# Manufacturing and assembling the Astra prototype

The final fabrication report records the checks on the released files, their revision, and the stock reported for a two-board order. Viewer captures and visual observations

## Fabrication order settings

Rigid FR-4 PCB, two layers, final nominal thickness 1.00 mm, 1 oz copper on outer layers, ENIG, green mask on both sides, components mounted on TOP. Standard PCBA process accepts BGA with 0.40 mm pitch on RT6160. The assembly panel requires process rails at least 5 mm wide on two sides, plus optical fiducials. Switching to HASL affects the flatness of WLCSP lands. At 1.00 mm, JLCPCB publishes a thickness tolerance of ±10%. The milled contour has a standard accuracy tolerance of ±0.20 mm. [PCB Rigid Capabilities](https://jlcpcb.com/capabilities/pcb-capabilities) · [PCBA Capabilities](https://jlcpcb.com/capabilities/pcb-assembly-capabilities) · [Processing Rails and Optical References](https://jlcpcb.com/help/article/how-to-add-edge-rails-fiducials-for-pcb-assembly-order)

Delivery uses Cartesian coordinates TOP, in millimeters, referenced to the origin of the board outline. For the assembly panel, JLCPCB can add fiducials and tooling holes on the panel rails. The side toward which the antenna extends must remain free, as must the space required for connectors. If a process edge intersects a component extending beyond the board, a clearance is milled. The supplier may use a reflow carrier for overhanging components. [Panelization](https://jlcpcb.com/help/article/96-PCB-Panelization) · [Clearances for protruding components](https://jlcpcb.com/blog/v-cut-panelization-standards) · [Support devices](https://jlcpcb.com/help/article/pcb-assembly-fixtures)

For 1 oz copper on two layers, the published limits are 0.10 mm for trace width, 0.10 mm between traces, 0.15 mm between SMD land pads from different nets, and 0.20 mm to the cut edge. Between via holes, a clearance of 0.20 mm is required, and between terminal holes, 0.45 mm is required. The separation from the hole edge to the trace is 0.20 mm for vias or NPTH, and at least 0.28 mm for PTH. For PTH terminals on 1 oz boards, 0.18 mm is the absolute limit for the annular ring, and 0.25 mm is the recommended value. [Holes, traces, and outlines](https://jlcpcb.com/capabilities/pcb-capabilities)

The minimum solder-mask dam width for green mask is 0.10 mm. Between an opening and the copper of an adjacent trace, the threshold is 0.09 mm. The silk screen uses characters of at least 1.0 mm, a line width of 0.15 mm, and a distance of 0.15 mm from the land. Use the assembly drawing for reference designators that are hard to read. Check the separate hole rules for vias, mounting holes and component leads. [Mask and silk screen](https://jlcpcb.com/capabilities/pcb-capabilities)

## Solder paste and reflow inspection

RT6160 features 15 contacts with a pitch of 0.40 mm. For the mask-defined land, the Richtek drawing allows adjustment of ±0.025 mm. A copper land diameter of 0.250 mm and an opening of 0.220 mm ensure a 0.150 mm gap between copper and a 0.180 mm gap between openings. For the circular opening of Ø0.220 mm, the area ratio of the opening to the sidewall area is `d/(4t)`. At a local thickness of 0.080 mm, the ratio is 0.688. At 0.100 mm, the ratio is 0.550. The stencil specification is a 0.10 mm foil for the general board and a 0.08 mm region at RT6160, on the template in frame. Request SPI inspection of the deposits and radiography for this WLCSP after reflow. For the pilot lot, acceptance includes all 15 balls being populated and the absence of bridges. [Richtek Drawing, last page of footprint](https://www.richtek.com/assets/product_file/RT6160A/DS6160A-05.pdf) · [Stencil capabilities](https://jlcpcb.com/capabilities/pcb-stencil-manufacturing) · [Area ratio for BGA](https://jlcpcb.com/blog/bga-stencil-design-apertures-thickness-tips)

Hirose specifies a local foil thickness of 0.15 mm for FH12-24S-0.5SH(55). Terminal apertures are 0.25 × 1.30 mm. The geometric volume per terminal is 0.04875 mm³ and the area ratio is 0.699 at 0.15 mm. An alternative process of 0.10 mm deposits nominally 0.03250 mm³, representing 33% less. The order requires a step of 0.15 mm for FPC. If the line process differs, qualification includes measurement of deposition via SPI, visual inspection of solder fillets, and connector stress testing. Verify the geometric clearance between stencil steps prior to cutting. [Official FH12 Catalog](https://www.hirose.com/en/product/p/CL0586-0521-0-55) · [Multi-step Stencil](https://jlcpcb.com/blog/step-stencil-design-complete-technical-guide)

The `stencil-step-zones-mm.dxf` file specifies the two thickness regions on different layers in millimeters, using the same origin as the paste Gerber file. The general sheet thickness is 0.10 mm. The DXF lines define the boundaries of thickness changes and remain outside the data for aperture perforation. Rectangular regions include adjacent components, so terminals of a component receive the same thickness. The CAM report measures the distance from each edge of the step to **all** active apertures and verifies the area ratio at the local foil thickness. For the cutting file, use the GTP apertures at 1:1 scale, with sheet in frame, electropolishing, and SPI control. [JLCPCB process for apertures and steps](https://jlcpcb.com/capabilities/pcb-stencil-manufacturing) · [Minimum distance to the edge of the step](https://jlcpcb.com/blog/step-stencil-design-complete-technical-guide)

Recommended distances for access during assembly, inspection, and rework depend on the pair of component packages. The boundary used for verification includes the body and terminal lands. Examples are 0.15 mm between two 0402 components, 0.18 mm for 0402–0603, 1.0 mm between a passive and QFN/BGA, and 1.5 mm between QFN and BGA. For families without a row in the JLC table, the report lists the closest part and the measured distance. [JLCPCB Measurement Matrix and Drawing](https://jlcpcb.com/help/article/minimum-spacing-for-smd-components)

## Stock and placement

`tools/cam_stock.py` queries the public assembly library from JLCPCB by part code C and compares the returned MPN exactly (case-insensitive), stock level, and available quantity for purchase in the private library. The standard check quantity is set for two prototypes. The quantity needed to feed the assembly line is estimated conservatively using `max(minimum placement quantity, parts required for all boards + max(fixed loss, ceil(parts required × volume loss fraction)))`. The registry maintains these three catalog fields separately. Results include the UTC timestamp, URL, SHA256 of the raw response, and the compressed JSON response. Actual reservation and pricing depend on the BOM association to the PCBA order. [JLCPCB Library](https://jlcpcb.com/parts) · [Minimum tape consumption during assembly](https://jlcpcb.com/help/article/common-bom-and-cpl-matching-issues-and-explanations)

`tools/cam_assembly.py` checks the alignment of references between the native source and BOM. For each part number C, it compares the center coordinates of distributor footprints with those of the project footprint. The CPL rotation is the sum of the EAGLE part rotation and the orientation correction derived from the comparison with the catalog footprint. CPL coordinates represent the center of the part on the PCB. Upon receipt of the production drawing, verify pin 1 keying, cathode orientation, FPC input, connector orientation, and the radiant end of the module. [BOM and CPL table format](https://jlcpcb.com/help/article/how-to-generate-the-bom-and-centroid-file-from-kicad) · [Orientation in JLCPCB preview](https://jlcpcb.com/help/article/pcb-assembly-faqs-part-2)

For L102, Coilcraft XGL4015-471MEC, part number C5452431, the JLC catalog lists the component without a publicly available footprint. JLC defines the zero position by band orientation. The Coilcraft drawing with sprocket holes at the top and tape feed to the right shows the "C" mark above the value, with pads aligned vertically. The annotated drawing identifies the shorted terminal by the bar adjacent to "C". In this orientation, the shorted terminal is the top one, at +Y. A +90° rotation places the shorted terminal on native land 1 at −X, connected to RT_SW1. CPL applies this correction prior to instance rotation. The assembly drawing indicates axis 1–2 with a line and the shorted terminal with a dot. `placement-vs-import.json` compares the coordinates and rotation of the source with the independent KiCad export. [Coilcraft drawings for body, band, and orientation](https://www.coilcraft.com/en-us/products/power/shielded-inductors/molded-inductor/xgl/xgl4015/) · [JLCPCB zero convention](https://jlcpcb.com/help/article/pcb-assembly-faqs-part-2)

`off-board-items.csv` lists the three components mounted separately, including part numbers and electrical interfaces. `probe-map.csv` summarizes top access to test contacts, effective copper exposure diameter, and distance to adjacent bodies. For the fixture, a test-pad diameter of 0.8 mm for signals, 1.0 mm for power and ground, a 0.5 mm clearance from bodies, a pitch of at least 1.27 mm, and a distance of 3.2 mm to the milled edge is verified. The list `astra.ipc` enables comparison or electrical testing of the blank board. [Test point design guide](https://jlcpcb.com/blog/pcb-test-points-and-smart-dft)

## CAM comparison and traceability

`tools/cam_export.py` imports the EAGLE board into KiCad 10.0.8, records the import report, and verifies geometry against manufacturer rules. The board used for CAM declares the thickness and finish of the order. Gerber X2 and Excellon use the same origin. PTH and NPTH files are distinct. Gerbv 2.13.0 opens these exports and generates views for copper, mask, solder paste, silk screen, outline, and drill. [KiCad CLI Documentation](https://docs.kicad.org/10.0/en/cli/cli.html) · [Gerbv](https://gerbv.github.io/)

`tools/cam_geometry.py` independently interprets Gerber primitives and polarity operations. From the copper of the two layers, drill holes are subtracted, islands are connected through plated walls, and the result is compared against contacts from the EAGLE source. Short circuits, opens, mismatches between drill and source, common mask openings, and stencil area ratio are identified. X2 net names are used separately to verify land coordinate accuracy. Arcs are approximated to a maximum of 0.8 µm. Images and numeric reports are regenerated for each revision of the PCB.

The hole positions and diameters are individually associated between design and the two Excellon lists. The decimal format uses a 1 µm grid and may round a native coordinate exactly at the midpoint of an interval to either adjacent neighbor. For traces, the axes and widths are compared on each net and layer. For contours, the Hausdorff distance and the area of the symmetric difference between the cutting axes are measured. The original KiCad descriptor includes both the bounding dimension and the line graphic width. In the delivered `.gbrjob`, the dimensions are those measured along the cutting axis and `ProjectId.Revision` is A. The field `TF.ProjectId` has revision A on each of the eight layers via the CAM copy. The original KiCad and the pre- and post-values along with their hashes are preserved in `verification/manufacturing/gerber-job-provenance.json`.

Import uses the stricter rules derived from the design and JLC limitations for trace width, spacing, holes, and copper-to-border distance. The power class maintains a trace width of 0.30 mm. DRC includes additional checks for trace centering on via and compatibility between the footprint type and terminals. KiCad retains three optional checks disabled in the imported project. The KiCad courtyard does not exist in the native EAGLE format and is replaced by measuring the board outline + land contours using the manufacturer's matrix. The KiCad symbol library filters and trace length matching profiles are not defined in this project. The raw DRC file preserves the list and all severity levels.

### Regenerating the files

From the project root, use Python 3.12, the packages listed in `tools/cam_requirements.txt`, KiCad CLI 10.0.8 and Gerbv 2.13.0. Set `KICAD_CLI` and `GERBV` to the executable paths. Run the commands in the order shown below. The final report returns an error code if any executable check is still outstanding. Physical prototype procedures are in `docs/qualification.md`.

```sh
python3 -m pip install -r tools/cam_requirements.txt
python3 tools/cam_stock.py --quantity 2
python3 tools/cam_export.py
python3 tools/cam_assembly.py
python3 tools/cam_dft.py
python3 tools/cam_receipt.py
```

## Manufacturing verification log

- In the first placement revision, two solder-mask openings at the regulator input merged. Another two openings were separated by only 0.060 mm. We moved the parts, repeated the export and repositioned the display MOSFET pin 1 marker. The final minimum measured silkscreen-to-mask clearance exceeded 0.22 mm.
- At the three fiducial points, the ground plane reached a distance of 0.028 mm from the mask opening. The clearance in copper was increased. The geometric comparison was repeated on the reverse mask.
- The check against the JLC assembly drawing found eight pairs of components too close together once their terminals were included. The comparator and its diode had 0.175 mm clearance against the recommended 0.40 mm. Repositioning preserved the switching loops and resolved all eight findings.
- The first BOM check showed four MCP6542T-I/MS comparators in stock. Two boards needed one each, but the assembly feeder required five parts. MCP6542-I/MS has the same circuit and package with a different shipping format. We checked C636338 and corrected the MPN in the design and BOM.
- The public catalog data for coil L102 omitted the orientation. The dimensional drawing was cross-referenced with the Coilcraft coil image and the JLC convention. A calculated correction of +90° was applied to CPL, and the assembly drawing shows the short end of the winding.
- On the first routed board, the CAM check found ground split into 30 groups and 10 thermal reliefs with a single spoke. After correcting the copper and adding return paths, nine isolated pads remained. Each physical group was compared against the schematic to identify the pads by name. An unused via on PV_MPP was removed.
- The inspection of packages without a specific row in the JLC matrix revealed a gap of only 0.025 mm between the nominal body of Q301 and the solder paste aperture of coil L301. The maximum body length of SOT-23, 3.04 mm, allowed for an overlap of 0.045 mm even with perfect positioning. L301 was displaced by 0.35 mm. At every export, the maximum bodies of Q301 and L301 are reverified against the paste of all other components. For mounting qualification, a positioning error of ±0.05 mm per axis has been added. Dimensions from Onsemi, page 7 · Dimensions from Bourns
- The third removable connection, R126, enables separate measurement of photovoltaic current. The file `measurement-links.csv` lists the nets on both sides and the coordinates for each of R124–R126. Normal assembly uses a 0 Ω resistor for each. Reassembly after modification includes reapplying width rules and verifying all networks.
