Hardware reference

Engineering notes for anyone modifying the board, respinning it, or reviewing it. For the student-facing guide see ../README.md.

• Design: campv2/ — KiCad 10.0, file format 20260206
• Title block: TechnoCamp2026 Circuitry Class — schematic rev B, board rev B, 2026-08-09
• Outline: 80.0 × 80.0 mm, rounded corners, 1.6 mm FR-4, 2 layers, HASL
• Assembly: 100 % through-hole, single-sided placement except U1 (bottom)
• Vias: none. Every net is routed on one layer or reaches the other through a through-hole pad.

1. What this board is

A passive carrier for an Arduino Nano. There is no active silicon on the PCB — no regulator, no level shifter, no protection. The board contributes:

1. A socket for the Nano and headers for four off-board modules,
2. Six current-limiting resistors for two RGB LEDs,
3. Three buttons wired for internal pull-ups,
4. A jumper that reconfigures the RGB LEDs between common-cathode and common-anode,
5. Power distribution via two copper pours.

Design intent is pedagogical: every net should be traceable by eye with a multimeter, and every part should be replaceable with a soldering iron.

2. Netlist

Extracted from campv2.kicad_pcb. Reference designators are as they appear on the silkscreen (see §7 — they differ from the schematic).

Power

VCC and +5V are separate nets. VCC is the raw screw-terminal input feeding the Nano's VIN pin through its on-board regulator; +5V is the regulated rail coming back out of the Nano and feeding the sensor modules. Nothing on the PCB bridges them.

Signals

Deliberately unconnected on the Nano: D0/RX, D1/TX (kept free so the USB serial link is never contended), D4, D7, D13, A2, A3, A6, 3V3, AREF, RESET. D13 is left free on purpose — it drives the Nano's on-board LED, which makes it a poor general-purpose output. SW1–SW3 pads 2 and 3 are the mechanically-linked halves of the tactile switches and carry no net.

That leaves D4, D7, A2, A3, A6 genuinely available for a rev C — five pins, two of which (A6, A7… note A7 is taken) are analogue-input-only.

3. Power topology

screw terminal U1 ──VCC──► Nano VIN ──[Nano's own 5 V regulator]──► Nano +5V ──┬─► DHT11
                                                                               ├─► MQ-7
       USB ─────────────────────────────────────────────────────────────────►  ├─► LCD
                                                                               └─► J5 pin 3

There is no reverse-polarity protection, no fuse and no ORing diode. USB and the screw terminal must not be connected simultaneously — the Nano's regulator output and the USB 5 V rail would be driven against each other. This is called out in the student README but is not enforced in copper, which is a legitimate criticism of the design and the first thing to fix in a rev C (a Schottky in series with VCC, or a P-FET ideal-diode).

Copper pours

Back silkscreen. Besides the two logos and the U1 polarity marks, B.Silkscreen carries the motto PER ASPERA AD ASTRA as a board-level gr_text at (72.25, 20), 2 mm high, 0.5 mm thickness, bold, left/bottom justified and mirrored. It clears H1 and H2 because those sit at x = 20.5 and x = 90.5 while the text spans roughly x = 40–72.

Three zones total. Because both rails are planes, no power tracks were routed: every module header, every LED cathode return and all four mounting-hole pads pick up their rail from the nearest plane. H1–H4 are MountingHole_Pad footprints with plated pads tied to GND, so metal standoffs bond the frame to ground.

Signal routing: 90 track segments, predominantly 1.0 mm wide with a few at 0.5 mm and 1.5 mm. That is far wider than the ~50 mA these signals carry; the width is chosen so the tracks are visible and probe-able by students, not for current capacity.

4. Design rules as shipped

From campv2.kicad_pro:

Every one of these is well inside the capability of the cheapest 2-layer service, which is the point — the board is meant to be ordered in class quantities from whoever is fastest, not whoever is most capable.

5. Repository conventions

Library resolution

Both library tables are project-relative and therefore machine-independent:

; campv2/sym-lib-table
(lib (name "easyeda2kicad") (type "KiCad")
     (uri "${KIPRJMOD}/../lib/lcsc/easyeda2kicad.kicad_sym"))

; campv2/fp-lib-table
(lib (name "easyeda2kicad") (type "KiCad")
     (uri "${KIPRJMOD}/../lib/lcsc/easyeda2kicad.pretty"))
(lib (name "production")    (type "KiCad")
     (uri "${KIPRJMOD}/../production"))

${KIPRJMOD} expands to the directory containing the .kicad_pro, so both entries resolve wherever the repository is cloned. Note the second footprint entry: the two logo footprints on B.Silkscreen were placed from a library nicknamed production, and the footprint instances inside campv2.kicad_pcb still carry that nickname, so the nickname has to stay exactly that. It points at the top-level production/ folder, which is where the .kicad_mod files live. That folder does not carry the conventional .pretty suffix; KiCad reads it anyway, but if you ever want it to be textbook-correct, rename it to production.pretty and change the URI to match — the nickname stays production either way.

3D model paths in the PCB likewise use ${KIPRJMOD}/../lib/3d/…, ${KIPRJMOD}/../lib/lcsc/… and ${KICAD10_3DMODEL_DIR}/…. No user-defined path variables are required.

If you add a library, add it to the project table, not the global one. A global entry works on your machine and breaks for everyone who clones the repository.

Adding a part from LCSC

pip install easyeda2kicad
# append the LCSC code (e.g. C2837020) to lcsc.txt, then:
python lcsc.py lcsc.txt ./lib/lcsc

This pulls the symbol, footprint and 3D model straight into lib/lcsc/, where the project tables already point. Codes currently in use:

Regenerating production files

The campv2/production/ outputs were generated by the KiCad Fabrication Toolkit plugin; its settings are stored in campv2/fabrication-toolkit-options.json. Re-running the plugin reproduces the gerber zip, bom.csv, positions.csv, designators.csv and netlist.ipc in one step.

Do not hand-edit anything in campv2/production/. It is generated output. If a value there is wrong, the schematic or the layout is wrong.

6. What lives in archive/

The earlier vector traces of the two silkscreen logos, and the PNG/JPG artwork they were made from, sit alongside the live ones in the top-level production/ folder. Only turin_logo2 and assotsiatsiya_logo are on the board.

7. Known issues

1 — Reference designators differ between the schematic and the PCB. The board was re-annotated in the layout editor without back-annotating the schematic. The link is intact — all 21 footprints still match their schematic symbols by UUID — but the visible names differ:

Everything else (R4–R9, SW1–SW3, U1, J5, H1–H4) matches.

⚠️ Do not run Tools → Update PCB from Schematic on this project without checking the preview. KiCad will rename the footprints back to the schematic's designators, which silently invalidates the silkscreen you have already had manufactured and every reference in bom.csv, positions.csv and the firmware comments.

The clean fix is to re-annotate the schematic to match the board (right-click each symbol → Properties, or Tools → Annotate with the PCB as the source), then run the update. That is a rev-C task; the shipped rev B is consistent with itself everywhere that matters — silkscreen, BOM, pick-and-place and firmware all use the PCB names.

2 — The MQ-7 pin legend on the schematic is transposed. The text annotation beside J4 reads, top to bottom, DOUT / AOUT / GND / VCC. Pins 3 and 4 are correct (GND, +5V), but pins 1 and 2 are the wrong way round: pin 1 is wired to A7, which on an ATmega328P in the Nano package is an analogue input with no digital input buffer at all and therefore can only be the sensor's analogue output. Pin 2 goes to D12, the digital output. The firmware has it right (PIN_MQ7_ANALOG = A7, PIN_MQ7_ALARM = 12); only the drawing's caption is wrong.

This is cosmetic — no copper is affected — but it should be corrected in the schematic before the next class, because a student reading the schematic will wire their MQ-7 module backwards. MQ-7 breakout modules also vary in pin order between suppliers, so check the silkscreen on the module itself.

3 — No power-input protection. See §3.

8. Ideas for a rev C

Ordered by how much they would improve the class, not by difficulty:

1. Reverse-polarity and ORing protection on VCC, so a student cannot cook a Nano by powering it from USB and the terminal at once.
2. Back-annotate the designators so the schematic and the board agree (§7.1), and fix the MQ-7 caption (§7.2).
3. Per-pin silkscreen labels on the DHT11, MQ-7 and LCD headers. The pin functions are currently only on the schematic; putting GND VCC SDA SCL next to the LCD header would remove the most common wiring mistake at the bench.
4. Break the five free pins out (D4, D7, A2, A3, A6) to a 1×5 header with a GND and a 5 V pin beside it, so students can add their own sensor.
5. Test points on +5V, VCC and GND — teaching multimeter use is much easier with somewhere to put the probe.
6. A DHT22-compatible footprint — same 3 pins, so this costs nothing but a silkscreen note.

9. Toolchain

Anything older than KiCad 9 cannot open these files.