Skip to content

AW93x05 library acceptance

Checked 2026-10-25 against awinic AW93105 V1.3 (March 2022), AW93205 V1.2 (July 2025), AW933xx V1.8 (May 2025), and the common Hardware Design Guide V1.3 (June 2024). The accepted parts are AW93105DNR, AW93205DNR and AW93305DNR. The BFOR packages are excluded. Package compatibility does not establish software compatibility or sensing performance with ESPurr electrodes/fur.

Installed assets

  • Standalone breakout: AW93x05:AW93105DNR and AW93x05:DFN-10_1.8x2.1mm_P0.4mm_AW93x05, using project-relative library tables.
  • ESPurr shared symbols: Symbols:AW93105DNR, Symbols:AW93205DNR, Symbols:AW93305DNR in espurr/symbols.kicad_sym (relative to the repo root). Each has a default footprint of Footprints:DFN-10_1.8x2.1mm_P0.4mm_AW93x05 in espurr/footprints.pretty. Existing parent/ear/band project library tables already expose those shared libraries. No sensing IC was added to the ear or headband designs.
  • The two footprint files are identical. No generic DFN substitution, hidden exposed pad, importer model, or unverified 3D body is used.

The symbol/footprint were authored through Konnect in a disposable build/library-trials/aw93x05 project, queried back, placed and rendered before promotion. All three shared symbols were subsequently placed in build/library-trials/aw93x05-shared, with their default footprint resolved. The shared default fields were set through the native KiCad Symbol Editor, because Konnect's library creator has no default-footprint/property setter. KiCad serialised the shared library in its native KiCad 10 format.

Physical pin map

Top/component view, pin 1 upper left. The actual drawing has body X = 1.80 mm, Y = 2.10 mm, nominal height 0.55 mm. The ordering-table string “2.1 × 1.8” is not an instruction to rotate the footprint's body axes. All ten pads are on F.Cu/F.Paste/F.Mask; there is no exposed pad.

Symbol pin = PCB pad Function Local pad centre X, Y (mm) Land size X × Y (mm)
1 SCL −0.675, −0.800 0.650 × 0.200
2 SDA −0.675, −0.400 0.650 × 0.200
3 CS2 −0.675, 0.000 0.650 × 0.200
4 VCC −0.675, +0.400 0.650 × 0.200
5 GND −0.675, +0.800 0.650 × 0.200
6 CS1 +0.675, +0.800 0.650 × 0.200
7 CS0 +0.675, +0.400 0.650 × 0.200
8 CS3 +0.675, 0.000 0.650 × 0.200
9 CS4 +0.675, −0.400 0.650 × 0.200
10 INTN +0.675, −0.800 0.650 × 0.200

The drawing's 2.00 REF is the outside copper envelope, not centre spacing. Centres are 1.350 mm apart. Row pitch is 0.400 mm. Pad 1 is rectangular; other pads have 0.15 round-rectangle ratio, preserving the specified envelope and centres. Courtyard bounds are X ±1.25 mm, Y ±1.30 mm. The Fab body has a pin-1 chamfer and silk has a pin-1 dot. U1 is front, 0°; its pin-1 pad is upper left in CAD, Gerbers and the placement preview. Supplier rotation remains a separate assembly-preview check.

Evidence and limits

Manufacturer pin drawings: AW93105 p.3, AW93205 p.3, AW933xx p.9. Land patterns: AW93105 p.22, AW93205 p.25, AW933xx DNR p.44. Common guide pp.7/10/13 show the same reference wiring; pp.18–21 give layout guidance. Native saved-board readback checks all ten U1 pad numbers, positions, sizes and nets, including the easily confused CS0=7 / CS1=6 / CS2=3 mapping. The PCB has 43 physical component pins; their net assignments are checked against the KiCad CLI XML netlist.

The breakout's schematic-to-PCB import initially omitted net-tie metadata and custom fields. A Konnect library refresh refused the jumper's zone_connect attribute. After a verified save and clean close, the repository-authorised native pcbnew fallback restored complete library footprints, pad identities, nets, symbol fields and manual/copper placement exclusions. The saved result was read back and checked using KiCad CLI ERC/DRC with schematic parity. JP1's copper bridge, net-tie group and allowed solder-mask bridge are preserved; it has no paste.

The local source PDFs remain outside tracked source:

  • ~/Downloads/DG_AW9310x&AW9320x&AW933xx_Hardware_Design_Guide_EN_V1.3.pdf
  • ~/Downloads/DS_AW93205_EN_V1.2.pdf
  • Official AW93105/AW933xx PDFs and rendered comparison pages under build/sensor-research/.

The design project contains schematic/PCB objects created from manufacturer dimensional facts, not redistributed manufacturer PDF drawings. Standard passives, headers and jumper reference the installed KiCad libraries. The custom IC footprint has no 3D model. Physical assembly, supplier DFM and electrode performance remain unverified; see the prototype README.