Making a printed circuit board takes ten steps: write down the circuit, draw it, check it, give every part a footprint, lay out the board, route it, check it again, export the files, order, and assemble. Each step below is shown on a real board generated in PCBEditor (the browser PCB tool I work on). The mistakes are left in, because seeing a mistake once is the fastest way to stop making it.
Short answer: to make a PCB, draw the circuit as a schematic and give each part a footprint (its pad layout). Then place the parts on a board outline, connect them with copper traces and run a design-rule check. Export the Gerber and drill files, check them in a viewer, and upload the zip to a PCB manufacturer, which makes the bare boards in a few days. Then solder the parts on, or order assembly with a parts list and a pick-and-place file. All of the design steps can be done free in a browser.
1. Write down what the board must do
Before drawing anything, write one paragraph: what the board does, what powers it (USB, a battery, a 12 V adapter) and how much current it draws, the main parts by part number, the connectors, and the size it must fit. Every number you leave out gets decided for you later, by you or by a tool, often badly. This paragraph is also exactly what an AI PCB tool needs as a prompt. The board in the next two steps started as this one:
Single-cell LiPo charger board: USB-C 5 V input, MCP73831 charger set to 500 mA, a charge status LED, a JST-PH 2-pin battery connector, and an AP2112K 3.3 V regulator output on a 3-pin header. 2-layer board.
2. Draw the schematic
The schematic is the circuit as a diagram: every part as a symbol, every connection as a wire or a shared net name. Draw it in a circuit diagram maker or an EDA tool, or describe it and let the AI draw a first version. If the symbols are new to you, the schematic symbols chart covers the common ones.
The generated schematic of the LiPo charger: USB-C input with 5.1 kΩ CC pull-downs, the MCP73831 with 2 kΩ on PROG (500 mA) and its charge LED on STAT, and the AP2112K 3.3 V regulator fed from the battery, out to a 3-pin header.
3. Check it against the datasheets
A schematic can be tidy and still wrong. Before any layout, check the parts that decide whether the board works:
- Power from the connector to every chip, and every supply against every part's absolute maximum rating.
- Reset, boot and enable pins, each with the pull-up or pull-down and capacitor the datasheet asks for.
- Special-function pins (I²C, SPI, UART, USB, ADC, crystal, programming header) on pins that have that hardware.
- Decoupling capacitors at the values the datasheet gives, one per supply pin.
This is where most mistakes hide. In our six-board test, four boards passed every automated check with a schematic mistake still in them: a reset button on a spare GPIO, an LED that could never flash. The whole review is in I Asked an AI to Design Six PCBs.
4. Give every part a footprint
A footprint is the pattern of copper pads the part is soldered to, plus its outline and courtyard (the keep-clear area around it). It must match the exact package you will buy: a resistor in 0603 and one in 0805 are the same symbol on two different footprints. Most parts have one in the KiCad libraries. For the rest, build one from the datasheet's land pattern with a footprint generator.
Pin 1 on the symbol must be pad 1 on the footprint. Transistors and regulators come in several pin orders in the same package. A footprint that fits the package but numbers its pads differently from the symbol gives you a board that cannot work, and no design-rule check will notice.
5. Set the outline, layers and rules
Draw the board outline, choose the layer count (two is enough for most boards) and enter the design rules your manufacturer can build: minimum trace width and spacing, minimum drill and via size, copper-to-edge distance. Then size the traces that carry real current; the trace width calculator gives the width for a current and a temperature rise.
6. Place the parts
Placement decides most of how a board performs. Put connectors on the edges, facing out. Put decoupling capacitors next to the pins they serve, and keep a radio module's antenna at the board edge with no copper under it. Then place the rest to keep the important connections short. The ESP32 board below passed every rule check in its first layout and still had its antenna over a ground pour. A review caught it, and one move fixed it.
The first layout: the module in the middle, with its antenna end (above the top row of pads) over R1, the regulator and a ground pour that covers the whole bottom layer. It passed DRC. The review caught it.
After the move: 21 parts on 32.6 × 44.1 mm, two layers, every net routed, 0 DRC errors. The module sits on the top edge so its antenna overhangs the board.
7. Route the traces
Routing turns each connection into copper. Route power first and wide, then the sensitive signals (crystal, USB pair, analog inputs) short and direct, then everything else. Fill the spare area with a ground pour. An autorouter does the bulk well once placement is good. Check what it did with critical signals, though.
The LiPo charger routed on two layers: 14 parts on 32.5 × 34.5 mm, USB-C on the top edge, the battery connector bottom left and the 3.3 V output header bottom right.
8. Run the design-rule check and a review
The design-rule check (DRC) compares the copper against your manufacturer's limits: clearances, widths, drills, unrouted connections, overlapping parts. Fix every error. Then review what DRC cannot see: the circuit, the connector orientation, the antenna keep-out.
The design-rule check on a motor driver board: 0 errors and 1 warning (a courtyard overlap), with the board's net classes, trace widths and clearances in the panel on the right.
A clean DRC is where the review starts, not where it ends. The first version of that motor driver board had zero DRC errors and the Arduino Nano's VIN pin unconnected, so the board went dark the moment the USB cable came out. DRC checks the copper against the netlist; it can't tell that the netlist is missing a connection.
9. Export and check the Gerbers
Export the Gerber files (one per layer) and the drill files, usually as one zip. If you want the boards assembled, also export the BOM and the pick-and-place file. Before uploading, open the zip in a Gerber viewer and look at each layer. It is the file the fab will build from, and the place where a missing outline or holes off the pads show up.
One export for every fab format: Gerber X2, Excellon drill, pick-and-place (CPL), BOM, IPC-D-356, IPC-2581, ODB++, assembly and fabrication PDFs, a STEP model and a KiCad board, in one zip.
10. Order, assemble and power up
Upload the zip to a PCB manufacturer and pick the options. The standard ones suit most boards: FR-4, 1.6 mm thick, 1 oz copper, HASL or ENIG finish, green solder mask. Budget prototype services usually make a minimum of five boards. For assembly, the same services can solder the parts from your BOM and pick-and-place file, or you solder them yourself, smallest parts first.
The first power-up:
- Inspect the board under good light for solder bridges, especially on fine-pitch chips.
- With a multimeter, check that no supply rail is shorted to ground.
- Power it from a bench supply with a low current limit, not straight from a battery or adapter.
- Measure each rail before you plug in modules or programme the microcontroller.
The assembled charger in the 3D view: USB-C receptacle, JST-PH battery connector, the 3-pin output header, and the charger and regulator between them.
Making a PCB at home
Simple boards can be made at home. Transfer the copper layout onto copper-clad board, with laser-printer toner ironed on or a photoresist film, etch away the bare copper in ferric chloride or a similar etchant, and drill the holes. It works for single-sided and simple double-sided boards with wide traces. You get no solder mask, no silkscreen and no plated holes, and the etchant stains, corrodes and must be disposed of properly. Ordered prototypes are now cheap and fast enough that most people etch only when they need a board the same day.
How many layers, and which software?
Two layers are enough for most hobby and small product boards, including microcontroller boards with USB. Four layers help with dense parts such as fine-pitch QFN or BGA chips, high-speed signals and boards that need a solid ground plane under every signal.
For software, any PCB design (EDA) tool will do: KiCad is free and runs on the desktop; PCBEditor runs in the browser and can also generate a first draft from a description. Both export the Gerber, drill and assembly files a fab needs.
The full guide, with every step and the figures at full size, is at pcbeditor.com/how-to-make-a-pcb.
What was the mistake on your first board? Of the six test boards, the one that taught me most was the ESP32: a clean design-rule check, and an antenna sitting over a ground pour.
Top comments (0)