Skip to the content
2 layers100 × 80 mmPotholeCart Expansion, the printed circuit board in 3D

PotholeCart expansion carrier board (KiCad 10): Pi ribbon + L298 + SIM800L + GPS + buzzer, DRC-clean with Gerbers

Size
100 × 80 mm
Copper layers
2
Thickness
1.6 mm
Parts
38
Nets
21
Pads
114
Tracks, vias
131, 15
Pours
1
Routed
Yes
KiCad
KiCad 10.0 (file 20241229)
Created
25 Sep 2026
Updated
25 Sep 2026

Overview

PotholeCart Expansion is an open-source printed circuit board by thrishunchand-fpga, from the thrishunchand-fpga/potholecart-pcb repository on GitHub. It is a 2-layer board of 100 × 80 mm with 38 parts on 21 nets, routed with 131 tracks and 15 vias.

It is built around the SMBJ5.0A and TP1. Its parts include 7 connectors, 6 resistors, 5 capacitors, 2 diodes and 1 transistor. It belongs with the radio and wireless boards of this library.

Main components

2

README

README.md

PotholeCart Expansion Board — README

Standalone expansion (carrier) board for the Smart Pothole Detection cart (Raspberry Pi 3B+). The Pi connects by 40-way ribbon; L298, SIM800L, GPS and buzzer plug/solder into headers. Camera stays on Pi USB.

  • KiCad 10.0.6 project: PotholeCart_Expansion.{pro,sch,pcb}
  • Board: 100 x 80 mm, 2-layer, 1.6 mm, 1 oz Cu, ENIG (JLCPCB 2-layer rules)
  • Source of truth: gen_pcb.py in temp opencode folder — edit IT, never the KiCad files by hand, then regenerate (workdir = this folder): python gen_pcb.py

1. Connection map (matches pi_pothole_complete_system.py)

Pi GPIOBoard netGoes to
12 / 23 / 24GPIO12_ENA / IN1 / IN2J4 pins 1-3 (L298 left channel)
13 / 27 / 22GPIO13_ENB / IN3 / IN4J4 pins 7/5/6 (L298 right channel)
14 → / → 15GPS_TX / GPS_RXJ2 (GY-NEO6MV2 RX/TX), 9600 NMEA
5 → / → 6GSM_TX_PI / GSM_RX_PIJ3 (SIM800L RX/TX), 9600 SW UART
18GPIO18 → R1 1k → Q1 base (Q1_B net) → BUZ_PLUSQ1 2N2222 driver → J7/buzzer, PWM beep

J1 (2x20 IDC) carries Pi 5 V (pins 2,4), GND (6,9,14,20,25,30,34,39), all above signals; all other Pi pins are no-connects.

2. Power tree (3 separate sources, star GND on board)

  • Pi 5 V adapter -> Pi -> J1 pins 2/4 +5V_IN (board is a LOAD on the Pi, not a source). +5V_IN feeds only: riser/corridor, TP1, F1 pin 1.
  • F1 500 mA fuse is the ONLY +5V_IN -> +5V bridge (no copper shorts it). +5V (fused, ~100 mA peripherals only) feeds: GPS J2p1, buzzer BZ1p1/D1, PWR LED R5, C3, TVS1. TP1 reads the PRE-fuse side.
  • Motor battery 6-12 V -> J5 VBATT_IN -> L298 VS only.
  • SIM800L supply ~4 V / 2 A peak (LiPo or buck) -> J6 VGSM_IN -> V_GSM4V rail with 1000 uF (C2) + 470 uF (C1) + 100 nF (C5) bulk. C1 sits on V_GSM4V, NOT on +5V.
  • L298 logic 5 V jumper stays CONNECTED (module self-powers logic).
  • Protection: F1 500 mA fuse + TVS SMBJ5.0A + green PWR LED on +5V.
  • SIM800L TX -> GPIO6: divider pads R3 (10k) / R4 (18k), BOTH DNP by default; SJ1 jumper 1-2 DIRECT fitted (2-3 kills UART). Fit R3/R4 only if SIM800L replies are garbled (then remove SJ1 jumper).
  • SIM_RST has R6 10k pullup to V_GSM4V (TP9).

3. Bring-up order

  1. Visual inspection (bridges, orientation), then continuity: GND net across J1/J2/J3/J4/TP2, no shorts between +5V / V_GSM4V / VBATT / GND.
  2. Power 5 V only (no modules): LED1 on, TP1 = 5 V, TP2 = 0 V.
  3. Power motor battery only: VBATT at J5, no heat on L298.
  4. Power 4 V only: V_GSM4V present, bulk caps correct polarity.
  5. Plug modules one at a time (GPS, GSM, L298, buzzer), re-check rails.
  6. Connect Pi ribbon LAST, boot, run pigpiod + system script.

4. Assembly checklist

  • Solder order: passives (R1-R6, D1, C3-C5, TVS1, LED1) -> headers (J1-J4, J7, SJ1) -> screw terminals (J5, J6) -> bulk caps (C1, C2, watch polarity — BOTH on the V_GSM4V rail) -> Q1 (flat side to silkscreen) -> fuse holder.
  • R3/R4 divider: DNP by default, SJ1 1-2 DIRECT jumper fitted. Fit R3/R4 only if SIM800L replies are garbled (then remove SJ1 jumper).
  • Q1 2N2222: pads numbered to symbol pins 1=B(middle)/2=C/3=E — VERIFY against the physical transistor before soldering (DMM diode test). R1 (1k) drives the base, R2 (10k) pulls it down — GPIO18 never touches the transistor directly.
  • Buzzer: 12 mm passive piezo, ~7.6 mm pitch (confirm with calipers).
  • J2/J7 are JST-XH; J3/J4/SJ1 are 2.54" headers; J5/J6 are 5.08 mm.
  • Hand-soldering: GND pads use SOLID pour (no thermals) — use 350 C+ iron, preheat, allow extra dwell on J1/J5/J6 ground pins.

5. Test procedure (TP1-TP9, multimeter/scope)

TPNetExpect
TP1 / TP2+5V_IN (pre-fuse) / GND5.0 V / 0 V, powered
TP3GPS_TX3.3 V UART bursts (scope), NMEA on console
TP4 / TP5GSM_TX_PI / GSM_RX_PI3.3 V activity during AT/HTTP
TP6 / TP7GPIO12_ENA / GPIO13_ENB1 kHz PWM, ~70 % while driving
TP8BUZ_PLUS2-15 Hz beeps near potholes
TP9SIM_RSThigh via R6 pullup to V_GSM4V, pulses on reset

6. Validation status (2026-09-23, after 3 must-fixes)

  • Must-fixes applied + verified: (1) Q1 base via R1 1k on dedicated Q1_B net with R2 10k pulldown (D1 moved east to clear the routing); (2) F1 fuse split +5V_IN (Pi source side) / +5V (fused peripherals), F1 body is the only bridge; (3) C1 470u moved to the V_GSM4V rail (GSM bulk = 1000u + 470u + 100n). Also: R6 10k TP9→V_GSM4V pullup, +5V_IN power symbol, PWR_FLAG power_out.
  • exact.py (rect-exact crossings/clearance): 0 crossings, 0 pad hits.
  • kicad-cli sch erc (erc_20260923b.txt): 0 errors. Only headless-env library warnings (missing lib tables); the 4 former power_pin_not_driven errors are gone.
  • kicad-cli sch export netlist (netlist_20260923.xml): schematic <-> PCB pin-net tables match (incl. +5V_IN, Q1_B).
  • kicad-cli pcb drc --refill-zones (drc_20260923.json, drc_20260923_run2.json): 0 unconnected, 0 electrical errors, identical across 2 runs. Residual: 17 silkscreen-over-pad cosmetics (reference fields vs pads — JLCPCB auto-clips, zero electrical impact, waived) + headless-env library warnings.
  • Re-verified same session (drc_20260923_verify3.json + drc_20260923_verify3_run2.json, erc_20260923_verify3.txt, netlist_20260923_verify3.xml, exact.py 0/0): same profile — 0 unconnected, 0 ERC errors, silk cosmetics only. No layout change, fab/ (19:52, from current PCB rev 19:48) stays valid.
  • kicad-cli is run-to-run nondeterministic — always re-run with unique output names; DRC is the final authority.

7. JLCPCB ordering notes

  • 2-layer, 1.6 mm, 1 oz, ENIG, green mask. Ready-to-send outputs in fab/ (generated 2026-09-23 via kicad-cli pcb export gerbers/drill): F/B copper, masks, silkscreens, Edge.Cuts, .drl + .gbrjob. Regenerate after any layout change.
  • Design rules used: 0.2 mm min track/clearance (JLCPCB 2-layer); power 1.0-1.2 mm, motor 1.5 mm, signals 0.25-0.3 mm. Zone clearance 0.25 mm, solid GND pad connections.

8. Still needs physical sign-off (measure before fab)

  • Buzzer pin pitch (photo says 12 mm / 7.6 mm — confirm with calipers).
  • SIM800L-mini header pin order on YOUR module.
  • GY-NEO6MV2 4-pin order (VCC/RX/TX/GND as silkscreened?).
  • Gold-P169 signal-row order (ENA IN1 IN2 GND IN3 IN4 ENB).
  • JST-XH vs 2.54" headers actually owned.
  • Q1 E-B-C orientation vs flat side.
  • Motor stall current vs 1.5 mm copper.

9. Demo video

assets/demo/pcb-demo.mp4 (119.8 s, 1920x1080, narrated walkthrough: connection map → power tree → must-fixes → DRC/ERC evidence → bring-up → sign-off). Voiceover: Kokoro af_heart, 6 scene-paced lines (vo-s1..s6.txt, WAVs in composition/assets/). Poster: assets/demo/pcb-demo.jpg (S4 evidence frame, also baked as frame 0). Caption: assets/demo/share-copy.txt. Plan/brief: brag-plan.md, composition-brief.md. Composition source: assets/demo/composition/ (npx hyperframes check 0 errors).

Parts

38
QtyValueFootprintReferences
4M3MountingHole:MountingHole_3.2mm_M3H105, H105, H195, H195
3100nCapacitor_SMD:C_0805_2012MetricC3, C4, C5
310kResistor_THT:R_Axial_DIN0207_L6.3mm_P7.62mm_HorizontalR2, R3, R6
21kResistor_THT:R_Axial_DIN0207_L6.3mm_P7.62mm_HorizontalR1, R5
11000u_10VCapacitor_THT:CP_Radial_D12.5mm_P5.00mmC2
118kResistor_THT:R_Axial_DIN0207_L6.3mm_P7.62mm_HorizontalR4
11N4148Diode_THT:D_DO-35_SOD27_P7.62mmD1
12N2222Package_TO_SOT_THT:TO-92_InlineQ1
1470u_10VCapacitor_THT:CP_Radial_D10.0mm_P5.00mmC1
1500mAFuse:Fuseholder_Cylinder-5x20mm_ContactPitch15.24mm_HorizontalF1
1BUZZERConnector_JST:JST_XH_B2B-XH-A_1x02_P2.50_VerticalJ7
1GPS_GYNEO6MV2Connector_JST:JST_XH_B4B-XH-A_1x04_P2.50_VerticalJ2
1GSM_DIV_BYPASSConnector_PinHeader_2.54mm:PinHeader_1x03_P2.54_VerticalSJ1
1GSM_SIM800LConnector_PinHeader_2.54mm:PinHeader_1x06_P2.54_VerticalJ3
1MOTOR_SIG_P169Connector_PinHeader_2.54mm:PinHeader_1x07_P2.54_VerticalJ4
1PIEZO_12MMBuzzer_Beeper:Buzzer_12x9.5RM7.6_P7.6mmBZ1
1PWR_GREENLED_THT:LED_D5.0mmLED1
1Pi_Ribbon_2x20Connector_IDC:IDC-Header_2x20_P2.54_VerticalJ1
1SMBJ5.0ADiode_SMD:D_SMBTVS1
1TP1TestPoint:TestPoint_THTPad_D2.0mmTP1
1TP2TestPoint:TestPoint_THTPad_D2.0mmTP2
1TP3TestPoint:TestPoint_THTPad_D2.0mmTP3
1TP4TestPoint:TestPoint_THTPad_D2.0mmTP4
1TP5TestPoint:TestPoint_THTPad_D2.0mmTP5
1TP6TestPoint:TestPoint_THTPad_D2.0mmTP6
1TP7TestPoint:TestPoint_THTPad_D2.0mmTP7
1TP8TestPoint:TestPoint_THTPad_D2.0mmTP8
1TP9TestPoint:TestPoint_THTPad_D2.0mmTP9
1VBATT_INConnector_BarrierStrip:BarrierStrip_1x02_P5.08J5
1VGSM_INConnector_BarrierStrip:BarrierStrip_1x02_P5.08J6

Similar boards

  • 2 layers114 × 56.6 mmProbeBoardPublicV5, the printed circuit board in 3D

    ProbeBoardPublicV5

    novintic/FlukeEmu-FluCom

    HW/SW solution for Fluke 9010 mainframe emulation

    76 parts27GPL-2.0
  • 2 layers60 × 100 mmEsp gps ntp, the printed circuit board in 3D

    Esp gps ntp

    liebman/esp32-gps-ntp

    This is an esp-idf app using platformio.

    28 parts22MIT
  • 2 layers100 × 120 mmDcc station, the printed circuit board in 3D

    Dcc station

    cc90202/DCC-esp32

    DCC command station for ESP32-C6 — NMRA-compliant model railroad controller in Rust

    82 parts12
  • 4 layers43 × 66 mmWookey, the printed circuit board in 3D

    Wookey

    wookey-project/hard-wookey-motherboard

    WooKey Secure Mass Storage Mainboard PCB

    90 parts10
  • 4 layers85 × 60 mmKeithleyUpgrade, the printed circuit board in 3D

    KeithleyUpgrade

    asanza/keithley_199

    Upgrades for an old Keithley 199 multimeter

    75 parts8GPL-3.0
  • 2 layers39.4 × 43.2 mm3-roll, the printed circuit board in 3D

    3-roll

    DIY-Nabra/nabrafootprints

    KiCAD footprints for the symbols used in Ciat-Lonbarde paper circuits

    18 parts5BSD-2-Clause
  • 2 layers40.1 × 109.9 mmDemiurge, the printed circuit board in 3D

    Demiurge

    AwesomeAudioApparatus/demiurge

    Demiurge is a combination of Hardware and Software for Digital Sound Processing in the Eurorack Modular Synthesizer environment.

    155 parts4Apache-2.0

Questions

How big is the PotholeCart Expansion PCB?

It measures 100 × 80 mm and has 2 copper layers, 1.6 mm thick.

What parts does the PotholeCart Expansion use?

38 parts, built around the SMBJ5.0A and TP1. 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 PotholeCart Expansion KiCad files?

From the thrishunchand-fpga/potholecart-pcb repository on GitHub, at the commit this page was made from: the board is PotholeCart_Expansion.kicad_pcb and its schematic PotholeCart_Expansion.kicad_sch. PCBKit opens the board in the browser, with nothing to install.

Can I use the PotholeCart Expansion design in my own project?

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