Skip to the content
4 layers50.8 × 22.9 mmZb1, the printed circuit board in 3D

This folder holds the complete electronic CAD for the ZB-1 development board:

Size
50.8 × 22.9 mm
Copper layers
4
Thickness
1.6 mm
Parts
71
Nets
57
Pads
309
Tracks, vias
1,127, 149
Pours
8
Routed
Yes
KiCad
KiCad 7 (file 20221018)
Created
19 Oct 2026
Updated
21 Oct 2026

Overview

Zb1 is an open-source printed circuit board by danindiana, from the danindiana/zemizdat repository on GitHub, published under the Apache-2.0 licence. It is a 4-layer board of 50.8 × 22.9 mm with 71 parts on 57 nets, routed with 1,127 tracks and 149 vias.

It is built around the ESP32-S3-MINI-1-N8, DW01A and MAX17048G+T10, with the RT9080-33GJ5, USBLC6-2SC6 and B5819W among its other parts. Its parts include 25 resistors, 16 capacitors, 7 ICs, 6 connectors and 3 diodes. It belongs with the ESP32 boards of this library.

Main components

8

README

05_hardware/zb1/cad/README.md

ZB-1 CAD package — KiCad 7 schematic, 4-layer PCB, fab outputs, 3D model

This folder holds the complete electronic CAD for the ZB-1 development board:

  • a KiCad 7 project with schematic and routed 4-layer PCB;
  • Gerbers, drill, pick-and-place and BOM;
  • a STEP model of the assembled board, plus rendered views.

Everything is generated by scripts from one design database (scripts/zb1_design.py), so the board can be rebuilt and every number below re-checked.

ZB-1 3D render, top

Licence:

If you modify the design and share it, say so in your copy (CERN-OHL-P §3.3).

Status: design files, not a proven board. Nothing here has been fabricated, assembled or powered. The layout was placed by script and routed by an autorouter. DRC results are reported honestly in §5, including the items that still need a human. A qualified layout review is required before ordering boards; see the checklist in §7.

Board50.8 × 22.86 mm (Adafruit Feather outline), 1.5 mm corner radius, 1.6 mm FR-4
Layers4: F.Cu signal / In1 solid GND plane / In2 signal + GND fill / B.Cu signal + GND fill
Parts69 electrical parts + 2 mounting holes placed (7 of them DNP by default), top and bottom side
Routing1 127 track segments, 149 vias; 0.15 mm signal / 0.3 mm power / 0.2 mm USB tracks, 0.5/0.25 mm vias
Antennamodule antenna flush with the board edge; copper keep-out on all four layers past x = 45.4 mm
Netlistschematic netlist checked pin by pin against the design database: OK — 69 components, 57 nets, 264 pin connections; the PCB pads were cross-checked the same way (0 mismatches)
DRC0 unconnected, 0 clearance / hole / short errors. 8 mechanical items waived (mounting-hole courtyards, edge-mount microSD shell), 94 cosmetic warnings (silkscreen, library-copy differences) — see §5

1. Files

PathWhat it is
zb1.kicad_pro, zb1.kicad_sch, zb1.kicad_pcbKiCad 7 project: open zb1.kicad_pro in KiCad 7.0 or newer
lib/zb1.kicad_symproject symbols for parts KiCad 7 lacks: BQ21040, RT9080-33, DW01A, FS8205A, MAX17048
lib/zb1.pretty/ESP32-S3-MINI-1.kicad_modmodule footprint from espressif/kicad-libraries (CC-BY-SA 4.0 with the KiCad design exception)
lib/3dmodels/Espressif module STEP model, plus simple dimensioned envelope bodies for parts without a KiCad 3D model (USB-C, microSD, both JST connectors, KMR2 switches, crystal)
fab/zb1_gerbers.zipGerber X2 (11 layers) + Excellon drill (PTH and NPTH separate): upload this to a PCB fab
fab/zb1_bom.csvgrouped BOM with MPNs; DNP lines marked
fab/zb1_pos.csvpick-and-place centroids, both sides, mm (DNP and through-hole parts excluded)
docs/zb1_schematic.pdfschematic, one A2 sheet in seven titled blocks
docs/zb1_assembly_top.pdf, docs/zb1_assembly_bottom.pdfassembly drawings (fab layer with every reference)
docs/*drl_map.pdfdrill maps
3d/zb1.stepwhole assembly for enclosure/mechanical CAD (FreeCAD, Fusion, Onshape, SolidWorks)
images/schematic PNG, per-copper-layer plots, board-surface images, 3D renders
reports/drc.rptfull KiCad DRC report
reports/netlist_check.txtschematic-vs-design-database check
scripts/the generators (§6)
build.shrebuilds everything above from scripts/zb1_design.py

2. Schematic

Schematic

The schematic implements exactly the circuit in ../README.md §3–§5. It is drawn in a "label per pin" style: every pin gets a short stub with its net label. It is generated from zb1_design.py, so edit that file and regenerate rather than editing the schematic by hand. reports/netlist_check.txt confirms that the netlist KiCad exports from the schematic matches the database:

  • every component present, with the designed footprint and value;
  • every designed pin connection present;
  • no extra connections.

Changes from the earlier text description, made while drawing it:

  • BQ21040 pinout checked against the TI datasheet: 1 TS, 2 OUT, 3 /CHG, 4 ISET, 5 VSS, 6 IN. TS must not float (that enters a test mode), so R4 = 10 kΩ to GND stays fitted.
  • USBLC6-2SC6 is flow-through: pins 1/6 and 3/4 are the same line, so each data line is one net.
  • TPS22917 QOD is tied to VOUT so the card's supply is actively discharged when switched off. CT is left open for the fastest turn-on.
  • Battery connector: J3 pin 1 = BAT−, pin 2 = BAT+. Check this against your cell: JST-PH LiPo leads have no polarity standard, and a reversed cell will destroy the charger.
  • Optional cell protection: U6 DW01A and Q2 FS8205A are drawn and laid out but DNP. SJ2 bridges BATN to GND. Cut SJ2 if you fit them.

3. PCB

TopBottom (seen from below)
topbottom

Top side

  • ESP32-S3-MINI-1 with its antenna at the right-hand edge.
  • USB-C at the left, with ESD protection.
  • Charger and power-path parts.
  • Vertical JST-PH battery jack.
  • RESET and BOOT buttons.
  • 32.768 kHz crystal placed against the module's XTAL_32K pins.
  • Charge and user LEDs.
  • Feather headers (supplied loose).

Bottom side

  • microSD socket, slot at the USB end.
  • SD load switch and pull-ups.
  • LDO and the current-measurement jumper SJ1 (marked CUT=I).
  • Battery divider.
  • STEMMA-QT connector.
  • Test pads TP1–TP5 for a pogo-pin fixture: TP_EN, VBAT, VSYS, 3V3, GND.
  • Optional protection and fuel-gauge footprints.
F.CuIn1 (GND plane)
F.CuIn1
In2B.Cu
In2B.Cu

Layout decisions:

  • Antenna:
    • The module sits flush with the board edge.
    • A rule area bans copper pour, tracks and vias on all four layers under and beyond the antenna (x > 45.4 mm).
    • No parts sit on either side in that zone.
  • No tracks under the module's centre on F.Cu. A rule area 1.4 mm inside the pad ring allows only vias and the GND pour there. Pads may take a short inward stub to a via (standard practice for LGA modules, and needed to escape 0.85 mm-pitch pads). The centre GND pad has nine via-in-pad stitches to the In1 plane; specify them filled and capped, or tented from the bottom.
  • GND:
    • In1 is an unbroken plane.
    • F.Cu, In2 and B.Cu are GND-filled with thermal reliefs.
    • Every SMD GND pad that had room received its own via to the plane before routing.
  • Mounting holes:
    • Only the two antenna-end Feather holes (M2) are present.
    • The two USB-end holes collide with the microSD socket on the bottom and were omitted — a deliberate deviation from the Feather specification.
    • The antenna-end holes touch the module courtyard, exactly as on Adafruit's own ESP32-S3 Feather.
  • Silkscreen:
    • Feather pin names on the top.
    • Battery polarity marks, button names and board name on the top.
    • Passive references only on the assembly drawings, to keep the silkscreen legible.
    • No serial numbers or unique identifiers (../README.md R8).

Design rules used

Set for a standard 4-layer prototype service (JLCPCB/PCBWay class): track/space 0.15/0.15 mm signal (fab minimum is typically 0.09–0.1 mm), 0.3 mm power, via 0.5 mm pad / 0.25 mm drill, hole-to-copper 0.2 mm, copper-to-edge 0.25 mm. Check the 0.25 mm drill against your fab's standard (not premium) capability before ordering.

4. 3D model

iso bottom

3d/zb1.step contains the bare board and every fitted part:

  • the real Espressif module model;
  • KiCad library models for the passives, ICs and headers;
  • simple dimensioned envelope bodies for the six parts KiCad 7 ships no model for (USB-C, microSD socket, JST-PH vertical, JST-SH vertical, KMR2 switches, 3215 crystal).

The envelopes are correct in footprint position and outline size, so they are good enough for designing an enclosure, but they are not detailed parts. DNP parts are omitted. The renders overlay the board's real copper, mask, ENIG pads and silkscreen, composited from the KiCad layer plots, onto the STEP geometry.

5. DRC result and what still needs a human

Report: reports/drc.rpt, KiCad 7.0.11 DRC run on the saved board with all zones refilled.

CategoryCountSeverityStatus
Unconnected items0errorevery net is routed
Clearance, hole clearance, shorts, track width, annular ring, keep-out violations by copper0error—
Courtyard overlap: M2 holes H3/H4 vs module U1 and the header rows4errorwaiver. These are the screw-head courtyards of the antenna-end Feather holes, with exactly the same geometry as Adafruit's ESP32-S3 Feather. The holes are NPTH, with no copper. Use nylon screws or bottom-side standoffs only.
Items not allowed: H3/H4 courtyard inside the module footprint's antenna keep-out2errorwaiver for the same holes: no copper and no parts sit in the keep-out; only the screw-head clearance circle touches it. Drop H3/H4 entirely if you prefer a strictly clean report.
Copper to board edge: microSD shell tabs (J2 pad 11)2errorwaiver. The socket is edge-mounted by design: its slot is at the board edge. The tabs are GND.
Silkscreen overlap / clipped by mask / clipped by edge73warningcosmetic. Mostly footprint outlines on dense 0402 areas and the USB-C/microSD outlines that cross the edge. The fab clips silk to mask (--subtract-soldermask).
Footprint differs from library copy21warningexpected: these footprints were given envelope 3D models or the DNP attribute in the board

How routing was completed. Three routing tools were involved, in order:

  1. Maze pre-route (scripts/complete.py). A small net-aware A* router on a 0.05 mm grid routes a few nets first and locks them:
    • the USB D+/D− lines;
    • both 32 kHz crystal lines;
    • the ESD chip's VBUS hop;
    • one protection-circuit hop.
  2. Freerouting 1.4.4. It routes everything else around the locked nets.
  3. Maze completion pass. It closes whatever Freerouting left open, with local rip-up and retry. It also does two clean-ups:
    • moves a stranded test pad next to its own net;
    • trims short dangling stubs, with connectivity checked after each removal.

Freerouting is deterministic for a given input, but small input changes reshuffle its result. So scripts/best_of.py tries three pre-route sets and keeps the best. Result:

Pre-route setUnconnected
A1
B0 (used)
C1

What still needs a human before ordering (beyond the checklist in §7):

  • Trace quality, not just legality. The routing is DRC-clean but autorouted: there are detours and more vias than a hand layout would have. Re-routing the charger/power-path loop and shortening the SD bus are worthwhile.
  • USB D+/D− are routed as two single 0.2 mm tracks, not a coupled 90 Ω pair. That is acceptable for 12 Mbit/s full-speed, but re-route them as a pair if you touch that area.
  • Via-in-pad under the module centre (9 vias): order them filled and capped, or tented.
  • Test pad TP3 (VSYS) sits beside the regulator rather than in the TP row, because the router could not reach the original spot.

6. How it was generated (and how to change it)

text
scripts/zb1_design.py     single source of truth: every part, footprint, value, MPN, pin -> net
scripts/gen_libs.py       project symbols + module footprint/3D model
scripts/gen_models.py     envelope STEP bodies for parts without library models
scripts/gen_schematic.py  zb1.kicad_sch (A2, seven blocks), verified by verify_netlist.py
scripts/gen_pcb.py        outline, fixed placements, greedy courtyard-clearing placement of the rest,
                          antenna keep-out, module no-track area          -> build/zb1_placed.kicad_pcb
scripts/route.py          GND fan-out vias, Specctra DSN (with In1 GND plane), Freerouting -> build/zb1.ses
scripts/finish.py         session import, GND pours on 4 layers, silkscreen, zone fill, DRC
scripts/export.py         Gerbers/drill/pos/BOM, PDFs, STEP, layer plots, surface textures, renders
scripts/texture.py        mask/copper/ENIG/silk composite of the KiCad layer plots
scripts/render3d.py       STEP -> OpenCASCADE -> VTK off-screen renders

To change the circuit:

  1. Edit zb1_design.py.
  2. Run ./build.sh.

To move parts, edit FIXED / TARGET in gen_pcb.py.

Toolchain used (2026-10-19):

  • KiCad 7.0.11 (Ubuntu 24.04 packages, with the symbol, footprint and 3D libraries).
  • Freerouting 1.4.4 built from source. The only local patch is an optional time cap on the post-route optimiser (-Dzb1.opt.seconds), set to 600 s here.
  • OpenCASCADE (cadquery-ocp) and PyVista/VTK for the renders.
  • Shapely for placement geometry.

KiCad 8/9 will open and upgrade the project.

7. Review checklist before ordering

  1. Open zb1.kicad_pro in KiCad, run DRC, and finish or clean up anything listed in §5.
  2. USB D+/D−: the autorouter does not do differential pairs. At USB 2.0 full speed (12 Mbit/s, which is what the S3's USB block runs) this is tolerable, but re-route them as a 90 Ω pair if you touch the area.
  3. Check the power-path and charger loop areas (VBUS → U2 → VBAT → Q1 → VSYS → U3). The 0.3 mm power tracks carry at most 500 mA charge current or about 350 mA module peak; widen where space allows.
  4. Check the BQ21040 R_ISET, the RT9080 pinout (VIN-GND-EN-NC-VOUT) and the DW01A/FS8205A pinouts against the datasheets of the exact parts you buy. Second-source parts differ.
  5. Confirm J3 polarity against your battery (§2).
  6. Confirm the microSD and USB-C footprints against the exact connector part numbers in the BOM. Look-alike parts often have different shell-pad positions.
  7. Order 5 bare boards plus a stencil, or PCBA, and run the bring-up procedure in ../README.md §10.

Parts

71
QtyValueFootprintReferences
810kResistor_SMD:R_0402_1005MetricR4, R9, R10, R11, R12, R13, R14, R25
41MResistor_SMD:R_0402_1005MetricR5, R6, R8, R22
41uFCapacitor_SMD:C_0402_1005MetricC4, C10, C15, C16
3100kResistor_SMD:R_0402_1005MetricR7, R16, R17
3100nFCapacitor_SMD:C_0402_1005MetricC7, C13, C14
310uFCapacitor_SMD:C_0603_1608MetricC1, C6, C11
218pFCapacitor_SMD:C_0402_1005MetricC8, C9
222uFCapacitor_SMD:C_0805_2012MetricC3, C5
24.7kResistor_SMD:R_0402_1005MetricR18, R19
25.1kResistor_SMD:R_0402_1005MetricR1, R2
2M2MountingHole:MountingHole_2.2mm_M2H3, H4
11.07kResistor_SMD:R_0402_1005MetricR3
1100Resistor_SMD:R_0402_1005MetricR23
11kResistor_SMD:R_0402_1005MetricR21
12.2kResistor_SMD:R_0402_1005MetricR20
12kResistor_SMD:R_0402_1005MetricR24
132.768kHz 12.5pFCrystal:Crystal_SMD_3215-2Pin_3.2x1.5mmY1
133Resistor_SMD:R_0402_1005MetricR15
13V3TestPoint:TestPoint_Pad_D1.0mmTP4
14.7nFCapacitor_SMD:C_0402_1005MetricC12
14.7uFCapacitor_SMD:C_0603_1608MetricC2
1B5819WDiode_SMD:D_SOD-123D1
1BATT JST-PHConnector_JST:JST_PH_B2B-PH-SM4-TB_1x02-1MP_P2.00mm_VerticalJ3
1BOOTButton_Switch_SMD:SW_Push_1P1T_NO_CK_KMR2SW2
1BQ21040DBVRPackage_TO_SOT_SMD:SOT-23-6U2
1CHG orangeLED_SMD:LED_0603_1608MetricLED2
1DMG3415UPackage_TO_SOT_SMD:SOT-23Q1
1DW01APackage_TO_SOT_SMD:SOT-23-6U6
1ESP32-S3-MINI-1-N8zb1:ESP32-S3-MINI-1U1
1FS8205APackage_SO:TSSOP-8_4.4x3mm_P0.65mmQ2
1Feather 12Connector_PinHeader_2.54mm:PinHeader_1x12_P2.54mm_VerticalJ6
1Feather 16Connector_PinHeader_2.54mm:PinHeader_1x16_P2.54mm_VerticalJ5
1GNDTestPoint:TestPoint_Pad_D1.0mmTP5
1I_MEASJumper:SolderJumper-2_P1.3mm_Bridged_RoundedPad1.0x1.5mmSJ1
1MAX17048G+T10Package_DFN_QFN:TDFN-8-1EP_2x2mm_P0.5mm_EP0.8x1.2mmU7
1PROT bypassJumper:SolderJumper-2_P1.3mm_Bridged_RoundedPad1.0x1.5mmSJ2
1RESETButton_Switch_SMD:SW_Push_1P1T_NO_CK_KMR2SW1
1RT9080-33GJ5Package_TO_SOT_SMD:SOT-23-5U3
1STEMMA-QTConnector_JST:JST_SH_BM04B-SRSS-TB_1x04-1MP_P1.00mm_VerticalJ4
1TPS22917DBVRPackage_TO_SOT_SMD:SOT-23-6U4
1TP_ENTestPoint:TestPoint_Pad_D1.0mmTP1
1USB-CConnector_USB:USB_C_Receptacle_HRO_TYPE-C-31-M-12J1
1USBLC6-2SC6Package_TO_SOT_SMD:SOT-23-6U5
1USER redLED_SMD:LED_0603_1608MetricLED1
1VBATTestPoint:TestPoint_Pad_D1.0mmTP2
1VSYSTestPoint:TestPoint_Pad_D1.0mmTP3
1microSD push-pushConnector_Card:microSD_HC_Hirose_DM3AT-SF-PEJM5J2

Similar boards

  • 2 layers79 × 30 mmLIA, the printed circuit board in 3D

    LIA

    JGAguado/LIA

    Low-power pet tracking platform built around Meshtastic and LoRa mesh networking

    81 parts29
  • 2 layers30 × 65 mmDevboard, the printed circuit board in 3D

    Devboard

    dark-Phoenix2077/voidboard

    custom esp32 devboard with extensive power management and a built-in IMU

    44 parts
  • 4 layers70.9 × 75 mmFlagshep Audio Player V1, the printed circuit board in 3D

    Flagshep Audio Player V1

    HYLDAIC/Flagshep-V1_Audio-Player

    A high fidelity semi-portable audio player student project with provided PCB files, 3D files and Code

    77 parts1CERN-OHL-P-2.0
  • 2 layers45 × 95 mmAirquality, the printed circuit board in 3D

    Airquality

    MorgenWebDigital/airquality

    A battery-powered indoor air quality monitor. Real CO₂ from a photoacoustic sensor, VOC and NOx, temperature, humidity and ambient light, shown on a 2.13" e-paper display and sent over Bluetooth LE.

    78 parts
  • 2 layers80 × 34 mmDji fcc, the printed circuit board in 3D

    Dji fcc

    nikolaus018/dji-fcc-esp32

    ESP32-S3 firmware that switches a DJI N1 remote to FCC mode over USB (replaces the Android app)

    69 parts3MIT
  • 2 layers93.2 × 93.2 mmSmartcoaster routed, the printed circuit board in 3D

    Smartcoaster routed

    bdus/SmartCoaster

    AI native Industrial and Embedded Design

    70 parts
  • 2 layers96 × 50 mmPager, the printed circuit board in 3D

    Pager

    justinlindh/bramble

    Privacy-first LoRa mesh networking for ESP32-S3, built with ESP-IDF

    97 parts2MIT
  • 2 layers80.5 × 75.1 mmF411-TableClock, the printed circuit board in 3D

    F411-TableClock

    DRIFTYY777/F411-TableClock

    61 parts

Questions

How big is the Zb1 PCB?

It measures 50.8 × 22.9 mm and has 4 copper layers, 1.6 mm thick.

What parts does the Zb1 use?

71 parts, built around the ESP32-S3-MINI-1-N8, DW01A, MAX17048G+T10 and RT9080-33GJ5. 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 Zb1 KiCad files?

From the danindiana/zemizdat repository on GitHub, at the commit this page was made from: the board is 05_hardware/zb1/cad/zb1.kicad_pcb and its schematic 05_hardware/zb1/cad/zb1.kicad_sch. PCBKit opens the board in the browser, with nothing to install.

Can I use the Zb1 design in my own project?

Its repository publishes it under the Apache-2.0 licence: you may reuse it on that licence's terms (keep the author's notice, and for a copyleft licence share your changes alike).