jlcpcb

Original：🇺🇸 English

Translated

JLCPCB PCB fabrication and assembly — BOM/CPL generation, basic vs extended parts, assembly constraints, design rules, ordering workflow. Use with KiCad for JLCPCB manufacturing. Use this skill when the user mentions JLCPCB, wants to order PCBs or assembled boards, needs prototype bare PCBs and stencils, wants to know JLCPCB design rules and capabilities, or is asking about PCB manufacturing costs or turnaround times. For gerber/CPL export, stencil ordering, and BOM management, see the `bom` skill.

2installs

Sourceaklofas/kicad-happy

Added on2026-04-25

NPX Install

npx skill4agent add aklofas/kicad-happy jlcpcb

SKILL.md Content

View Translation Comparison →

JLCPCB — PCB Fabrication & Assembly

JLCPCB is a PCB fabrication and assembly service based in Shenzhen, China. It is a sister company to LCSC Electronics (common ownership) — they share the same parts library.

Typical usage: Order bare prototype PCBs + framed stencil from JLCPCB during prototyping (parts sourced separately from DigiKey/Mouser, hand-assembled in lab). For production runs (100s qty), order fully assembled boards from JLCPCB using LCSC parts. PCBWay is an alternative assembler. For component searching, see the

lcsc

skill. For BOM management, gerber/CPL export, and stencil ordering, see the

bom

skill.

Related Skills

Skill	Purpose
`kicad`	Read/analyze KiCad project files, DFM scoring against JLCPCB capabilities
`bom`	BOM management, gerber/CPL export, stencil ordering
`digikey`	Search DigiKey (prototype sourcing, primary — also preferred for datasheet downloads via API)
`mouser`	Search Mouser (prototype sourcing, secondary)
`lcsc`	Search LCSC (production sourcing — JLCPCB uses LCSC parts library)
`pcbway`	Alternative PCB fabrication & assembly
`emc`	EMC pre-compliance risk analysis — run before fab to catch EMC issues
`spice`	SPICE simulation — verify analog subcircuits before committing to fab

Assembly Parts Library

Part Categories

Category	Description	Assembly Fee
Basic	~698 common parts (resistors, caps, diodes, etc.) pre-loaded on pick-and-place machines	No extra fee
Preferred Extended	Frequently used extended parts	No feeder loading fee (Economic assembly)
Extended	300k+ less common parts loaded on demand	$3 per unique extended part

LCSC Part Numbers

Every assembly component is identified by an LCSC Part Number (

Cxxxxx

, e.g.,

C14663

). This is the definitive identifier for BOM matching. See the

lcsc

skill for searching parts.

Parts Search (JLCPCB-Specific)

Parts library:

https://jlcpcb.com/parts/componentSearch?searchTxt=<query>

Basic parts only:
```
https://jlcpcb.com/parts/basic_parts
```

BOM Format for Assembly

JLCPCB accepts CSV, XLS, or XLSX BOMs with these columns:

Column	Required	Description
`Comment` / `Value`	Yes	Component value (e.g., 100nF, 10k)
`Designator`	Yes	Reference designators, comma-separated (e.g., C1,C2,C5)
`Footprint`	Yes	Package/footprint name
`LCSC Part #`	Recommended	LCSC part number (Cxxxxx) — guarantees exact match

The column header for LCSC numbers must be exactly "LCSC Part #" or "LCSC Part Number" — typos cause upload failures.

KiCad BOM Export for JLCPCB

In KiCad schematic editor, add an
```
LCSC
```
field to each symbol with the LCSC part number
Export BOM as CSV with columns: Reference, Value, Footprint, LCSC

Rename columns to match JLCPCB's expected format:

```
Reference
```
->
```
Designator
```
```
Value
```
->
```
Comment
```
```
Footprint
```
->
```
Footprint
```
```
LCSC
```
->
```
LCSC Part #
```

For gerber export settings, CPL format, and stencil ordering, see the

bom

skill.

JLCPCB Official API (Approval Required)

Apply at

https://api.jlcpcb.com

. Access is gated — requires review based on order history and business profile.

Available APIs (once approved):

Components API — real-time pricing, inventory, component specs
PCB API — upload gerbers, get quotes, place orders, track status
Stencil API — stencil quoting and ordering
3D Printing API — SLA/MJF/SLM/FDM ordering

PCB Design Rules (JLCPCB Capabilities)

Standard PCB (1-2 layers)

Parameter	Minimum
Trace width	0.127mm (5mil)
Trace spacing	0.127mm (5mil)
Via diameter	0.45mm
Via drill	0.2mm
Annular ring	0.125mm
Min hole size	0.2mm
Board thickness	0.4-2.4mm (default 1.6mm)
Min board size	6x6mm
Max board size	500x400mm (2-layer)

Multi-layer (4+ layers)

Parameter	Minimum
Trace width	0.09mm (3.5mil)
Trace spacing	0.09mm (3.5mil)
Via diameter	0.25mm
Via drill	0.15mm
Board thickness	0.6-2.4mm

Importing DRU into KiCad

If you have a JLCPCB

.kicad_dru

design rules file, import it in KiCad Board Editor > Board Setup > Design Rules > Import Settings.

Assembly Constraints

Economic vs Standard Assembly

Feature	Economic	Standard
Sides	Top only	Top + Bottom
Component types	SMD only	SMD + through-hole
Min component size	0201	01005
Fine-pitch BGA/QFP	Down to 0.5mm pitch	Down to 0.4mm pitch
Turnaround	~3-5 days	~3-5 days
Extended part fee	$3 per unique part	$3 per unique part

General Constraints

Minimum order: 5 PCBs for assembly
Unique parts limit: No hard limit, but each extended part adds $3
Basic parts: No extra fee, pre-loaded on machines

Rotation Offsets

JLCPCB's pick-and-place uses different rotation conventions than KiCad for some footprints. Common offsets:

Footprint Family	Typical Offset
SOT-23, SOT-23-5, SOT-23-6	+180°
SOT-223	+180°
SOIC-8, SOIC-16	+90° or +270°
QFN (all sizes)	+90°
SMA/SMB/SMC diodes	+180°
USB-C connectors	Varies — check datasheet

To fix rotation issues:

Add rotation corrections directly in the CPL file before uploading (adjust the Rotation column)
For custom footprints, verify pin 1 orientation matches JLCPCB expectations
JLCPCB's review step catches major errors, but subtle 180° rotations on symmetric parts (caps, resistors) may slip through
After first assembly order, note any rotation corrections needed and apply them to future CPL exports

Ordering Workflow

Prototype Order (Bare PCB + Stencil)

Export gerbers from KiCad (see
```
bom
```
skill for export settings)
Upload gerbers to
```
https://cart.jlcpcb.com/quote
```
— configure layers, thickness, color, qty
Add a framed stencil to the cart (uses paste layers from your gerbers)
Order — PCBs and stencil typically arrive in ~1 week

Production Order (Assembled Boards)

Export gerbers from KiCad (see
```
bom
```
skill for export settings)
Export BOM as CSV with LCSC part numbers (format above)
Export CPL (placement file) as CSV (see
```
bom
```
skill for format)
Upload gerbers to
```
https://cart.jlcpcb.com/quote
```
— configure layers, thickness, color, qty
Enable "PCB Assembly", select Economic or Standard
Upload BOM and CPL files
Review part matching — fix any unmatched parts by searching LCSC numbers
Confirm and order

Tips

Prefer Basic parts — no extra fee, always in stock, faster assembly
Check stock before ordering — extended parts can go out of stock; use the
```
lcsc
```
skill to search
Panel by JLCPCB — for small boards, let JLCPCB panelize (cheaper) vs custom panels
Lead-free solder — default is leaded (HASL); select lead-free HASL or ENIG if needed
Impedance control — available for multi-layer boards, specify stackup in order notes
Castellated holes — supported, enable in order options
V-cuts and mouse bites — supported for panel separation
Silkscreen minimum — 0.8mm height, 0.15mm line width for readable text
Edge clearance — keep copper >=0.3mm from board edge (0.5mm recommended)