jlcpcb

name

jlcpcb

description

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.

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	Common parts (resistors, caps, diodes, common ICs) pre-loaded on pick-and-place machines	No extra fee
Extended	300k+ less common parts loaded on demand	$3 per unique extended part

JLCPCB occasionally promotes a subset of frequently-used extended parts with a discounted or waived feeder fee (the program's name and terms shift over time). Check the current JLCPCB parts library page for any specific extended part before assuming the standard $3 fee applies.

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

1. In KiCad schematic editor, add an LCSC field to each symbol with the LCSC part number
2. Export BOM as CSV with columns: Reference, Value, Footprint, LCSC
3. 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:

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

Ordering Workflow

Prototype Order (Bare PCB + Stencil)

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

Production Order (Assembled Boards)

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

Translating Altium / KiCad BOM and CPL files

For boards exported from Altium (or other tools) whose BOM/CPL formats don't match JLCPCB's expected columns, the bom skill ships translate_bom_pnp.py to convert them. Two subcommands:

# BOM: KiCad/Altium CSV → JLCPCB BOM CSV (Comment, Designator, Footprint,
#                                         LCSC Part #, MPN, Manufacturer,
#                                         Quantity, Notes)
python3 skills/bom/scripts/translate_bom_pnp.py bom input_bom.csv -o jlc_bom.csv

# CPL: input CPL → JLCPCB Pick-and-Place CSV (Designator, Mid X, Mid Y,
#                                              Layer, Rotation), with mil→mm
#                                              and TopLayer/BottomLayer
#                                              normalization
python3 skills/bom/scripts/translate_bom_pnp.py pnp input_cpl.csv -o jlc_cpl.csv

The 3-step PCBA upload workflow (avoids rejection)

JLCPCB's PCBA web upload rejects orders when the CPL contains designators that aren't in the BOM (mechanical holes, fiducials, test points, etc. that appear in the CPL output but aren't assembly components). The translator's --bom filter mode solves this:

1. Translate the BOM first — produces the JLCPCB-format BOM and establishes the authoritative designator set:

   python3 skills/bom/scripts/translate_bom_pnp.py bom input_bom.csv -o jlc_bom.csv
   

2. Translate the CPL with --bom filter — intersects CPL designators with BOM designators, dropping orphans:

   python3 skills/bom/scripts/translate_bom_pnp.py pnp input_cpl.csv -o jlc_cpl.csv --bom jlc_bom.csv
   

   The returned filtered_orphans count plus filtered_orphan_samples list lets the operator confirm which CPL rows were dropped — sanity- check this list before uploading. Common orphans (mounting holes, fiducials, test points) are expected; anything else may indicate a BOM/PCB mismatch worth investigating.

3. Tabulate consigned-parts cost separately — JLCPCB's quote does not auto-itemize consigned (user-supplied) part costs. Build a quote summary that shows: PCB fabrication, PCBA assembly fee, basic vs extended parts cost (per JLCPCB invoice), and a separate user-sourced parts subtotal. Without this breakdown the quote understates true unit cost by the consigned-parts amount.

This workflow is documented because JLCPCB's web upload UX silently rejects orphan-designator CPLs with an unhelpful error; the parity check via --bom is the single highest-value step in shipping a clean PCBA 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)