Skip to the content
2 layers25.6 × 15.8 mmBus tap, the printed circuit board in 3D

Reverse-engineering an Urmet Bibus VOP intercom to bridge it into Home Assistant

Size
25.6 × 15.8 mm
Copper layers
2
Thickness
1.6 mm
Parts
25
Nets
17
Pads
67
Tracks, vias
96, 77
Pours
1
Routed
Yes
KiCad
KiCad 10.0 (file 20260206)
Created
14 Sep 2026
Updated
14 Sep 2026

Overview

Bus tap is an open-source printed circuit board by Cptmeme, from the Cptmeme/Urmet-Bibus-intercom-tap repository on GitHub, published under the GPL-3.0 licence. It is a 2-layer board of 25.6 × 15.8 mm with 25 parts on 17 nets, routed with 96 tracks and 77 vias.

It is built around the MCP6004-E/P and BAT54S. Its parts include 11 resistors, 7 capacitors, 3 connectors, 2 diodes and 1 IC. It belongs with the ESP32 boards of this library.

Main components

2

README

bus_tap/README.md

Urmet Bibus VOP — L1/L2 + C1/C2 analog tap

Front end that lets an ESP32 act as the oscilloscope we don't have, so we can measure the modulation depth and bit timing on the Urmet door-phone bus.

Target hardware: Urmet Bibus 2nd Ed. VOP, Artico monitor Ref. 1705/1 on bracket Ref. 1705/954. Manual in ../docs/.

Wiring

Intercom side

BoardIntercom terminalNote
J1-1L1bus positive (22.5 V idle as measured)
J1-2L2becomes board GND
J2-1C1floor call
J2-2C2floor call

Leave VPI / VPU alone. They carry the monitor's operating power (700 mA, 16–18.5 Vdc), not just video.

ESP32 side — J3

J3ESP32 (classic DevKit)Signal
13V3supply for U1
2GND= bus L2
3GPIO34ADC_DC — channel A, absolute bus voltage
4GPIO35ADC_AC — channel B, AC-coupled ×11
5GPIO36 (VP)ADC_FC — channel C, floor call

Use ADC1 pins only. ADC2 is unusable while Wi-Fi is on, and we need Wi-Fi (see safety note below). GPIO34/35/36 are input-only, which suits analog.

Channels

  • A — absolute. R1/R2 divide by 11, U1A buffers, R3/C1 anti-alias at ~16 kHz. Window 0–34 V, so 22.5 V idle sits at 2.05 V. Shows big dips and the DC level.
  • B — AC-coupled, gain 11. C2 blocks DC, R4/R5 re-bias to 1.65 V, U1B gains ×11. Net effect: 1 V of bus swing = 1 V at the ADC, centred on 1.65 V, ±1.5 V before clipping, 3.2 Hz high-pass. This is the channel that will show small modulation and edges that channel A buries in quantisation noise.
  • C — floor call. Same divider + buffer on C1/C2.

MCP6004 is CMOS (~1 pA bias), so the 1 MΩ divider costs ~1 µV of offset. Do not substitute a bipolar op-amp such as LM324 — it is neither rail-to-rail nor happy at 3.3 V, and its bias current would swamp the divider.

Connector notes

There is no separate external GND. Board GND is bus L2 - it arrives on J1-2 and leaves on J3-2 to the ESP32. Do not add a dedicated ground pin; the one thing this board must not have is two references.

Mis-plugging is harmless: both bus channels use identical 1M/100k front ends, so swapping the L1/L2 and C1/C2 headers does nothing bad, and reversing L1/L2 polarity merely pins channel A at zero (D1 clamps at -0.3 V, the 1 M holds current to ~22 uA).

The one real risk is a wire that works loose and dangles behind the intercom, where it could bridge L1 to L2. A disconnected tap is harmless - it is passive and high-impedance, you just lose data - but a flapping conductor on a shared bus is not. Use short leads with heat-shrink strain relief, or fit keyed/latching connectors (JST-XH is 2.54 mm pitch, polarised, and JLC-stocked) if you want it fit-and-forget.

Safety

  1. This tap is NOT isolated — board GND is bus L2. Power the ESP32 from an isolated USB wall wart and get data off over Wi-Fi/UDP. Never plug the laptop's USB in while J1 is connected to the bus; that would tie the building's bus rail to your laptop's ground.
  2. Bus loading: 22.5 V / 1.1 MΩ ≈ 20 µA. The manual specs the whole monitor's standby draw on L1/L2 as 1.6 mA max, so this tap is ~1.3% of it. This is why the PC817 opto board must not go here — at 3.3 kΩ it would draw 5.9 mA, ~3.7× the entire monitor.
  3. JP1 links C2 to board GND. Fit it only after confirming with a multimeter that the C1/C2 loop shares a reference with L2. If that loop floats, leave JP1 open and sense C1/C2 with the separate opto board — C1/C2 is local to this monitor only, so nothing there can affect neighbours.

JLCPCB part status

Checked against JLCPCB's Economic Parts list (Basic + Preferred Extended = $0 feeder fee). Everything below is in that list except the three noted.

PartLCSCLibraryNote
R 1k 0402C11702Basic
R 10k 0402C25744Basic
R 100k 0402C25741Basic
R 1M 0805C17514Basic150 V rated
C 10n 0402C15195Basic
C 100n 0402C1525Basic
C 1u 0402C52923Basic
C 10u 0402C15525Basic6.3 V X5R
BAT54S SOT-23C7420333Preferred Ext.$0 fee, 1.2 M in stock
MCP6004T-I/SLC7378Extendedfeeder fee
2.54 mm 1x02 header-Extendedno connectors are economic parts
2.54 mm 1x05 header-Extended"

3 unique Extended parts -> roughly $9 in one-off feeder fees.

Why R1/R9 stay 0805: the 0402 1M (C26083) is rated 50 V, the 0805 1M (C17514) is 150 V. R1/R9 take 10/11 of anything appearing on L1/L2, and the door strike is inductive. This is the one place the extra millimetre is worth it.

Cutting the feeder fees to zero

  1. Hand-solder the four headers. They are the only through-hole parts and the only reason to pay for THT assembly at all. Removes 2 of the 3 Extended parts.
  2. Swap the quad for 2x MCP6002 (C7377, Preferred Extended, $0). Two SOIC-8 instead of one SOIC-14. Only 3 of the 4 amplifiers are used, so two duals give the same single spare. Costs a schematic edit and one more decoupling cap.

Do NOT substitute LM324

LM324DT (C71035) is a Basic part, SOIC-14, and pin-compatible with the MCP6004. It will not work here. Its input common-mode range is Vee to Vcc-1.5 V, i.e. 0 to 1.8 V on a 3.3 V rail - but channel A's input sits at 2.05 V, outside that range entirely. Its 45 nA input bias across the 90.9 kOhm source would also add several mV of offset where the MCP6004's ~1 pA adds a microvolt. Same footprint, free, and completely wrong.

Files

FilePurpose
bom.csvfull engineering BOM (refs, values, footprints, LCSC, JLC library)
bom_jlcpcb.csvupload this to JLCPCB - Comment / Designator / Footprint / LCSC Part #, SMD only
bus_tap.pdfschematic print
erc.rptERC report

bom_jlcpcb.csv covers 21 assembled parts over 10 lines. J1, J2, J3 and JP1 are deliberately excluded - they are the only through-hole parts, they are the only Extended parts left once the MCP6004 fee is paid, and hand-fitting four headers takes minutes. Designators are written as explicit lists (R2,R4,R5,R6,R10), not KiCad's default ranges (R4-R6), which JLC's BOM parser does not understand.

Each symbol carries LCSC and JLC fields, so both BOMs regenerate straight from the schematic.

JLCPCB upload files (jlc/)

FileUpload as
bus_tap-gerbers.zipPCB (11 fab layers, gerber drill included)
bom_jlc.csvBOM - Comment / Designator / Footprint / LCSC Part #
cpl_jlc.csvCPL - Designator / Mid X / Mid Y / Layer / Rotation

J1, J2, J3 and JP1 are excluded from both CSVs (hand-soldered). BOM and CPL designators cross-check: 21 each, no orphans.

CPL rotation corrections - ALREADY APPLIED to cpl_jlc.csv

JLC's library orientation differs from KiCad's for two packages here. Determined empirically from JLC's upload preview, and baked into cpl_jlc.csv:

PartPackageKiCad rotCorrectionCPL value
D1SOT-230+180180
D2SOT-23180+1800
U1SOIC-140-90 (90 CW)270

Rotation in the CPL is counter-clockwise-positive, matching KiCad's own pos file (which emits -90 for C6/C7 and +90 for R10). KiCad places SOIC-14 with the long axis vertical and pin 1 top-left; JLC's library has it horizontal, hence the 90 deg.

The 18 chip R/C parts need no correction - they are two-terminal and non-polarised, so 0 vs 180 is electrically identical.

Verification on next upload: the preview should need NO manual rotation. If any of these three still looks wrong, the correction above is stale - re-derive it rather than nudging it in the preview.

Status

  • Schematic: complete, hand-tidied in eeschema, ERC clean (0 violations), netlist verified unchanged.
  • Footprints: assigned on all 25 parts, 9 distinct footprints, all verified present in the KiCad libraries.
  • PCB: not started. Target is JLCPCB Economic PCBA. Run Tools > Update PCB from Schematic (F8) in the PCB editor to seed it.

Parts

25
QtyValueFootprintReferences
5100kResistor_SMD:R_0402_1005MetricR2, R4, R5, R6, R10
310nCapacitor_SMD:C_0402_1005MetricC1, C4, C5
31kResistor_SMD:R_0402_1005MetricR3, R8, R11
210uCapacitor_SMD:C_0402_1005MetricC3, C7
21MResistor_SMD:R_0805_2012MetricR1, R9
2BAT54SPackage_TO_SOT_SMD:SOT-23D1, D2
1100nCapacitor_SMD:C_0402_1005MetricC6
110kResistor_SMD:R_0402_1005MetricR7
11uCapacitor_SMD:C_0402_1005MetricC2
1C1/C2Connector_PinHeader_2.54mm:PinHeader_1x02_P2.54mm_VerticalJ2
1ESP32 DevKitConnector_PinHeader_2.54mm:PinHeader_1x05_P2.54mm_VerticalJ3
1JUMPERConnector_PinHeader_2.54mm:PinHeader_1x02_P2.54mm_VerticalJP1
1L1/L2Connector_PinHeader_2.54mm:PinHeader_1x02_P2.54mm_VerticalJ1
1MCP6004Package_SO:SOIC-14_3.9x8.7mm_P1.27mmU1

Similar boards

  • 2 layers248.9 × 120.7 mm16nx, the printed circuit board in 3D

    16nx

    16n-faderbank/16nx

    16nx is a controller for musical instruments. Sixteen faders,MIDI over USB and jack, CV out, and I2C out. Based around RP2040.

    171 parts76
  • 4 layers58.4 × 101.9 mmUp5k osc, the printed circuit board in 3D

    Up5k osc

    emeb/up5k_osc

    The brute-force approach is to synthesize these analog waveforms at sufficiently high sample rates that the timing jitter becomes imperceptible.

    137 parts36MIT
  • 2 layers88.9 × 106 mmMarbles v70, the printed circuit board in 3D

    Marbles v70

    mort13/clandestine_circuitry

    Collection of diy synth projects

    208 parts12GPL-3.0
  • 2 layers47.6 × 220.4 mmModule, the printed circuit board in 3D

    Module

    zlosynth/proton

    Playground module for eurorack prototyping.

    124 parts7
  • 2 layers97 × 100 mmPortadora, the printed circuit board in 3D

    Portadora

    jdavidguerrero/grooveforge-brain

    Boutique hybrid AI synthesizer — Teensy 4.1 + ESP32-S3 + discrete 2N3904 ladder filter.

    64 parts
  • 2 layers101.3 × 108.5 mmTouch, the printed circuit board in 3D

    Touch

    microresearch/allcolours

    all the colours of the noise

    157 parts16

Questions

How big is the Bus tap PCB?

It measures 25.6 × 15.8 mm and has 2 copper layers, 1.6 mm thick.

What parts does the Bus tap use?

25 parts, built around the MCP6004-E/P and BAT54S. 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 Bus tap KiCad files?

From the Cptmeme/Urmet-Bibus-intercom-tap repository on GitHub, at the commit this page was made from: the board is bus_tap/bus_tap.kicad_pcb and its schematic bus_tap/bus_tap.kicad_sch. PCBKit opens the board in the browser, with nothing to install.

Can I use the Bus tap design in my own project?

Its repository publishes it under the GPL-3.0 licence: you may reuse it on that licence's terms (keep the author's notice, and for a copyleft licence share your changes alike).