BOM Management in KiCad and EasyEDA: Export for JLCPCB

A Bill of Materials (BOM) is the complete list of every component used in your PCB design — part numbers, quantities, values, footprints, and sourcing information. Good BOM management is what separates a professional PCB design from a prototype that cannot be reproduced. For Indian engineers ordering assembled PCBs from JLCPCB, understanding how to structure and export your BOM is essential to getting accurate PCBA (PCB Assembly) quotes and error-free assembly.

This guide covers BOM generation in KiCad and EasyEDA, how to format BOMs for JLCPCB SMT assembly, component substitution strategies, and BOM management best practices.

What Is a BOM?

A BOM lists every unique component in your design along with:

• Reference designator (R1, C5, U3…)
• Value (10k, 100nF, ATmega328P…)
• Footprint/package (0402, SOIC-8, DIP-28…)
• Manufacturer and manufacturer part number (MPN)
• Quantity needed
• Unit cost (for quoting)

The BOM is used by: assembly houses for ordering components, procurement teams for cost estimation, inventory management systems, and production records for traceability.

BOM Fields and Attributes

In your EDA tool schematic, every component symbol should have these properties filled in:

BOM Generation in KiCad

Method 1: Built-in BOM Export (KiCad 7+)

1. In KiCad Schematic Editor, go to Tools > Generate BOM
2. The built-in BOM dialog opens. Select the output format (CSV is most useful)
3. Choose fields to include: Reference, Value, Footprint, Quantity, and any custom fields you added (MPN, LCSC, etc.)
4. Set “Group By” to Value + Footprint to consolidate identical parts
5. Click Generate — saves as a .csv file

Method 2: KiCad BOM Script Plugins

KiCad supports Python-based BOM plugins. Popular options:

• bom_csv_grouped_by_value: Built-in KiCad plugin, groups parts by value. Good for manual ordering.
• KiCost: A Python tool that auto-fetches prices from distributors (Mouser, DigiKey, LCSC) and generates a cost-optimized BOM. Install via pip: pip install kicost
• InteractiveHtmlBom: Generates an interactive HTML BOM with PCB overlay — extremely useful for manual assembly. Download from GitHub (openscopeproject/InteractiveHtmlBom).

Adding Custom Fields in KiCad Schematic

To add LCSC part numbers to every component:

1. Select a component in the schematic
2. Press E to open properties
3. In the “Fields” tab, click Add Field
4. Name the field “LCSC” (exact capitalization matters for JLCPCB BOM import)
5. Enter the LCSC part number (e.g., C17497 for a common 10k 0402 resistor)
6. Repeat for all components

Tip for efficiency: Edit the symbol in the symbol library to include the LCSC field with a default value. This saves entering it on every schematic instance.

KiCad BOM CSV Column Order for JLCPCB

JLCPCB’s BOM importer expects specific column names. Configure your KiCad BOM export to match or rename columns afterward:

Required JLCPCB BOM columns:
  Comment  (= Value field)
  Designator  (= Reference, comma-separated for groups: "R1,R2,R5")
  Footprint  (= package description)
  LCSC Part Number  (= LCSC field)

BOM Generation in EasyEDA

EasyEDA Native BOM Export

1. In EasyEDA Schematic Editor: go to Fabrication > BOM (Bill of Materials)
2. EasyEDA auto-generates a BOM from component properties
3. Review the list: verify LCSC Part Numbers are populated for all components you want assembled
4. Download as CSV or XLS

Setting LCSC Part Numbers in EasyEDA

EasyEDA integrates directly with LCSC (both owned by JLCPCB parent company EasyEDA/SZLCSC):

• Search for a component in EasyEDA’s component library — LCSC part numbers are already linked for library components
• For custom components: in component properties, set the “LCSC Part Number” attribute directly
• EasyEDA’s one-click JLCPCB order automatically passes the LCSC numbers to the assembly order

JLCPCB BOM Format

When uploading your BOM to JLCPCB for SMT assembly (PCBa service), the BOM CSV must have these columns:

Comment,Designator,Footprint,LCSC Part Number
10k,"R1,R2,R3",R_0402_1005Metric,C17497
100nF,"C1,C2,C4,C5",C_0402_1005Metric,C307331
ATmega328P-AU,U1,TQFP-32,C14877
1uF,C3,C_0805_2012Metric,C28323

Important rules:

• Multiple designators for identical parts must be in a single cell, comma-separated and quoted: “R1,R2,R5”
• LCSC part numbers must be current (LCSC stock can go out of stock — verify availability before ordering)
• Footprint column is informational for JLCPCB — they use the Gerber/CPL for actual placement
• Components with no LCSC number cannot be assembled — mark them as “Do Not Place” or source externally

Basic vs Extended Library at JLCPCB

JLCPCB divides components into:

• Basic library: ~1000 most common passives and ICs. Free to use (no extra setup fee). Mark with “(Basic)” in part picker.
• Extended library: 300,000+ parts. Each unique extended part adds a ¥3 setup fee per part.

For cost optimization, use Basic library parts wherever possible (common 0402/0603 resistors and capacitors, standard logic ICs).

LCSC Part Numbers and JLCPCB Assembly

Finding LCSC Part Numbers

• Search lcsc.com directly for your component value, package, and specs
• Use yaqube.de/kicad-bom-tools for KiCad-specific LCSC lookup
• EasyEDA component library shows LCSC numbers inline
• Component Search Engine (componentsearchengine.com): enter your component, get multi-distributor links including LCSC

Verifying LCSC Availability Before Ordering

Always check LCSC stock levels before finalizing your BOM for assembly. JLCPCB will reject parts that are out of stock. Use the LCSC website or JLCPCB’s BOM upload tool which checks stock in real time during order entry.

CPL (Component Placement List)

JLCPCB requires a CPL file (also called pick-and-place or PnP file) in addition to the BOM. The CPL defines the X,Y coordinates and rotation of every SMD component to be assembled.

KiCad CPL Export

1. In KiCad PCB Editor: File > Fabrication Outputs > Component Placement (.pos)
2. Set: Format = CSV, Units = mm, Only SMD footprints = Yes (for JLCPCB SMT assembly)
3. KiCad generates a .pos file with columns: Ref, Val, Package, PosX, PosY, Rot, Side
4. JLCPCB CPL column names: Designator, Val, Package, Mid X, Mid Y, Rotation, Layer
5. Rename columns to match JLCPCB’s expected names

EasyEDA CPL Export

EasyEDA’s Fabrication > PCB Fabrication File automatically includes the CPL in the download package. Named as “Gerber_PickAndPlace_*.csv”.

Common CPL Issues

• Rotation offset: KiCad’s footprint rotation origin and JLCPCB’s pick-and-place machine reference can differ by 0, 90, 180, or 270 degrees depending on the footprint. If assembled components are rotated, add offsets in the CPL file for those footprints.
• Origin mismatch: JLCPCB uses the board origin as 0,0. Ensure your board origin (set in PCB Editor) matches the expected reference point.

BOM Management Best Practices

• Use LCSC numbers in every schematic component: This allows direct BOM-to-assembly-order flow and eliminates manual lookup at order time.
• Verify stock before design freeze: Check LCSC stock for all non-standard components. If a critical IC is out of stock, find alternatives early — not after PCBs arrive from the fab.
• Prefer Basic library parts for passives: Use standard E-series values (10k, 100nF, 1uF) from JLCPCB’s Basic library to minimize extended part fees and stock risk.
• Version your BOM: Keep BOM in version control (git) alongside your KiCad project. Tag BOM versions with hardware revisions.
• Separate DNP (Do Not Place) components: Mark test points, optional components, and debug features as DNP in your BOM. JLCPCB accepts DNP designators and will skip those pads.
• Document substitutions: When you substitute an equivalent part (different manufacturer, same specs), note it in the BOM “Notes” column for traceability.

Component Substitution in India

LCSC/JLCPCB primarily stocks Chinese brand components. For prototypes assembled in India (hand assembly or local assembly house), you may need to source from Indian distributors:

• Mouser India: Wide range of Vishay, Murata, TDK passives and ICs. Higher pricing than LCSC but genuine parts with full traceability.
• DigiKey India: Similar to Mouser, excellent for specialized components
• Element14 (India): Farnell/Avnet distribution, strong industrial component selection
• Robu.in, Zbotic.in: For development boards, popular modules, and project components

When substituting, verify: value, package, and critical specifications (voltage rating, tolerance, temperature coefficient for capacitors). Document in BOM with MPN cross-reference.

Frequently Asked Questions