Skip to the content
2 layers60 × 64 mmBlueaudio puck, the printed circuit board in 3D

Turn wired headphones wireless: an ESP32 Bluetooth audio receiver (A2DP sink) with I2S DAC output, parametric EQ, AVRCP remote control and battery-aware power management. Built on ESP-IDF v5.5.

Size
60 × 64 mm
Copper layers
2
Thickness
1.6 mm
Parts
50
Nets
34
Pads
220
Tracks, vias
195, 60
Pours
2
Routed
Yes
KiCad
KiCad 10.0 (file 20260206)
Created
30 Aug 2026
Updated
31 Aug 2026

Overview

Blueaudio puck is an open-source printed circuit board by Zektopic, from the Zektopic/esp32-blue-audio-puck repository on GitHub, published under the MIT licence. It is a 2-layer board of 60 × 64 mm with 50 parts on 34 nets, routed with 195 tracks and 60 vias.

It is built around the ESP32-WROOM-32U, AP2112K-3.3 and LP2985-33DBV, with the PCM5102APW, MMBT3904 and BT3 among its other parts. Its parts include 18 capacitors, 9 resistors, 5 ICs, 5 connectors and 5 switches. It belongs with the audio and music and radio and wireless boards and the ESP32 boards of this library.

Main components

6

README

hardware/README.md

BlueAudio Puck carrier board, rev A

KiCad 10 schematic and PCB for a single-board version of the puck: ESP32-WROOM-32U, PCM5102A DAC, Li-po charging, two separate 3V3 rails, OLED header, three user buttons and a 3.5 mm output — 60 × 64 mm, drawn to JLCPCB's two-layer rules.

FileWhat it is
blueaudio-puck.kicad_proProject — open this
blueaudio-puck.kicad_schSchematic
blueaudio-puck.kicad_pcbBoard
bom.csvBill of materials
preview/SVG renders of both
scripts/The generator — see below

Read this before you order anything

[!CAUTION] Not finished: eight nets still need routing by hand.

Everything the generator lays is DRC-clean — zero clearance violations, zero shorts, zero hole-clearance errors under JLCPCB's rules. But 25 of 33 nets are routed, not 33, and the remaining eight are unconnected copper:

+3V3A · AUDIO_L · CC1 · CC2 · DAC_LDOO · DAC_VNEG · I2S_BCK · I2S_LRCK

All eight are around the two fine-pitch parts — the TSSOP-20 DAC and the USB-C receptacle. Open the board in Pcbnew and its interactive router will finish them far faster and better than the one in scripts/. Do not order anything until DRC reports zero unconnected items.

[!WARNING] Nothing here has been fabricated or tested. It passes ERC and the DRC checks that apply to an unrouted board. It has never been a physical object. Review the schematic against the datasheets before you spend money.

Verification

Actually run, with the output quoted rather than summarised:

text
$ kicad-cli sch erc --severity-error --severity-warning
Found 4 violations                    # all lib_symbol_mismatch, see below

$ kicad-cli pcb drc --severity-error --severity-warning
Found 25 violations
Found 22 unconnected items

The schematic is clean: zero electrical errors, no unconnected pins, no dangling labels, no malformed outline. All four ERC warnings are lib_symbol_mismatch on KiCad's derived symbols — the two regulators and the two transistors. Cosmetic; see below.

The board has no electrical errors either. Breaking the 25 down:

CountKindStatus
22unconnected_itemsMust fix — the eight unrouted nets
15silk_over_copperCosmetic; every fab ignores it
10silk_overlapCosmetic

No clearance, no shorting_items, no hole_clearance. That took three fixes to the router's geometry, each of which had produced copper that looked right and was not — they are written up in the file that makes them:

  • A track is not a point. A 0.4 mm power track centred on a 0.25 mm grid cell spills into its neighbours; checking only the cell it steps through let it sit 0.15 mm from a pad. Same for vias, which are 0.6 mm across — one landed on top of another net's track.
  • Clearance belongs in the check, not the map. Growing a clearance halo around every pad and checking a track's own clearance against it demanded the gap twice, which makes escaping a 0.65 mm pitch TSSOP impossible.
  • Holes are stricter than copper. Copper-to-hole is 0.25 mm where copper-to-copper is 0.15 mm, so drilled pads are claimed slightly larger than their copper.

The router still gets 25 of 33 nets rather than all of them. It routes in order and never rips up an earlier net to make room, which is the difference between it and a real autorouter.

The two ERC warnings are lib_symbol_mismatch on AP2112K-3.3 and LP2985-3.3. Both are KiCad derived symbols (extends), and the generator flattens them to embed them; the flattened copy differs cosmetically from the library's. Connectivity and pin numbering are unaffected. Eeschema's Update Symbols from Library clears it.

The silkscreen warnings are reference designators sitting over pads. Normal for auto-placed boards, ignored by every fab, and worth tidying only once placement is final.

How it is generated

Both files come from one netlist, in scripts/design.py.

That matters more than it sounds. A schematic and a PCB authored separately disagree about connectivity, and KiCad does not tell you until someone runs ERC and gets a wall of errors. One source, two emitters, no drift.

text
scripts/design.py         parts, nets, no-connects, board size  <- edit this
scripts/kisym.py          pulls symbols out of the KiCad libraries
scripts/check_sheet.py    catches stubs from different nets touching
scripts/gen_schematic.py  emits the .kicad_sch
scripts/gen_pcb.py        emits the .kicad_pcb (needs KiCad's python)

To regenerate:

bash
cd hardware/scripts
python design.py          # netlist self-check
python check_sheet.py     # no two nets touching
python gen_schematic.py
"C:/Users/manup/AppData/Local/Programs/KiCad/10.0/bin/python.exe" gen_pcb.py

gen_pcb.py needs KiCad's bundled interpreter — pcbnew lives only there.

Symbols and footprints are copied from the installed libraries rather than transcribed, so the output files are self-contained and open on a machine with no libraries configured. A hand-typed pin table is exactly the kind of error nothing but a human eye can catch.

Once you edit it by hand

The generators overwrite their outputs. Move the files out of hardware/, or stop regenerating, once you start editing in KiCad — which you will, because routing is the next step.

The design

text
USB-C ──> MCP73831 ──> Li-po ──┬──> AP2112K ──> +3V3  ──> ESP32, OLED, DAC digital
                               └──> LP2985  ──> +3V3A ──> DAC analogue

Two regulators from the cell, not one. The DAC's analogue rail gets its own low-noise LP2985 with a bypass capacitor. Sharing a rail with a Bluetooth radio is what makes a DAC hiss, and docs/hardware.md said so before this board existed.

No MCLK. The PCM5102A has SCK grounded and runs from its internal PLL, matching the hand-built prototype and what the firmware expects.

JP1 sits in series with I²S data on GPIO 2. That pin is a boot strapping pin, and a DAC loading it is why the prototype needs BOOT held to flash. Lift the jumper and the board flashes normally.

Battery sense is R7/R8, a 2:1 divider into GPIO 35, matching PUCK_BATTERY_DIVIDER_RATIO_X100=200.

Three user buttons on GPIO 32/33/27, matching the firmware — SW1 is BT1 (next / volume up), SW2 is BT2 (play-pause / pairing), SW3 is BT3 (previous / volume down). All active low straight to ground; the ESP32's internal pull-ups mean no external resistors. SW4 and SW5 are RESET and BOOT.

Note there is no LED on GPIO 27 on this board. The Kconfig help for PUCK_LED_GPIO suggests 27 for an external status LED, which would collide with BT3 on a breadboard. Here the only LED is D1, the charge indicator on CHG_STAT, so GPIO 27 is unambiguously BT3.

Where it departs from docs/hardware.md

Both departures are deliberate and both are rev B work:

No buck-boost. docs/hardware.md specifies a TPS63020 for efficiency — roughly 20–25% more runtime than an LDO. KiCad's standard library has no symbol for it, and inventing one is precisely the silent error this generator exists to avoid. Rev A uses LDOs and pays the efficiency.

No headphone amplifier. The PCM5102A is line level: audible on 32 Ω headphones but quiet, exactly as the docs warn. A TPA6132A2 is the rev B addition, and it is QFN-16 — it would make this board far harder to hand-build.

Manufacturing rules

Written into the project file, so DRC enforces them rather than leaving them as folklore. JLCPCB's standard two-layer process, with margin:

JLC minimumUsed here
Track width0.127 mm0.20 mm
Clearance0.127 mm0.15 mm
Via drill0.20 mm0.30 mm
Via diameterdrill + 0.260.60 mm
Annular ring0.13 mm0.15 mm
Hole to hole0.50 mm0.50 mm
Track to outline0.20 mm0.50 mm

Only clearance sits near a limit, and it is still 18% above JLC's floor. The 0.05 mm it frees up per side compared with KiCad's 0.2 mm default is most of what lets the congested area route at all.

Teardrops are configured but not generated. The parameters are in the project file; KiCad adds the actual teardrops on demand. Run Edit → Teardrops → Add Teardrops in Pcbnew once routing is finished — doing it before then would only have to be redone.

What is left to do

  1. Route the last eight nets in Pcbnew: +3V3A, AUDIO_L, CC1, CC2, DAC_LDOO, DAC_VNEG, I2S_BCK, I2S_LRCK. All are around the TSSOP-20 DAC and the USB-C part. The interactive router will do this in minutes.
  2. Add teardrops once routing is done.
  3. Check the antenna keep-out. The WROOM-32U has an external connector so there is no PCB antenna to clear, but leave the module's edge unpoured.
  4. Re-run DRC and get it to zero before ordering anything.
  5. Review against datasheets. Especially the MCP73831 programming resistor (R5 = 2 kΩ, about 500 mA) against your cell's charge rate.
  6. Rounded corners were dropped — arcs whose endpoints did not meet left the outline open, and KiCad will not guess. Add them in Pcbnew, where the editor keeps the ends joined.

Parts

50
QtyValueFootprintReferences
6100nC_0805_2012MetricC1, C4, C5, C7, C10, C18
61uC_0805_2012MetricC3, C8, C9, C11, C13, C15
4H1, H2, H3, H4
410uC_0805_2012MetricC2, C6, C14, C16
310kR_0805_2012MetricR1, R2, R9
2100kR_0805_2012MetricR7, R8
25k1R_0805_2012MetricR3, R4
2MMBT3904SOT-23Q1, Q2
10RR_0805_2012MetricJP1
110nC_0805_2012MetricC17
11kR_0805_2012MetricR6
12kR_0805_2012MetricR5
13.5mmJack_3.5mm_CUI_SJ1-3513N_HorizontalJ2
14u7C_0805_2012MetricC12
1AP2112K-3.3SOT-23-5U4
1BATTJST_PH_S2B-PH-K_1x02_P2.00mm_HorizontalJ4
1BOOTPanasonic_EVQPUJ_EVQPUASW5
1BT1Panasonic_EVQPUJ_EVQPUASW1
1BT2Panasonic_EVQPUJ_EVQPUASW2
1BT3Panasonic_EVQPUJ_EVQPUASW3
1CHGLED_0805_2012MetricD1
1ESP32-WROOM-32UESP32-WROOM-32UU1
1LP2985-3.3SOT-23-5U5
1MCP73831-2-OTSOT-23-5U3
1OLEDPinHeader_1x04_P2.54mm_VerticalJ3
1PCM5102ATSSOP-20_4.4x6.5mm_P0.65mmU2
1PROGPinHeader_1x06_P2.54mm_VerticalJ5
1RESETPanasonic_EVQPUJ_EVQPUASW4
1USB-CUSB_C_Receptacle_HRO_TYPE-C-31-M-12J1

Similar boards

  • 4 layers31.8 × 37.3 mmRaven hardware, the printed circuit board in 3D

    Raven hardware

    merrittlj/raven-hardware

    A minimalistic smartwatch's hardware.

    83 parts1GPL-3.0
  • 2 layers45 × 99.5 mmRainbow2-rp2040, the printed circuit board in 3D

    Rainbow2-rp2040

    taka-tuos/iidx_pcb

    Open-Source Beatmania Controller PCBs

    21 parts3GPL-3.0
  • 4 layers80 × 54 mmPoket, the printed circuit board in 3D

    Poket

    kaorii-ako/Poket

    ESP32-S3 Bluetooth MP3 player - custom PCB + 3D-printed case, built from scratch

    104 parts
  • 2 layers230 × 160 mmAntcontroller, the printed circuit board in 3D

    Antcontroller

    cr1tbit/antcontroller

    402 parts1
  • 2 layers39.1 × 68.9 mmBaseChipOnly, the printed circuit board in 3D

    BaseChipOnly

    ZonatedCord/Yggdrasill

    Smart LED plant pot — ESP32 PCB, WS2812B/SK6812 LEDs, WLED firmware, modular 3D-printed vase, and a native iOS app with Apple's Liquid Glass design.

    34 parts1
  • 2 layers129.6 × 89.8 mmPowerMeter REV36, the printed circuit board in 3D

    PowerMeter REV36

    dj1yr/LJ-RF-Powermeter-Teensy-4.1

    Here is a collection of files for the RF Powermeter with Teensy 4.0/4.1. Since I could not find any source files for the PCB, I designed two boards based on Robert Entwistle (WA2T) and the really impressive software by…

    75 parts
  • 2 layers43.9 × 44.5 mmDisplay, the printed circuit board in 3D

    Display

    bullestock/acsv2

    Rewrite of Access Control System in Django

    17 parts2GPL-3.0
  • 2 layers69 × 58.7 mmRemote, the printed circuit board in 3D

    Remote

    bullestock/remote

    40 parts1

Questions

How big is the Blueaudio puck PCB?

It measures 60 × 64 mm and has 2 copper layers, 1.6 mm thick.

What parts does the Blueaudio puck use?

50 parts, built around the ESP32-WROOM-32U, AP2112K-3.3, LP2985-33DBV and PCM5102APW. The full list of its parts is on this page, with links to each part's symbol and footprint where PCBKit's library has them.

Where can I download the Blueaudio puck KiCad files?

From the Zektopic/esp32-blue-audio-puck repository on GitHub, at the commit this page was made from: the board is hardware/blueaudio-puck.kicad_pcb and its schematic hardware/blueaudio-puck.kicad_sch. PCBKit opens the board in the browser, with nothing to install.

Can I use the Blueaudio puck design in my own project?

Its repository publishes it under the MIT licence: you may reuse it on that licence's terms (keep the author's notice, and for a copyleft licence share your changes alike).