Skip to the content
2 layers126 × 187 mmWorkbench s3-r01, the printed circuit board in 3D

Workbench s3-r01

leowzz/kivo

把 ESP32-S3 / RP2040 实体按键变成文字粘贴与快捷键的 Tauri 桌面工具和固件。

Size
126 × 187 mm
Copper layers
2
Thickness
1.6 mm
Parts
70
Nets
65
Pads
341
Tracks, vias
664, 102
Pours
18
Routed
Yes
KiCad
KiCad 10.0 (file 20260206)
Created
27 Jul 2026
Updated
18 Oct 2026

Overview

Workbench s3-r01 is an open-source printed circuit board by leowzz, from the leowzz/kivo repository on GitHub. It is a 2-layer board of 126 × 187 mm with 70 parts on 65 nets, routed with 664 tracks and 102 vias.

Its parts include 18 diodes, 18 switches, 8 connectors, 4 resistors and 3 capacitors. It belongs with the keyboards and input boards and the ESP32 and RP2040 boards of this library.

README

hardware/workbench-r03/README.md

Kivo Workbench r03 PCB Draft

This is an editable electrical and placement draft, not a board ready to order. Open workbench-r03.kicad_pro in KiCad 10. The PCB is intentionally unrouted, and no Gerber, drill, or assembly-order files are provided.

Confirmed Scope

  • RP2040 chip directly on the main PCB, with factory assembly for the QFN.
  • 18 ordinary MX switches with Kailh-style hot-swap sockets on the PCB back.
  • USB-C for USB 2.0 device data and 5 V power.
  • Existing SH1106, EC11, encoder press, confirm and back module connected by a harness. The module remains a separate panel-mounted assembly.
  • Enclosure changes and reprinting are permitted.

The existing r02 product YAML remains the source of the GPIO mapping. r03 here is a proposed new hardware revision, not a released Product Version ID.

Files

FilePurpose
workbench-r03.kicad_schEmbedded-symbol schematic, 59 components
workbench-r03.kicad_pcbFour-layer, 1.6 mm placement draft with 18 bottom sockets
workbench-r03.kicad_proKiCad project and preliminary design rules
Workbench.pretty/Local hot-swap socket and measured-head mounting footprints
key-coordinates.csvModel panel coordinates and PCB coordinates, in mm
placement.jsonReproducible placement and pin-to-net manifest
bom-draft.csvUncosted component list; not a factory purchasing BOM
verification.mdChecks performed and open issues

Electrical Design

The RP2040 core follows the Raspberry Pi hardware design guide: 3.3 V I/O, the internal 1.1 V regulator feeding DVDD, TESTEN tied to ground, local bypass capacitors, QSPI flash, and an external 12 MHz crystal. The proposed parts are:

FunctionProposed part / connection
MCURP2040, QFN-56 with exposed ground pad
FlashW25Q128JVSIQ, 128 Mbit / 16 MiB, 208 mil SOIC-8
CrystalAbracon ABM8-272-T3, 12 MHz, 15 pF loads, 1 kohm damping resistor
3.3 V regulatorAP2112K-3.3TRG1, 1 uF input and 4.7 uF output
USB-CGCT USB4105-GF-A, USB 2.0, separate 5.1 kohm CC1/CC2 pull-downs
USB dataUSBLC6-2SC6 protection, 27 ohm series resistors near RP2040
BOOTSELPush switch through 1 kohm to QSPI_SS; 10 kohm pull-up fitted
RESETPush switch to RUN, with 10 kohm pull-up
KeysEach GPIO to one socket contact; the other contact to GND
I2C pull-upsR9/R10 4.7 kohm footprints, DNP pending module inspection

Direct GPIO inputs use the existing firmware's pull-ups and debounce. This topology does not need matrix diodes. The 16 MiB flash matches the current YD-RP2040 build's maximum flash size. That does not, by itself, validate the custom board's firmware identity or boot behavior.

These are proposed MPNs, not a stock-checked shopping list. In particular, confirm the purchased socket's drawing against the vendored footprint, and confirm the exact USB connector suffix, plating and packaging before ordering. The PCB includes no microphone, speaker, battery, charger or RGB lighting.

Main Board Interfaces

J2 is a main-board harness pinout chosen for this PCB. It is not evidence of the left-to-right pin order of the purchased display module. Use individually mapped wires and the module's labels; do not assume a straight-through cable. The repository's YAML provides the GPIO assignments below, but does not record the module connector numbering or power specification.

J2 PinMain Board SignalRP2040 GPIO
1 (square pad)GND-
23.3 V-
3SCL27
4SDA26
5Confirm / OK22
6Encoder press28
7Encoder A21
8Encoder B20
9Back19

The main-board header is a 1x9, 2.54 mm pitch header. It is placed vertically in the PCB top view with pin 1 closest to the USB edge. J2 provides 3.3 V only; verify the module operates at 3.3 V and that its signals and I2C pull-ups do not drive 5 V into the RP2040. R9/R10 should be fitted only if the module lacks suitable pull-ups. The guide's "seven GPIO" count excludes power and ground.

J3 pins 1-4 are 3.3 V reference, GND, SWDIO and SWCLK. A debugger should sense the target voltage without powering a simultaneously USB-powered board.

J4 exposes all five unused RP2040 GPIOs at the rear-left (upper-left in top view) of the PCB. It is a 1x7 plated through-hole header, 2.54 mm pitch with 1.0 mm drills. Viewed from the component side with USB at the top, pin 1 is the leftmost square pad; the pins run left to right:

J4 PinSignal
1 (square pad)GND
23.3 V
3GPIO0
4GPIO23
5GPIO24
6GPIO25
7GPIO29 / ADC3

These pins connect directly to the RP2040 and use 3.3 V logic, not 5 V. External loads must fit within the regulator's remaining current and thermal budget. GPIO24/25 are free on this bare-chip design, but the current YD-RP2040 firmware pin whitelist excludes them. Enable them in the future custom-board definition before use; this hardware change does not change the product profile or assign functions to any expansion pins.

J5 (BOOT) and J6 (RESET) sit immediately to the left of the rear USB-C port. Each is a 1x2 plated through-hole footprint, 2.54 mm pitch with 1.0 mm drills, for a matching normally-open momentary button or short wires to a button. They are not a universal four-leg tactile-switch footprint. Viewed from the component side with USB at the top, pin 1 is the left square pad:

HeaderPin 1Pin 2Connection
J5 BOOTBOOT_BUTTONGNDParallel to SW19; through R7 (1 kohm) to QSPI_SS
J6 RESETRUNGNDParallel to SW20; R8 (10 kohm) pulls RUN up to 3.3 V

The onboard SW19/SW20 buttons remain fitted. To enter the USB bootloader, hold BOOT, press and release RESET, then release BOOT. Do not short QSPI_SS directly to ground; J5 preserves the existing series resistor.

K1-K18 retain GPIO1-GPIO18. Viewed from the key side with USB at the back, K1-K6 are the row closest to the display, K7-K12 are the middle row, and K13-K18 are closest to the user. The geometry script does not assign key IDs; this numbering follows the current product layout's reading order.

Mechanical Basis

Source: scripts/modeling/integrated_workstation.py, specifically KEY_COLUMNS, KEY_ROWS, KEY_PITCH, KEY_X0, KEY_Y0, PANEL_X0, and PANEL_Y0. The generated switch centers use the flat panel plane, not a top-down projection of its 30-degree assembled position.

  • Existing panel: 132 x 117 mm, tilted 30 degrees.
  • Proposed board: 126 x 105 mm, 1.6 mm thick, parallel to the panel.
  • Model panel coordinates: X to the right, Y from the front towards the rear.
  • Board coordinates in CSV: origin at the board's rear-left corner, X right, Y towards the user. Conversion: pcb_x = panel_x - 3, pcb_y = 113 - panel_y.
  • The KiCad page uses an additional (50, 50) mm translation for readability.
  • 19.05 mm switch pitch is preserved. The five 3.4 mm PCB holes are new proposed mounting positions; they do not reuse the existing panel screw axes.
  • The local mounting footprint assumes a screw head no larger than 5.6 mm, with a 6.0 mm clearance envelope and no large washer. This follows the project's measured 5.3 mm head, but actual fasteners and bosses need checking.

The current shell has two solid support walls in the key field, six fly-wire clips, a bottom-mounted development-board cradle and low rear USB openings. These features require redesign around the new board. The existing two-switch pod also needs a decision during the enclosure revision because it is absent from the current product's electrical configuration.

The Dwgs.User display rectangle is a reserved area, not a validated 3D module model. Before final PCB dimensions, verify the switch plate-to-PCB distance, socket underside height, display connector height, panel screw access and USB plug insertion. Include the J4 header/mating connector height near the display and the J5/J6 button or wire clearance in the enclosure check. The new USB port follows the sloped board and cannot align with the old bottom-board USB opening. The existing eight-pin modeling constant is inconsistent with the apparent nine contacts in refer/dsp-encp.png; keep the electrical harness independent of that mechanical assumption.

Remaining Design Work

  1. Verify the actual display module's voltage, connector labels and pull-ups, and the exact socket and USB connector drawings.
  2. Establish a manufacturer stackup and impedance geometry. The four-layer board is proposed to give USB and the RP2040 a continuous reference plane; the current layer count is not a validated impedance specification.
  3. Complete placement for short crystal, QSPI, regulator and decoupling paths, then route, pour ground planes and rerun DRC. Keep the USB pair over continuous ground and determine widths/gap for 90 ohm differential impedance from the selected stackup. Review QFN ground and paste/thermal-via assembly details.
  4. Revise and collision-check the enclosure in 3D, including MX plate capture thickness, new PCB mounts and the USB opening. Existing STLs are unchanged.
  5. Add the new board identity/build target and an r03 product definition when the electrical design is frozen; validate USB descriptors, flash size, BOOTSEL, reset, HID/CDC, all 18 keys, display and controls on assembled boards.
  6. Select purchasable parts, complete ERC/DRC and assembly review, and then export Gerbers, drill files, BOM and placement files for the board house.

Reproduction

The checked-in KiCad files are the editable design. The generators are a way to reproduce this first draft, not a substitute for the PCB editor. Generate into a new directory to preserve manual changes:

sh
uv run --script scripts/hardware/generate_workbench.py --output /tmp/workbench-review

Copy Workbench.pretty, 3dmodels, fp-lib-table and the project settings from this directory into that new directory, then run the placement script using KiCad's bundled Python interpreter:

sh
/Applications/KiCad/KiCad.app/Contents/Frameworks/Python.framework/Versions/3.9/bin/python3.9 \
  scripts/hardware/place_workbench.py /tmp/workbench-review/placement.json \
  /tmp/workbench-review/workbench-r03.kicad_pcb

The placement script refuses to overwrite an existing PCB. Both scripts accept explicit library paths for KiCad installations at other locations.

Sources

  • Existing product: products/kivo-workbench-rp-k18-disp-encp-r02/product.yaml.
  • Raspberry Pi Hardware Design with RP2040, release 2, sections 2.1-2.4. The source reference design's routing was not transplanted.
  • foostan/kbd MX hot-swap footprint, retrieved 2026-09-05, upstream blob 3601d4e1d8f8c5b49b9d56c87e00ec56cd4921a1. Only its 3D-model path was changed. The matching socket STEP model is vendored from the same repository. License: licenses/foostan-kbd-MIT.txt.
  • Standard electronic symbols, packages and 3D models come from installed KiCad 10.0.6 libraries. The schematic embeds the symbols for portability.

Parts

70
QtyValueFootprintReferences
181N4148W / K TO ROWD_SOD-123D1, D2, D3, D4, D5, D6, D7, D10, D11, D12, D13, D14, D15, D16, D17, D18 +2
12M3 head <=5.6mmMountingHole_M3_5.6mm_HeadH_D1, H_D2, H_D3, H_D4, H_L1, H_L2, H_L3, H_L4, H_U1, H_U2, H_U3, H_U4
6MouseBites_6x0.5_P0.8MouseBites_6x0.5_P0.8MB1, MB2, MB3, MB4, MB5, MB6
22.2k I2C PULLUPR_0805_2012Metric_Pad1.20x1.40mm_HandSolderR1, R2
1100n 16V X7RC_0805_2012Metric_Pad1.18x1.45mm_HandSolderC2
1100n 16V X7R / U1C_0805_2012Metric_Pad1.18x1.45mm_HandSolderC3
110kR_0805_2012Metric_Pad1.20x1.40mm_HandSolderR3
110k U1 RESET PULLUPR_0805_2012Metric_Pad1.20x1.40mm_HandSolderR4
110u 10V X7RC_0805_2012Metric_Pad1.18x1.45mm_HandSolderC1
1DISPLAY / MODULE PIN 1 = 3V3PinHeader_1x09_P2.54mm_VerticalJ2
1EXPANSION / 22 SPARE GPIO / 3V3 IOPinHeader_1x24_P2.54mm_VerticalJ4
1EXTERNAL BOOT / GPIO0 TO GNDPinHeader_1x02_P2.54mm_VerticalJ5
1EXTERNAL RESET / EN TO GNDPinHeader_1x02_P2.54mm_VerticalJ6
1KEY_1 MX HOTSWAPkeyswitch_cherrymx_hotswap_1uSW1
1KEY_10 MX HOTSWAPkeyswitch_cherrymx_hotswap_1uSW10
1KEY_11 MX HOTSWAPkeyswitch_cherrymx_hotswap_1uSW11
1KEY_12 MX HOTSWAPkeyswitch_cherrymx_hotswap_1uSW12
1KEY_13 MX HOTSWAPkeyswitch_cherrymx_hotswap_1uSW13
1KEY_14 MX HOTSWAPkeyswitch_cherrymx_hotswap_1uSW14
1KEY_15 MX HOTSWAPkeyswitch_cherrymx_hotswap_1uSW15
1KEY_16 MX HOTSWAPkeyswitch_cherrymx_hotswap_1uSW16
1KEY_17 MX HOTSWAPkeyswitch_cherrymx_hotswap_1uSW17
1KEY_18 MX HOTSWAPkeyswitch_cherrymx_hotswap_1uSW18
1KEY_2 MX HOTSWAPkeyswitch_cherrymx_hotswap_1uSW2
1KEY_3 MX HOTSWAPkeyswitch_cherrymx_hotswap_1uSW3
1KEY_4 MX HOTSWAPkeyswitch_cherrymx_hotswap_1uSW4
1KEY_5 MX HOTSWAPkeyswitch_cherrymx_hotswap_1uSW5
1KEY_6 MX HOTSWAPkeyswitch_cherrymx_hotswap_1uSW6
1KEY_7 MX HOTSWAPkeyswitch_cherrymx_hotswap_1uSW7
1KEY_8 MX HOTSWAPkeyswitch_cherrymx_hotswap_1uSW8
1KEY_9 MX HOTSWAPkeyswitch_cherrymx_hotswap_1uSW9
1LOWER / I2C4 TO J9 / 1:1JST_XH_B4B-XH-A_1x04_P2.50mm_VerticalJ8
1MCP23017-E/SO / 0x20SOIC-28W_7.5x17.9mm_P1.27mmU1
1UPPER / I2C4 TO J8 / 1:1JST_XH_B4B-XH-A_1x04_P2.50mm_VerticalJ9
1YD P1 / RIGHT SOCKET / 1x22PinSocket_1x22_P2.54mm_VerticalJ1
1YD P2 / LEFT SOCKET / 1x22PinSocket_1x22_P2.54mm_VerticalJ7

More from leowzz/kivo

2
  • 4 layers126 × 105 mmWorkbench r03, the printed circuit board in 3D

    Workbench r03

    leowzz/kivo

    把 ESP32-S3 / RP2040 实体按键变成文字粘贴与快捷键的 Tauri 桌面工具和固件。

    64 parts
  • 2 layers124 × 76 mmKeypad i2c k18-r01, the printed circuit board in 3D

    Keypad i2c k18-r01

    leowzz/kivo

    把 ESP32-S3 / RP2040 实体按键变成文字粘贴与快捷键的 Tauri 桌面工具和固件。

    47 parts

Similar boards

  • 2 layers61.8 × 73.2 mmBrain board STM32F407, the printed circuit board in 3D

    Brain board STM32F407

    rusefi/rusefi

    rusefi - GPL internal combustion engine control unit

    70 parts1.2k
  • 2 layers47.3 × 52.8 mmFinalv1, the printed circuit board in 3D

    Finalv1

    hackclub/OnBoard

    💡 Join 1,000 teenagers and make your first PCB with a $100 grant!

    70 parts915
  • 2 layers74.3 × 52.8 mmBq3060, the printed circuit board in 3D

    Bq3060

    iam4722202468/ThinkpadBattery

    Open source Thinkpad T420 battery design

    70 parts304MIT
  • 2 layers141 × 88 mmErgoSNM Keyboard Right Prototype 1, the printed circuit board in 3D

    ErgoSNM Keyboard Right Prototype 1

    siderakb/ergo-snm-keyboard

    ErgoSNM is a split ergonomic keyboard integrated with trackball, wireless is in beta

    70 parts172CERN-OHL-P-2.0
  • 2 layers90 × 100 mmAlu, the printed circuit board in 3D

    Alu

    imihajlow/ccpu

    A 8-bit computer made of 74xx series logic gates and memory ICs.

    70 parts145
  • 2 layers90 × 140 mmDrumkid, the printed circuit board in 3D

    Drumkid

    mattybrad/drumkid

    Version 4 was the first successful working design, with full code, schematics, Gerbers, etc available on GitHub.

    70 parts137
  • 2 layers152.5 × 117.5 mmKeytartouch, the printed circuit board in 3D

    Keytartouch

    cnlohr/cnhardware

    My dumping grounds for all my kicad projects and random hardware bringup.

    70 parts114

Questions

How big is the Workbench s3-r01 PCB?

It measures 126 × 187 mm and has 2 copper layers, 1.6 mm thick.

What parts does the Workbench s3-r01 use?

70 parts. 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 Workbench s3-r01 KiCad files?

From the leowzz/kivo repository on GitHub, at the commit this page was made from: the board is hardware/workbench-s3-r01/workbench-s3-r01.kicad_pcb and its schematic hardware/keypad-i2c-k18-r01/keypad-i2c-k18-r01.kicad_sch. PCBKit opens the board in the browser, with nothing to install.

Can I use the Workbench s3-r01 design in my own project?

Its repository states no licence, so its author keeps all rights: ask leowzz before reusing the design.