JLCPCB Package Preparation
The corner-support review destination tracks the 110 × 85 mm Board B with four independent corner holes, the shifted front-side PD stack and seven contacts moved right along the top edge. The PCB is implemented; native layout and power-path checks pass. Package reports determine CAD and export status. Read the manufacturing guide alongside the package's check reports, assembly drawings and BOM/CPL tables. Physical wire fit, tightening torque, leg clearance, connector seating and full-load qualifications remain open. The separately developed 18 mm printed leg addresses the earlier HC-11 option's nominal height conflict without changing the PCB or package. Check the support contract, including actual M3 passage through the existing Ø3.0 mm PCB holes. Only the current prototype package is maintained; no renewal hardware has been released or ordered.
Export each board independently from its final KiCad project. Retain validation reports and exports with the current prototype package. Record source revision, board dimensions and tool versions.
| File | Review |
|---|---|
| Gerber ZIP | Copper, mask, silkscreen and Edge.Cuts for the intended stack |
| Drill data | Plated/non-plated holes, units and origin |
| BOM CSV | References, values, footprints, exact LCSC codes; DNP omitted |
| CPL CSV | References, X/Y, rotation and side; DNP omitted |
| ERC/DRC reports | Errors resolved or accepted exclusions documented |
| Release manifest | Revision, dimensions, assembly scope and blockers |
Reconcile the package
BOM and CPL must cover the same fitted assembly scope. Through-hole connectors need an explicit assembly decision; a stock listing alone does not establish standard SMT assembly coverage. Review pin 1, key orientation and component rotations against the PCB in the order preview.
Inspect Gerber and drill views independently of the PCB editor. Confirm outline, mounting-hole centers, plated/non-plated classification and mating-cable clearance. The four corner holes are Ø3.0 mm NPTH, distinct from the three Ø3.2 mm PD mounts. Keep separately installed adhesive supports outside the electrical BOM and CPL. The C4749189 connectors replace the old printed-guard requirement; the historical guard-shaped outline is not the new mechanical specification.
J6/J7 now use two-pole screw-terminal blocks with wire entries facing left. Check J6.1=GND, J6.2=−12 V, J7.1=+5 V and J7.2=+12 V in both the schematic and assembly preview. Confirm both the retained front voltage labels and normally readable back labels against those pins. Check the front-down installation and front-side J5 stack in the assembly preview. The current left edge is plain. The printed accessory is the adhesive leg; no printed connector guard is required.
A package can exist while its design still has blockers. Its manifest must list those blockers and must not label it ready to order until the release gates are closed.
After an order is placed, retain exactly the submitted files in jlcpcb-order-snapshots/ and advance the order counter through the versioning workflow. Preparing files alone does not count as a PCBA order.
Repository export and independent rendering
Generate a temporary candidate from the current design using a new output directory:
python3 scripts/pcb/export-jlcpcb.py tmp/current-prototype-export --boards board-p board-b
uv run --with gerbonara --with resvg-py python scripts/pcb/verify-jlcpcb.py tmp/current-prototype-exportThe exporter checks ERC, DRC and schematic/PCB parity. Inspect its reports and the manufacturing guide for actual release status. The independent rendering step checks the manufactured layer files separately from KiCad. Both commands operate on local files and do not submit an order. After validation, replace the sole current package in manufacturing/; do not accumulate renewal backup sets. Keep the current package's source locks, checksums and reports consistent with its actual files.