Component Search (LCSC + easyeda2kicad)

Find and add component packages to a Zener project without relying on a private registry. The pipeline is:

MPN  ──►  LCSC C-number  ──►  easyeda2kicad  ──►  .kicad_sym + .kicad_mod + .step  ──►  Zener wrapper (.zen)

Use this workflow any time you need a part that isn't already in the workspace

components/

tree or covered by stdlib generics (

@stdlib/generics/Resistor.zen

Capacitor.zen

Led.zen

Thermistor.zen

, …).

Hard Stop Before Manual Creation

If LCSC has no entry for the MPN, or

easyeda2kicad

fails on the resolved C-number, don't fall back to hand-drawing a symbol/footprint silently. Report what failed, offer manual creation as an option, and get explicit user confirmation.

Search Priority

Always search in this order. Move down only when the higher tier doesn't apply.

Workspace
components/
tree —
```
glob
```
or
```
finder
```
for the MPN. If the part is already imported, reuse it via
```
Module("./components/<Mfr>/<MPN>/<MPN>.zen")
```
.
stdlib generics — for plain R, C, L, LED, diode, NPN/PNP, MOSFET, thermistor: use the generic, never import a vendor part.
LCSC + easyeda2kicad — for ICs, modules, connectors, crystals, anything with a specific MPN.

Step 1 — MPN → LCSC C-number

LCSC parts have a numeric

Cxxxxxx

ID. easyeda2kicad needs that ID, not the MPN. Use the agent's web tools:

web_search  query="<MPN> site:lcsc.com"
read_web_page  url=<top LCSC product page>  objective="Find the LCSC C-number (e.g. C25804) and confirm package."

Tips:

LCSC product URLs look like
```
https://www.lcsc.com/product-detail/.../C25804.html
```
— the trailing
```
Cxxxxx
```
before
```
.html
```
is the C-number.
The product page also lists package, datasheet, stock, and price — capture these for the user.
Some MPNs map to multiple C-numbers (different reels, suffixes, manufacturers). Pick the one that matches the requested package and shows real stock.
If no LCSC hit, try the base MPN family (drop
```
-TR
```
,
```
-R7
```
, reel/packaging suffixes).

When the user supplies a C-number directly, skip this step.

Step 2 — Import via easyeda2kicad

Resolve the manufacturer and a clean MPN slug first (no spaces, replace

with

). Pick a target package directory under

components/<Manufacturer>/<MPN>/

bash

mkdir -p components/<Manufacturer>/<MPN>
cd components/<Manufacturer>/<MPN>

easyeda2kicad --full --lcsc_id=Cxxxxx --output <MPN> --overwrite

This writes:

```
<MPN>.kicad_sym
```
— symbol library (single symbol)

<MPN>.pretty/<something>.kicad_mod

— footprint, inside a

.pretty

folder

```
<MPN>.3dshapes/<something>.{wrl,step}
```
— 3D model

Flatten the footprint so the Zener wrapper can reference it as a single file next to the

.zen

bash

mv <MPN>.pretty/*.kicad_mod ./<MPN>.kicad_mod
rmdir <MPN>.pretty

(Keep

<MPN>.3dshapes/

as a folder —

.kicad_mod

references the 3D model by relative path inside it.)

If the user wants to skip the 3D model for size, drop

--full

and use

--symbol --footprint

. Note that

pcb

does not require a 3D model to build.

Step 3 — Generate the Zener wrapper

Use the bundled generator script to turn the imported

.kicad_sym

into a starter

.zen

bash

python3 <SKILL_DIR>/scripts/zener-wrap.py \
  --kicad-sym components/<Manufacturer>/<MPN>/<MPN>.kicad_sym \
  --footprint <MPN>.kicad_mod \
  --mpn <MPN> \
  --manufacturer "<Manufacturer>" \
  --output components/<Manufacturer>/<MPN>/<MPN>.zen

The generator parses the

.kicad_sym

and emits a

.zen

skeleton with:

top docstring (MPN, manufacturer, package — fill in description by hand)
```
mpn
```
/
```
manufacturer
```
configs
one
```
io()
```
per pin, classified as
```
Power
```
,
```
Ground
```
, or generic
```
Net
```
by name
```
Component(...)
```
with the
```
pins=
```
dict mapping the original KiCad pin names to those ios

After generation, read the file and clean it up by hand:

Group related ios (split power, signal, control bundles).
Rename ios to integrator-facing names where it improves clarity (
```
+IN_A
```
→
```
IN_POS_A
```
).
Add
```
voltage="..."
```
to every
```
Power
```
io per the datasheet.
Replace
```
Net
```
with
```
Analog
```
/
```
Digital
```
/ typed interfaces from
```
@stdlib/interfaces.zen
```
where appropriate.
Remove
```
no_connect
```
pins from the
```
pins=
```
dict — leave them out, don't expose as ios.
Drop the auto-generated docstring and replace with a short, integrator-facing one (one paragraph: what it is, where it's used, key constraint).

See

idiomatic-zener

for the full style rules. See

reference-design

if you want to grow the wrapper into a richer reusable design with surrounding circuitry.

Step 4 — Workspace manifest

The new component package needs a

pcb.toml

so the workspace can resolve it. Create:

toml

# components/<Manufacturer>/<MPN>/pcb.toml
[package]
name = "<MPN>"
description = "<one-line description>"

If the workspace

pcb.toml

declares

members = [..., "components/*", ...]

(most do), the package is auto-discovered. Verify with:

bash

pcb build components/<Manufacturer>/<MPN>

Fix any errors before instantiating from a board.

Step 5 — Use it

python

MyPart = Module("./components/<Manufacturer>/<MPN>/<MPN>.zen")

MyPart(
    name="U1",
    VDD=vdd_3v3,
    GND=gnd,
    # ...
)

Verifying Sourcing with

pcb bom

Once the part is wired into a board, sanity-check sourcing:

bash

pcb bom boards/<Board>/<Board>.zen -f json

For an easyeda2kicad-imported part, the BOM will pick up the MPN you set in the wrapper (

mpn=

config default). LCSC stock is the same source easyeda2kicad pulled from, so the

Cxxxxx

you used is your sourcing record — capture it in the docstring or a

.zen

comment for traceability.

Generator Script

Path:

<SKILL_DIR>/scripts/zener-wrap.py

Usage:

bash

python3 zener-wrap.py \
  --kicad-sym path/to/<MPN>.kicad_sym \
  --footprint <MPN>.kicad_mod \
  --mpn <MPN> \
  --manufacturer "<Manufacturer>" \
  --output path/to/<MPN>.zen \
  [--datasheet docs/<MPN>.pdf]   # optional

Pin classification rules:

```
GND
```
,
```
VSS
```
,
```
VEE
```
,
```
AGND
```
,
```
DGND
```
,
```
V-
```
→
```
Ground
```
```
VCC
```
,
```
VDD
```
,
```
VPP
```
,
```
VBUS
```
,
```
VS
```
,
```
V+
```
,
```
AVDD
```
,
```
DVDD
```
,
```
VIN
```
,
```
VOUT
```
→
```
Power
```
everything else →
```
Net
```

The script never throws on unusual pin names — it sanitizes any string into a valid Zener identifier and falls back to

PIN_<num>

for unnamed pins.

Common Issues

easyeda2kicad: HTTP 404 on C-number — wrong C-number, or the part has been delisted. Re-search LCSC or pick the alternate-source listing.
Pin names look like
~{NAME}
(with overbar markup) — KiCad wraps inverted pin names in
```
~{...}
```
. The generator strips the markup for the io identifier but preserves the original string in the
```
pins=
```
dict so the symbol still matches.
Footprint references a 3D model that wasn't downloaded — happens with
```
--symbol --footprint
```
only. Either re-run with
```
--full
```
, or edit the
```
.kicad_mod
```
to remove the
```
(model ...)
```
block.
Symbol uses
~
/
#
/ spaces in pin names — the generator handles these. If the resulting Zener identifier is awkward, rename the io by hand and update the
```
pins=
```
mapping to keep the original KiCad name on the right.

component-search

NPX Install

Tags

SKILL.md Content

Component Search (LCSC + easyeda2kicad)

Hard Stop Before Manual Creation

Search Priority

Step 1 — MPN → LCSC C-number

Step 2 — Import via easyeda2kicad

Step 3 — Generate the Zener wrapper

Step 4 — Workspace manifest

Step 5 — Use it

Verifying Sourcing with
`pcb bom`

Generator Script

Common Issues