Library acceptance and provenance¶
Manufacturer: Gettop Acoustic. Exact MPN: MD-DRA371-H10. LCSC: C50275760.
Manufacturer PDF MDDRA371H10.pdf, retrieved 2026-10-16 from
https://en.gettopacoustic.com/Public/Uploads/uploadfile/files/20250817/MDDRA371H10.pdf.
The 16-page PDF has no visible revision identifier on the mechanical/land-pattern
pages; do not infer a document revision from its URL date.
Symbol: MD_DRA371:MD-DRA371-H10.
Footprint: MD_DRA371:MD-DRA371-H10_3x4mm.
Origin: physical body centre, with the 3 mm width along X, 4 mm length along Y.
At 0 degrees on F.Cu, the component's top marking and pin-1 dot are upright,
with pin 1 at upper left. Page 8 is a bottom view: mirror its X coordinates
to obtain this board's component-side view. Page 13's land pattern has its port
above the four signal lands; rotate that drawing 180 degrees to align it here.
| Datasheet lead | Function | Symbol pin / type | Footprint pad and local centre, mm | Evidence/view |
|---|---|---|---|---|
| 1 | CLK | 1 / input | 1: (-0.85, -1.50), 0.70 x 0.40 | p8 bottom-view upper-right becomes top-view upper-left |
| 2 | L/R | 2 / input | 2: (-0.85, -0.80), 0.70 x 0.40 | p8 bottom-view right second row becomes top-view left |
| 3 | GND | 3 / power_in | 3: annulus centred (0, +0.68), OD2.00 / ID1.20 | p8 bottom annulus; p13 land pattern |
| 4 | VDD | 4 / power_in | 4: (+0.85, -0.80), 0.70 x 0.40 | p8 bottom-view left second row becomes top-view right |
| 5 | DATA | 5 / tri_state | 5: (+0.85, -1.50), 0.70 x 0.40 | p8 bottom-view upper-left becomes top-view upper-right |
| Mechanical | Acoustic PCB opening | Absent from symbol | unnumbered NPTH (0, +0.68), drill 0.80 | p13 specifies NPTH 0.7-0.9 |
Counts reconcile: five physical electrical lands, five symbol pins, five electrical footprint pads and one mechanical NPTH. No duplicate numbered pads. The custom pad-3 anchor is at (+0.80, +0.68) on the annulus; its circle primitive is offset -0.80 in X, so the acoustic centre remains (0, +0.68). This anchor offset must not be mistaken for the component placement origin.
Pad 3 is native custom-pad copper only. A separate circular F.Mask annulus opens OD2.00/ID1.20. Three F.Paste polygons have those same radii and 0.14 mm parallel-sided radial webs at -90, +30 and +150 degrees. Curves in stencil polygons use 60 segments per arc (maximum chord error below 0.00015 mm). The NPTH itself has no mask/paste opening primitive. Its clear centre has no silkscreen, copper or vias. A local DRC rule allows the manufacturer-mandated 0.20 mm radial NPTH-to-seal clearance; other holes retain 0.25 mm minimum.
The symbol and footprint were queried back through Konnect and inspected in a disposable project before use. Final native pad primitives, net assignments, dimensions, hole and exports are checked again by the release inspector and KiCad ERC/DRC. CLK/DATA run on F.Cu above the connected rear ground pour; the compact revision-2 routing has short supply/SEL crossings in that reference. C1-to-U1 paths are both on F.Cu with no vias.
EasyEDA trial¶
easyeda2kicad 1.0.1 (uPesy upstream, PyPI) successfully imported the real
C50275760 symbol, footprint and SVGs into ignored build/library-trials/.
The importer required an absolute output path with --project-relative; its
relative-path failure and successful retry are recorded in the build logs.
KiCad 10's fp upgrade accepted the imported legacy module.
The imported footprint was named
MIC-SMD_5P-L4.0-W3.0-P0.90_MD-DRA361-P10-1. It used four custom segments
numbered 6, a 0.6 mm plated acoustic hole, and a displaced origin. It
was rejected rather than promoted. The reviewed source library was built from
the exact manufacturer's drawing. Konnect was used for the schematic, initial
library, placement/routing and checks; native KiCad 10 pcbnew objects completed
the exact annular pad, metadata, reference fields and rear-text mirroring after
the source board was saved and the editor closed. No schematic/PCB text
replacement or existing shared-library changes were used.
The installed Steffen-W impartGUI importer was located; the uPesy 1.0.1 CLI was selected because the real import worked. The source project has no runtime dependency on the importer or online library retrieval.
Channel solder jumper (revision 2)¶
JP1 uses KiCad 10's standard Jumper:SolderJumper_3_Open symbol and
Jumper:SolderJumper-3_P1.3mm_Open_RoundedPad1.0x1.5mm footprint. Both were
queried through Konnect before use. This is PCB copper rather than an orderable
component; it has no MPN/LCSC requirement. In the front/component view, pad 1
is left at (-1.3,0), pad 2 is centre at (0,0), and pad 3 is right at (+1.3,0).
The end pads use rounded custom geometry; pad 2 is 1.0 x 1.5mm. All are on
F.Cu/F.Mask only, with 0.25mm pad-to-pad gaps and no F.Paste. The nearby GND
pour keeps the project minimum 0.20mm clearance from the centre pad. Connections are
1=GND/L, 2=SEL, 3=VDD/R. Three symbol pins and three electrical pads reconcile;
there are no duplicate pads or mechanical holes. The saved placement, netlist
and rendered exports are checked again after layout.
Both bridges remain open in the manufactured PCB. R1 supplies the default low
selection. One manual solder bridge hard-selects low or high; bridging both
sides shorts the supply. JP1 is excluded from placement files and the generated
assembly BOM/CPL by Assembly=Copper; it does not add a purchased SMT part.