Skip to content

JLCPCB_WORKFLOW.md

Latest commit

 

History

History
177 lines (125 loc) · 9.62 KB

JLCPCB_WORKFLOW.md

File metadata and controls

177 lines (125 loc) · 9.62 KB
Raw

JLCPCB Assembly Workflow (KiCad + Bouni Plugin)

How OpenMuscle hardware revisions get from a routed KiCad project to a JLCPCB order. The procedure is the same for every board (Flex, Rigid, future revisions); only the specific LCSC parts change.

This document captures the workflow we use today. It is generic enough to apply to any V4+ revision of the FlexGrid or other Open Muscle boards.

Toolchain

Component What it does
KiCad 8.x Schematic capture + PCB layout (you already have this)
kicad-jlcpcb-tools plugin LCSC part search, LCSC-number tagging on components, BOM + CPL + Gerber generation in JLCPCB-friendly format
JLCPCB web ordering page https://jlcpcb.com/ (where the generated files actually get uploaded)

Plugin install (one-time per machine)

The plugin is not in KiCad's official Plugin and Content Manager repository, so two install paths:

Option A: Install from a release zip (recommended)

  1. Download the latest release from https://github.com/Bouni/kicad-jlcpcb-tools/releases (looks like KiCadJLCPCBTools.zip or similar)
  2. KiCad main window → Tools → Plugin and Content Manager
  3. Click Install from File... at the bottom
  4. Pick the downloaded zip
  5. Apply Pending Changes, restart KiCad

Option B: Add Bouni's PCM repository for auto-updates

  1. PCM dialog → Manage... (top right)
  2. Add a new repository:
    • Name: Bouni's repo
    • URL: https://raw.githubusercontent.com/Bouni/bouni-kicad-repository/main/repository.json
  3. Switch the repository dropdown to "Bouni's repo"
  4. Search jlcpcb, install the plugin, restart KiCad

After install: the plugin appears as a button in the PCB Editor toolbar (not the schematic editor). Also accessible at Tools → External Plugins → JLCPCB Tools.

Per-revision workflow

The 5 phases below run in order for every new revision. Each phase is a checkpoint; don't skip ahead.

Phase 1: tag LCSC parts on every component

Open the PCB editor for the board you are about to fab. Click the JLCPCB Tools button. A side panel opens listing every component on the board, color-coded:

  • Green = LCSC part is assigned, BOM and POS toggled on
  • Red = no LCSC part yet, needs attention
  • Yellow / partial = mixed state (some flags off)

For each red row:

  1. Click the row in the panel
  2. Click Assign LCSC number
  3. The plugin opens a search dialog into LCSC's catalog
  4. Search by part value (e.g. 100nF 0603 for a cap, or by exact MFR name like BSS84)
  5. Check all three tier boxes: Basic, Preferred, Extended
  6. Also check Only show parts in stock
  7. Look at the Package column to verify it matches your KiCad footprint
  8. Pick the row with the best stock + tier
  9. Click Select part

The LCSC number is now associated with that component.

Phase 2: handle hand-soldered parts

Any part you intend to hand-solder after JLC assembly (microSD socket, FFC connector, pin headers, battery JST, through-hole anything) should be excluded from both BOM and POS so JLC neither sources nor places it.

  1. Select the row in the plugin panel
  2. Click Toggle BOM POS (or Toggle BOM + Toggle POS individually)
  3. The BOM and POS columns should flip to red X marks
  4. Leave the LCSC field empty or as-is; the exclusion is what matters

A separate column called POP (Place On PCB) shows whether JLC's machines can actually assemble the part. POP = X means the part is sourceable but not assembleable; fix by picking a different LCSC part or accept the part as hand-soldered.

Phase 3: tier and stock sanity pass

Before generating, scan the panel for risk patterns:

  • Count rows with Type = Extended. Each one adds $3 setup fee to your order. Worth checking if a Basic-tier equivalent exists.
  • Look for rows with Stock < 1000. Those parts can go out of stock between now and when JLC places the order. Substitute if possible.
  • Spot-check value vs LCSC Params. The schematic value (e.g. "10k") should match the LCSC part description (e.g. "10kΩ ±1% 0603"). Mismatches are silent assembly bugs.

Phase 4: save and export

  1. Save mappings (button on the right side of the plugin panel). This writes your LCSC choices into the plugin's database for re-use across projects.
  2. Export to schematic. This writes the LCSC field into each component's symbol in the schematic file.
  3. Open the Schematic Editor and press Ctrl+S to actually save the schematic file (this is the step people miss; the export-to-schematic only marks the file as modified)

Phase 5: generate fab files

Back in the PCB editor JLCPCB plugin panel:

  1. Click Generate fabrication files for JLCPCB (top-left button)
  2. The plugin creates a jlcpcb/ directory next to your .kicad_pcb file containing:
jlcpcb/
|-- gerber/                                       individual Gerber + drill files
`-- production_files/
    |-- GERBER-<projectname>.zip                  what you upload
    |-- BOM-<projectname>.csv                     BOM with LCSC numbers
    `-- CPL-<projectname>.csv                     pick-and-place coordinates
  1. Open and verify the BOM and CPL CSVs:
    • BOM: every row should have a non-empty LCSC column (Cxxxxx format)
    • BOM: hand-soldered parts should be absent from the list
    • CPL: same set of designators as the BOM
    • Spot-check one or two rotation values against the part's datasheet pin-1 orientation (the plugin applies JLC's known rotation corrections automatically; this is a sanity check, not a fix)

Uploading to JLCPCB

Order page: https://jlcpcb.com/quote

  1. Drag the GERBER-<projectname>.zip into the gerber upload field
  2. JLCPCB reads the gerbers and shows a board preview. Verify board outline, layer count, dimensions, drill positions.
  3. Choose your PCB options (layers, thickness, color, surface finish, etc.)
  4. Toggle on PCB Assembly. Pick:
    • Assembly Side: single-side (TOP) by default. Choose double-side only if you have BOT components that need SMT placement.
    • Tooling holes: per JLCPCB's recommendation
    • Confirm parts placement: yes (gives you a final visual review)
  5. Upload the BOM CSV when prompted
  6. Upload the CPL CSV when prompted
  7. JLC processes the files. Within ~30 minutes you receive a parts placement preview email asking you to confirm rotations and positions before they cut metal.

Always review the placement preview. This is where rotation errors are caught (e.g., a SOT-23 placed 180 degrees rotated would short power to ground). If anything looks wrong, the plugin's rotation correction is the most common cause; adjust in KiCad, regenerate, re-upload.

BOM presentation in a public repo

A common ask for an open-hardware project: the repo's BOM should be readable by people who are not going to fab the board, while the BOM JLC actually uses needs to be machine-readable and accurate.

Two-file pattern:

File Audience Source of truth?
jlcpcb/production_files/BOM-<projectname>.csv JLCPCB Yes, this is what they assemble from. Do not hand-edit; regenerate from the plugin.
Optional BOM/Hand-Solder-Notes.md or repo README section Humans browsing the repo Human-friendly notes about what is hand-soldered and why

The plugin-generated BOM only includes parts JLC will assemble, which is what you want for the manufacturer. Hand-soldered parts get documented separately as prose, with the canonical list living in the revision's README (e.g. KiCad/OM-FlexGrid V4/README.md → "Hand-soldered parts").

Tips earned the hard way

  • Avoid "Auto-select alike" as a bulk action. It groups parts by footprint, not value, and will happily tag every 0603 resistor with the same LCSC number regardless of resistance. Tag manually one value at a time.
  • Check the Package column on every search result. Same MFR number can come in different packages; SOT-23 vs SOT-323 vs TSOT-23 look similar in name but have different pad geometry.
  • TSOT-23-6 is pad-compatible with SOT-23-6, same pitch + same pad layout, just thinner profile. A common gotcha when a part is only available in TSOT.
  • SOD-123FL is NOT pad-compatible with SOD-123, different pad geometry. Check before assuming.
  • Basic and Preferred tiers have no setup fee, Extended has $3 per unique part. A board with 5 Extended-tier parts costs $15 more in setup than a board with 5 Basic equivalents. Worth optimizing for.
  • The "Save mappings" plugin database remembers your choices across projects. After you have tagged a bunch of common values once, future projects auto-suggest the same LCSC parts.
  • POP = X in the plugin means JLC can source the part but cannot auto-place it. Pick a different LCSC part; do not just ignore the warning, the assembly will not happen.
  • For double-side assembly, JLC charges meaningfully more than single-side. If your BOT side has only one or two SMD parts, consider moving them to TOP in the next revision.

Workflow checklist (copy this into the revision's commit message)

[ ] Every component tagged with an LCSC part number (or explicitly excluded)
[ ] All hand-soldered parts have BOM and POS toggled OFF
[ ] No POP = X warnings remaining (or accepted as hand-soldered)
[ ] Tier mix is acceptable (counted Extended-tier parts, weighed setup cost)
[ ] Stock levels checked (no parts at < 1000 in stock)
[ ] Mappings saved + exported to schematic + schematic saved
[ ] Fab files regenerated AFTER schematic save
[ ] BOM CSV manually inspected (LCSC values present, hand-solder parts absent)
[ ] CPL CSV manually inspected (designators match BOM, rotations sane)
[ ] 3D STEP exported for mechanical fit check (if board lives in an enclosure)