicanvas.js (skills/pcb-pipeline/kit/vendor/ and its copy in the example) keeps its own MIT license and copyright, in kicanvas.LICENSE.md next to it.
  • KiCad libraries: symbols and footprints from the KiCad libraries used in the example boards are under the KiCad library license (CC-BY-SA 4.0 with an exception for designs that use them).
  • Tools fetched at setup: these keep their own licenses. All are MIT: KiCadRoutingTools, kicad-happy, KiKit, InteractiveHtmlBom and PcbDraw.

Parts

9
QtyValueFootprintReferences
25.1kResistor_SMD:R_0603_1608MetricR1, R2
110uF 10VCapacitor_SMD:C_0603_1608MetricC2
110uF 25VCapacitor_SMD:C_0805_2012MetricC1
11kResistor_SMD:R_0603_1608MetricR3
1HT7533-1Package_TO_SOT_SMD:SOT-89-3U1
1Header 1x3Connector_PinHeader_2.54mm:PinHeader_1x03_P2.54mm_VerticalJ2
1USB-CConnector_USB:USB_C_Receptacle_GCT_USB4125-xx-x-0190_6P_TopMnt_HorizontalJ1
1redLED_SMD:LED_0603_1608MetricD1

Similar boards

  • 4 layers101 × 51.5 mmQuack core, the printed circuit board in 3D

    Quack core

    HeyPCB/quack-core

    Brain board for the Open Duck Mini: Pi Zero 2W carrier, 14-servo STS bus, fused 2S power path in stitched copper zones (15-18 A battery side), USB-C charging with balancing, IMU.

    138 parts1CERN-OHL-S-2.0
  • 2 layers160 × 70 mmSeedSigner Plus smartcard pico, the printed circuit board in 3D

    SeedSigner Plus smartcard pico

    lightningspore/shieldsigner-dev

    ShieldSigner Luckfox carrier: KiCad design, smartcard docs, reproducible build tools and HTMX knowledge site

    61 partsMIT
  • 2 layers60 × 40 mmCanary, the printed circuit board in 3D

    Canary

    offgridevices/offgrid-hardware

    Open hardware from OffGrid Devices. One folder per board. CERN-OHL-S.

    52 partsCERN-OHL-S-2.0
  • 4 layers50 × 69.5 mmRia, the printed circuit board in 3D

    Ria

    B44ken/ria

    ria is a small wheeled biped built for jumping and fast ground motion.

    107 parts
  • 4 layers85.1 × 87.7 mmArt big paw, the printed circuit board in 3D

    Art big paw

    HeyPCB/led-art

    Shaped LED boards inspired by films, each in its own colour: KiCad 10, JLCPCB-ready, CERN-OHL-S-2.0

    48 partsCERN-OHL-S-2.0
  • 4 layers55.6 × 101.5 mmArt melody, the printed circuit board in 3D

    Art melody

    HeyPCB/led-art-2

    More shaped LED boards inspired by films, each in its own colour: KiCad 10, JLCPCB-ready, CERN-OHL-S-2.0

    26 partsCERN-OHL-S-2.0
  • 4 layers128 × 51.4 mmQuack face, the printed circuit board in 3D

    Quack face

    HeyPCB/quack-face

    Face board for the Open Duck Mini's head: eye LEDs, projector driver, I2S amp and mic, antenna servos, shaped to the head. 4-layer KiCad 10 board plus printed standoffs, fit-checked in the head CAD.

    55 partsCERN-OHL-S-2.0

Questions

How big is the Usb ldo PCB?

It measures 25 × 18 mm and has 2 copper layers, 1.6 mm thick.

What parts does the Usb ldo use?

9 parts, built around the HT7533-1, CL21A106KAYNNNE, PZ254V-11-03P and USB4125-GF-A-0190. 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 Usb ldo KiCad files?

From the kfihihc/pcb-pipeline repository on GitHub, at the commit this page was made from: the board is examples/usb-ldo/hw/usb-ldo.kicad_pcb and its schematic examples/usb-ldo/hw/usb-ldo.kicad_sch. PCBKit opens the board in the browser, with nothing to install.

Can I use the Usb ldo 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).