GnW-Zelda-MicroSD

A castellated-edge microSD interposer for the Game & Watch: The Legend of Zelda console mod scene -- built as original KiCad artwork, informed by existing community Gerber-only releases rather than copied from any of them.

The board mates directly to the console's STM32 mainboard via a 7-position castellated edge (real 0.3x1.2mm SMD pad geometry, machined flush by the board-edge mill -- this is the critical mechanical/electrical mating surface, not an approximation) and carries an onboard RT9193-28GB LDO regulating the console's raw ~4.2V battery rail down to a safe 2.8V for the microSD card.

This is a flex PCB, not rigid: 2-layer, 1oz copper both sides on a 2mil (50.8um) polyimide core, 0.1408mm total board thickness.

Status

Working draft, not yet fab-verified on real hardware. Electrically clean (0 unconnected nets, 0 shorts per kicad-cli pcb drc) with real routing and filled ground pours on both copper layers. Remaining DRC output is DFM-grade (clearances, drill sizes, silk overlap) -- normal manual-review territory before ordering boards, not electrical faults. See docs/design-notes.md for the full derivation, findings, and everything still worth double-checking by hand in the KiCad GUI before fabrication.

Commit history

• Initial commit -- the original reconstruction: schematic, PCB, footprints, and silkscreen rebuilt from scratch in KiCad from measured Gerber geometry (see Origin and attribution below). No third-party KiCad source files were used at this point -- every footprint was RE'd/approximated by hand from pad positions and sizes read off the Gerbers.
• This commit -- incorporates real assets from PrimoAngelo's native KiCad source (added as source material in the prior commit) now that he's confirmed as the known-good original author: J2 (microSD socket) and J3 (VBAT tab) were swapped from their RE'd/approximated footprints to his real MSD1A/Pad_1x1_5 pad geometry, and a real STEP model was wired into U1 (RT9193 LDO). C1/C2/R1 now carry a second, real hand-solder-0805 footprint stacked at the same location as their original passive footprint, so either package size can be assembled. Also fixed a schematic/PCB reference-designator mismatch (J2/J3 and U1/U2 were swapped between the two files) and a batch of inconsistent net names left over from re-syncing the PCB against the schematic.

Repository layout

hardware/         KiCad project (open GnW-Zelda-MicroSD.kicad_pro here)
production/       Gerbers + drill files (RS-274X, Excellon) + a zipped bundle
docs/             Design notes, top/bottom copper + 3D renders
source-material/  Original third-party source files this design descends
                   from, preserved for attribution/licence compliance --
                   see source-material/README.md
LICENSE           CERN-OHL-S v2 full text
NOTICE.md         Licensing rationale and attribution summary

Circuit

• U1 -- RT9193-28GB LDO. VIN <- raw battery (~4.2V) via the J1 castellated edge; EN <- console GPIO (via J1); VOUT -> 2.8V microSD supply.
• J2 -- microSD socket (SPI-mode wiring: CS/MOSI/MISO/CLK + VDD/GND), PrimoAngelo's real MSD1A footprint.
• J1 -- 7-position castellated edge: GND, CS, MISO, CLK, MOSI, NC (spare), EN.
• J3 -- castellated VBAT solder tab, PrimoAngelo's real Pad_1x1_5 footprint (same machined-edge technique as J1) -- solders directly to the positive terminal of an external SMD capacitor.
• R1 -- 100k pulldown holding the LDO disabled by default until the console GPIO actively enables it. Real hand-solder-0805 footprint stacked at the same location as the original RE'd footprint.
• C1/C2 -- input/output decoupling for U1. Same dual-footprint stacking as R1 (0805 hand-solder on top of the original).
• H1-H4 -- plated, electrically-isolated mounting pads (3.0mm pad / 1.8mm drill), positioned to match the reference designs' mounting pattern.

Origin and attribution

This design was reconstructed from precise geometry (board outline, pad positions/sizes, net connectivity, and real copper routing) extracted directly from Gerber-only community releases for the same G&W Zelda microSD mod, tracing back through three generations of prior work:

• Tim Schuerewegen originated the project.
• Hundshamer picked it up and pushed it forward to its final form, GNW-MICROSDx1-ZELDA-V3.4. Used during reconstruction for cross-validation (confirmed identical castellated pinout via a different edge-connector pin-numbering scheme than PrimoAngelo's release) and as the source for the drilled-via castellation technique referenced during development.
• PrimoAngelo began his own work from Hundshamer's v3.4 design, producing MicroSD_Zelda_FORO_JLC_FIX_V2 - NO_LOGO, credited to him in its own back-silkscreen (visible in the source Gerbers). This is the primary geometric basis for this repo's outline, placement, and routing.

Everything in this repository (schematic, PCB, footprints, silkscreen) was rebuilt from scratch in KiCad from measured geometry, not copied. This reconstruction was completed before any contact with any of the above. Afterward, both PrimoAngelo and Hundshamer were reached directly: PrimoAngelo confirmed authorship and provided native KiCad source for this design and a sibling Mario board; Hundshamer confirmed the lineage back to Schuerewegen's original project in a friendly exchange, but had no additional source material to contribute beyond what was already used above. All original source material received is preserved under source-material/ for full provenance and CERN-OHL-S v2 compliance; see source-material/README.md for the complete attribution chain and NOTICE.md for the licensing rationale. Full credit to the original designers for the mod itself; if you're one of them and want anything here changed or removed, open an issue.

License

CERN-OHL-S v2 (CERN Open Hardware Licence Version 2 - Strongly Reciprocal). See LICENSE and NOTICE.md.

Building / opening

Requires KiCad 10. Open hardware/GnW-Zelda-MicroSD.kicad_pro.

Most custom parts (castellated connectors, exact-geometry footprints for the LDO/passives) are embedded directly in the .kicad_pcb. J2 and J3 now use real footprints from PrimoAngelo's native library, referenced via project-scoped libraries in hardware/fp-lib-table that point into source-material/ with ${KIPRJMOD}-relative paths -- so the project stays portable to any clone location, but source-material/ must come along with it. The schematic symbol library (hardware/gnw_zelda_microsd.kicad_sym) is referenced the same way.

Before ordering boards

• This is a hand-routed/reconstructed draft -- give it a real pass in the KiCad GUI (visual DRC review, silk/courtyard cleanup) before sending to a fab.
• The castellated edge geometry is the one dimension that matters most: verify pad pitch/size against your actual console board before committing to a fab run.
• No BOM/pick-and-place export included yet -- add before ordering assembly.