WavetableController

PCB Analysis — WavetableController (Daisy Seed synth)

Read this first. This folder holds a completed design review of Trey's "WavetableController" board — an Electrosmith Daisy Seed–based wavetable synth controller, 2-layer, 165×102 mm, designed in KiCad 9. The board has been fabbed twice at JLCPCB and the physical boards mostly work. The analysis (all passes complete, 2026-08-13) found several real defects and produced a rev-2 plan.

If you are Claude opening this fresh: the authoritative output is analysis/FINAL_REPORT.md (tiered red flags + open questions for Trey), backed by the full findings ledger F-001…F-035 in analysis/FINDINGS.md. Do not re-derive anything before checking those. Methodology and which-file-is-truth rules are in analysis/SOURCE_OF_TRUTH.md.

Folder contents

Critical provenance warning

Trey sent files reluctantly and in stages: Gerbers+BOM first, then .pro/.sch, then the .kicad_pcb last. File mtimes are transfer times, not edit times. The .kicad_pcb in this folder matches the LedFix Gerbers ~97% but contains NO GND pour (only 5 keepout zones), while the fabbed B.Cu Gerber has a 164×100 mm filled pour covering 44/63 GND pads. It is a stale/wrong version — never regenerate Gerbers from this copy. Standing ask: get Trey's real working .kicad_pcb (the one that shows a filled B.Cu pour when opened). Where sch and pcb disagree (e.g. LED2 wiring), the pcb matches the fabbed boards, so the schematic is the outlier.

Headline findings (details + evidence in analysis/)

• Encoder push-buttons dead — ENCL_CLICK / ENCR_CLICK have zero copper in the Gerbers (floating inputs; ENCR lands on a 3.3V-only Daisy pin). Fab-confirmed.
• RGB LEDs triple-broken — LED1/LED2 (CLS6B-FKW) are unplaced (missing from BOM, though the paste stencil expects them), reverse-biased via 300Ω to +9V_FILT (never light either polarity), and three LED pins sit on Daisy's 3.3V-only pins 24/25/30.
• I2C has zero pull-ups in-design — the ~203 mm bus relies entirely on the OLED module's onboard pull-ups (open question F-027 for Trey).
• Duplicate refdes R21 — a layout-only 300Ω footprint at (170.1, 84.8) bridges /OLED_HOT–/+3V3_D in parallel with FB4 (Trey's noise-debug hack, on physical boards, not in schematic). Pick-and-place would put 300Ω where the 10Ω OLED damper belongs; breaks BOM/CPL matching.
• 0.1 mm traces board-wide — exactly AT JLCPCB's 2-layer 1oz minimum (not below it), zero margin; carries the +3V3_D rail, I2C, SD, MIDI, USB. Recommend 0.2–0.25 mm. DRC min_track_width is 0.0 in the .kicad_pro, so KiCad won't flag them.
• BOM refdes mismatch — BOM's S1/S2 don't exist in the schematic (real refs are TAC_SWITCH_1/2, TAC_SHIFT_L1/R1 — note: underscore refs escape [A-Z]+[0-9]+ regexes).
• 3 marginal fab violations (MK1 annular ring, P2 NPTH clearance, SW1 edge copper — the last is a deliberate notch, accepted). Power design: USB-C is data-only by design; 9V barrel → Schottky bridge → +9V_FILT (~8.3V).

Open questions blocked on Trey: F-014 (LED2 sch-vs-pcb, which is intended), F-027 (OLED module pull-up value), and the real .kicad_pcb with the GND pour.

Rev-2 screen work (planning only, no design files changed)

analysis/REV2_OLED_PLAN.md: replace the two HiLetgo SSD1309 modules (boost-coil whine) with bare COG panels on 0.5 mm ZIF, independent I2C addresses 0x3C/0x3D. Two candidate panels:

• Mono: Crystalfontz CFAL12864G-024W (2.4", SSD1309) — needs 12.5–13.5V VCC, so a 15V adapter + ~13V LDO. Mounting solved in screen mounting solution.md.
• Greyscale (user's preference): no 2.42" greyscale panel exists anywhere. Best match is Raystar REX012864U / Winstar WEO012864U — 2.7" SSD1357, 16-level grey, VCC 8–10.5V (12V adapter + 10V LDO). Unresolved geometry flag: two 73 mm glasses = 146 mm side-by-side and conflict with the x≈165–200 audio-corridor keep-out. Fallback: stay mono, or 1.54" SSD1327.

Board changes either way: add 2.2k I2C pull-ups, remove J2/FB4/C14/C17/both R21s, use Daisy spare pads 22 & 28 for RES# and VCC_EN sequencing.

Tooling notes

• KiCad 9.0.9 (Linux / Claude Code on the web): kicad-cli and the pcbnew Python module are on PATH. .claude/hooks/session-start.sh (a SessionStart hook) runs tools/kicad_env_setup.sh automatically in web sessions; run it by hand with sudo tools/kicad_env_setup.sh elsewhere. It installs the stock symbol/footprint libs and seed the user library tables (otherwise ERC/DRC add ~190 "library not found" warnings). tools/kicad_check.sh runs ERC, DRC, netlist, Gerber, SVG and PDF exports into kicad_out/ (git-ignored) as a smoke test.
• Freerouting 2.4.1 autorouter is installed by the same setup script (needs Java 25, installed alongside the system Java 21; freerouting wrapper on PATH runs it headless with analytics off). tools/autoroute.py IN.kicad_pcb OUT.kicad_pcb [--passes N] does DSN export → route → SES import. It temporarily renames the duplicate R21, because the Specctra exporter refuses boards with duplicate refdes (an independent confirmation of that finding). On the stale checked-in board, 2 passes took 53 unrouted connections to 5. Remaining lib warnings name Trey's private libs (Retroactive_Custom_Parts, Jack_3.5mm_CUI_RetroactiveCustom, SOP-6_...(RetroactiveCustom)), which only exist on his machine; footprints are embedded in the .kicad_pcb, so they are harmless. Note pcbnew.LoadBoard(...).Zones() returns 0 here because the 6 keepout zones live inside footprints, not at board level.
• On Trey's Mac, KiCad 10.0.5 lives at /Applications/KiCad.app (kicad-cli at Contents/MacOS/kicad-cli; brew cask fails without sudo).
• analysis/gerber_analyze.py is the Gerber parser/net-matcher that produced the routing CSVs. Other scratch scripts (pcb_parse.py, pcb_audit.py, DRC/ERC reports) lived in a session scratchpad and may be gone — regenerate from gerber_analyze.py patterns if needed.
• Net names in the routing CSVs are geometrically inferred (anchored at Daisy pins, 6/6 validated on LED nets), not authoritative; island_* = unidentified copper.