Files

T

shawn 0ae2ca6e8e feat: PCM1808+PCM5102 I2S HAT design files

Custom I2S HAT for Pi Multi-FX Pedal — full hardware package:

- KiCad project: schematic (kicad_sch), PCB layout (kicad_pcb), project file
- Custom DT overlay: pcm1808-pcm5102-overlay.dts (no upstream overlay exists for PCM1808)
- docs/hardware-bom.md: BOM (9.25 HAT + 1.75 with enclosure), wiring diagram, PCB design notes
- docs/config-audio.md: DT overlay build, ALSA config, JACK integration, troubleshooting
- scripts/install_hat.sh: One-command install + test suite (6 tests)
- hardware/gerber/: JLCPCB fab instructions and assembly notes

Circuit: Guitar input → TL072 preamp (gain ~20dB) → PCM1808 ADC → RPi I2S
  → PCM5102 DAC → RC filter → output jack
I2S: BCLK/GPIO18, LRCLK/GPIO19, DIN/GPIO20, DOUT/GPIO21
Stacking header passes all 40 GPIO pins for footswitches/LEDs/display

2026-06-07 23:52:13 -04:00

3.3 KiB

Raw Blame History

PCM1808+PCM5102 I2S HAT — JLCPCB Fabrication Package

This directory contains the fabrication files for the Pi Multi-FX Pedal I2S HAT. Board dimensions: 65×56mm, 2-layer, 1.6mm FR4 Target fab: JLCPCB (but compatible with any PCB fab)

Files

File	Description
`jlcpcb-bom.csv`	Bill of Materials for JLCPCB assembly
`jlcpcb-cpl.csv`	Component placement / centroid file
`fabrication-readme.md`	This file — fab notes and instructions

Gerber Generation

Gerber files must be exported from KiCad (not committed as generated binary files):

# Using KiCad 8.0 CLI:
kicad-cli pcb export gerbers \
  --layers "F.Cu,B.Cu,F.Paste,B.Paste,F.SilkS,B.SilkS,F.Mask,B.Mask,Edge.Cuts" \
  --output hardware/gerber/ \
  hardware/pi-multifx-hat.kicad_pcb

# Generate NC drill file:
kicad-cli pcb export drill \
  --output hardware/gerber/ \
  hardware/pi-multifx-hat.kicad_pcb

# Generate placement file for PCBA:
kicad-cli pcb export position \
  --format csv \
  --units mm \
  --output hardware/gerber/jlcpcb-cpl.csv \
  hardware/pi-multifx-hat.kicad_pcb

JLCPCB Order Specs

Parameter	Value
PCB Qty	5 (minimum)
PCB Layers	2
PCB Thickness	1.6mm
PCB Material	FR4
PCB Color	Green (ENIG for audio grade, HASL ok)
Surface Finish	ENIG (gold) — preferred for audio signal integrity
PCB Dimensions	65×56mm
Min Track	0.254mm (10mil)
Min Hole	0.3mm
Impedance	Not critical (audio frequencies)
PCBA	Top side only (bottom is GND pour)
RoHS	Yes

Design Notes for Fab

Edge plating: Request edge plating on mounting holes for EMI shielding (connect to GND)
Copper pour: GND flood fill both layers — no thermal relief needed on audio circuit
Via tenting: Tent all vias (prevents solder wicking during wave soldering)
Silkscreen reference designators: Use JEDEC standard ref des (U1-U4, C1-C10, R1-R6, J1-J3)
Mounting holes: 3.2mm non-plated through holes at 4 corners (standard 1590B footprint)
ENIG preferred over HASL: Lower noise floor for audio circuits

PCBA (Assembled Board) Parts

For JLCPCB assembly (PCBA service), the following parts must be in their extended/global parts catalog:

Part	JLCPCB Part?	Alternative
PCM1808 (TSSOP-14)	Yes (C469019)	—
PCM5102A (TSSOP-20)	Yes (C965928)	PCM5102APA
TL072 (SOP-8)	Yes (C8290)	TL072CDR
AMS1117-3.3 (SOT-223)	Yes (C6078)	—
0805 caps (100nF)	Yes (C52923)	—
0805 resistors	Yes	—

Components NOT in JLCPCB assembly catalog (must be hand-soldered or requested separately):

Electrolytic capacitors (10µF radial) — verify JLCPCB has SMD alternatives
6.35mm audio jacks (panel-mount)
2×20 female stacking header
M2.5 standoffs and screws

Case Fit

The PCB is 65×56mm, designed to fit a 1590B diecast aluminum enclosure (internal dimensions ~107×55×25mm usable). Mounting hole centers at 3.175mm from edges.

Test Points

Consider adding test points on next revision:

TP1: 3.3V rail
TP2: 5V rail
TP3: Preamp output (before DC blocking cap)
TP4: PCM1808 DOUT (verify I2S data with scope)

3.3 KiB Raw Blame History Unescape Escape