KiCad — Tutorial¶

Five levels, each one a complete project. Don't skip levels; each introduces a constraint the next assumes you've internalized. The point is finished boards, not pristine ones — every level ends with Gerbers you could send to a fab.

Level 1 — Blinking LED¶

Goal: end-to-end pipeline on the smallest possible circuit.

Circuit: Coin cell → slide switch → resistor → LED → back to coin cell.

What you'll learn: the four operations from Quickstart, but for real — with through-hole footprints sized for an actual battery holder you can buy, traces wide enough to be hand-solderable, and a board outline.

Steps:

1. Schematic: BAT_HLD_CR2032, SW_SPDT, R 470Ω, LED. Wire them. ERC clean.
2. Footprint assignments: real parts you can find on Digi-Key or LCSC. BatteryHolder_Keystone:BatteryHolder_Keystone_3000_1x12mm is a real battery holder.
3. PCB: drop a 50 × 25 mm rectangle on the Edge.Cuts layer. Place the parts inside.
4. Route 0.4 mm tracks on F.Cu. Two layers is overkill for this — leave B.Cu empty or fill it with a GND zone.
5. DRC clean. Export Gerbers + drill files: File → Plot. Send the zip to JLCPCB or PCBWay if you want; their cheap option is ~$5 for 5 boards.

Stop conditions: ERC clean, DRC clean, Gerbers exported, 3D viewer looks like a circuit.

Level 2 — Microcontroller dev board¶

Goal: a real digital board with a regulator and a chip.

Circuit: USB-C connector → 5V → AMS1117-3.3V LDO regulator → ATtiny85 / ATmega328 / RP2040 (pick one) → status LED + reset button + ICSP/SWD header.

What you'll learn:

• Decoupling caps — every IC needs 100 nF as close to its power pins as physically possible. This is non-negotiable.
• Net classes — make a Power class with wider tracks (0.6 mm) and stricter clearance.
• 2-layer routing with a ground pour — F.Cu for signals, B.Cu as a solid GND plane filled with Add Filled Zone.
• SMD pads — most modern parts are 0805 or smaller. You'll need to learn to place them by typing exact coordinates.
• Hierarchical labels — when the schematic gets > ~30 components, split it into sheets.

Steps:

1. Draft the power section first. ERC the partial schematic.
2. Add the MCU. Decoupling caps within 5 mm of every power pin.
3. Programming header on the edge of the board for cable clearance.
4. PCB: place the MCU first (it's the busiest), then everything radiates outward. USB-C goes on a board edge.
5. Route signals on F.Cu, leave B.Cu as a continuous GND pour. Use vias to stitch GND.
6. DRC. Order the board.

Stop conditions: the board powers up without smoke when you plug in USB.

Level 3 — Mixed-signal board¶

Goal: stop pretending PCBs are 2D.

Circuit: MCU + microphone preamp (op-amp + filter) + audio output (PWM through low-pass) — or any analog block of your choosing. The point is one analog domain, one digital domain, on the same board.

What you'll learn:

• Star grounding / split planes / single-point connection — analog GND and digital GND are the same net in KiCad, but you control where they meet on the board. Get this wrong and your audio path picks up MCU clock harmonics.
• Differential pairs (skim) — KiCad's tuned routing for things like USB D+/D−, even at low speeds it doesn't hurt to learn.
• Component placement strategy — analog parts on one side of the board, digital on the other, single bridge between the GND pours.
• Net classes for analog vs digital — different track widths, different clearances.

This is also the level to start using the Schematic hierarchy. Make the analog block its own sheet so it's reusable.

Stop conditions: the analog signal is recognizable on a scope without obvious 1 MHz hash riding on it.

Level 4 — Multi-layer board (4 layers)¶

Goal: stackup awareness. Most "professional" boards are 4-layer; the cost premium is small (~2× of 2-layer at JLCPCB) and it eliminates an entire class of routing problems.

Project ideas: a USB-PD trigger board, a bigger MCU board with an external crystal and a few ICs, an LED matrix driver.

What you'll learn:

• Stackup design — Board Setup → Board Stackup → Physical Stackup. Set the manufacturer's stackup (JLCPCB has fixed 4-layer stackups; you don't pick layer thicknesses, you pick from their menu).
• Power and GND planes as their own layers — F.Cu (signals), GND (plane), Power (plane), B.Cu (signals). This is the standard 4-layer recipe and it solves a huge amount of EMI and decoupling weirdness.
• Vias as a first-class layout tool — once you have a GND plane, every component drops a via to GND right at its pad. No more "running a GND track halfway across the board."
• Impedance — for any high-speed line (USB, HDMI, DDR), trace width is determined by stackup, not by intuition. Use the Saturn PCB Toolkit or your fab's impedance calculator.

Stop conditions: the board works the first time. (At Level 4 it usually does, because power integrity is no longer fighting you.)

Level 5 — Custom symbols, footprints, and a board you'd put in a product¶

Goal: the part you need isn't in the standard library. Make it yourself, correctly.

What you'll learn:

• Symbol Editor: draw a new schematic symbol from a part datasheet. Pin numbers MUST match the manufacturer's package. Add a description, datasheet URL, and at least one MPN to the symbol fields.
• Footprint Editor: lay out pads from the datasheet's "Recommended Land Pattern." This is the most error-prone step in PCB design — get it wrong and the part doesn't fit. Use IPC-7351 recommended land patterns when the datasheet doesn't specify one.
• 3D model linking: download a STEP file from the manufacturer (or GrabCAD) and link it to the footprint so the 3D viewer is accurate.
• Design for manufacturing (DFM): silkscreen polarity marks, designators readable on the assembled board, fiducials if you're going to PCBA, panelization if you're ordering quantity.
• BOM and pick-and-place files for assembly: Tools → Generate Bill of Materials and File → Fabrication Outputs → Component Placement.

Project idea: a small product. A dev tool, a USB gadget, a custom keyboard PCB, a sensor board. Something you'd be willing to put in a case and use for a year.

Stop conditions: you assemble the board (or pay JLCPCBA to assemble it), it works, and you'd be willing to send the design files to another person without embarrassment.

After Level 5¶

You're not "done" — but the marginal value of more tutorials is low. Pick a real problem and design a board for it. Topics to dig into when relevant:

• High-speed routing: length matching, controlled impedance, return paths.
• RF: antenna keep-outs, ground stitching, microstrip vs. CPW.
• Power supplies: switcher layout (current loops!), thermal vias, copper area for heat dissipation.
• Flex / rigid-flex: when your product needs to bend.
• Scripting KiCad: the Python API for batch operations and custom DRC checks.

The Learning page has resources for each.