From idea to Gerbers: the workflow

A printed circuit board is just a flat sandwich that holds components in place and connects them with copper instead of wires. Designing one looks intimidating until you see that the whole job is a pipeline of five small steps, each with a clear check at the end. In this course you will walk that pipeline once, with a real project: a small ESP32-C3 board with a USB-C connector, one LED, one push button and two rows of pin headers. By lesson 5 you will have a folder of files you could upload to a factory today.

What a PCB is made of

A standard two-layer board is built from a few thin layers glued together:

The copper starts as a solid sheet on both faces. The factory etches away everything that is not a trace, pad or pour. Soldermask then covers the whole board except the pads, so solder sticks only to metal you meant to solder. Silkscreen is printed last and carries no electrical meaning, but it is what lets a human assemble and debug the board.

Why 1.6 mm FR4? It is the cheapest, most common stack, so every fab can make it, every connector footprint assumes it, and it is stiff enough that a USB plug will not bend it. Thin 0.8 mm boards exist, but you only pay for them when you need them.

Drag to orbit

Blue pins: analog inputs. Orange pins: digital I/O.

Layers inside KiCad

KiCad draws each physical layer, and a few helper layers, separately:

• F.Cu and B.Cu: front and back copper. Your traces live here.
• F.Mask and B.Mask: openings in the soldermask. A shape drawn here means "no lacquer, bare metal".
• F.Silkscreen and B.Silkscreen: text and outlines.
• F.Paste: where solder paste goes if you use a stencil for reflow.
• Edge.Cuts: the board outline. The factory routes the board along this line.

A two-layer board is plenty for this project. Four layers (two inner copper planes for power and ground) become useful when you have fast signals or dense BGA chips, not for a breakout like ours.

The five-step workflow

1. Schematic. Draw the circuit as symbols and wires. No sizes, no positions, only connections. This is where you decide what the board does.
2. Footprints. Give every symbol a physical land pattern: the exact copper pads where the real part will be soldered.
3. Layout. Draw the board outline, place footprints, then route copper traces between pads.
4. Checks. Run the Electrical Rules Checker (ERC) on the schematic and the Design Rules Checker (DRC) on the board. Look at it in 3D.
5. Fabrication files. Export Gerber files (one per layer) and drill files, zip them, upload them to a fab such as JLCPCB or PCBWay.

The order matters because each step locks in decisions for the next. A wrong footprint discovered during routing costs an hour. A wrong footprint discovered after the boards arrive costs two weeks and a few dollars of wasted boards. The checks exist so that mistakes are found as early and as cheaply as possible.

Our project

You will design a board around an ESP32-C3-MINI-1 module. Why a module and not the bare chip? The module already contains the chip, flash memory, crystal and a tuned antenna, so the radio part is solved. Our board only needs to supply it with 3.3 V and give it something to talk to.

• USB-C connector for 5 V power and native USB (the ESP32-C3 has USB built in, so no separate USB-to-serial chip).
• A 3.3 V regulator to turn 5 V into the module's supply.
• One LED and one button on spare GPIO pins.
• A BOOT button and reset circuit so you can program it.
• Two 2.54 mm pin headers so you can reach the GPIOs with jumper wires.

Target size: about 40 mm by 25 mm, two layers, all passives 0603 so you can hand-solder them.

This is a good first project because every part of it teaches something reusable: power input, regulation, decoupling, a module with strapping pins, a USB data pair and simple user I/O. The same steps scale to boards ten times larger, only with more repetition and more care.

Installing KiCad

Download the stable installer from the official site, kicad.org. This course uses KiCad 8 or 9; menu names are nearly identical between them, and the few differences are noted as we go. The installer is a few gigabytes because it includes the symbol, footprint and 3D model libraries, which you want offline. It runs on Windows, macOS and Linux.

When you open KiCad you see the Project Manager. Create a project with File > New Project, name it esp32c3-breakout, and KiCad makes three files that matter: a .kicad_pro project file, a .kicad_sch schematic and a .kicad_pcb board. Double-click the schematic to open the Schematic Editor and the board to open the PCB Editor. A third and fourth tool, the Symbol Editor and Footprint Editor, are for managing library parts.

In the next lesson you will open that blank schematic and draw the first part of the circuit.