The plan
A printed circuit board (PCB) starts as a schematic: a wiring diagram. Each part is a symbol and each line is a net, a set of pins joined together. Ours: a microcontroller lights an LED through a resistor, powered at 3.3 V.
Each symbol is matched to a footprint: the copper pads its real part will be soldered to, spaced like its legs. The chip's legs are 1.27 mm apart. Thin lines called airwires show which pads must be joined.
Placement means choosing where each footprint sits inside the board outline, here 50 by 30 mm. Good placement keeps connected parts close, so their copper paths stay short. Watch the airwires stretch as the parts move.
Copper
Routing turns each airwire into a trace: a flat strip of copper on the board. Traces on the same layer must never touch, or they short together. The power trace and the signal traces run on the top layer.
A trace must be wide enough for its current, or it heats up. By the IPC-2221 design standard, a 0.25 mm outer trace in standard 35 µm copper carries about 0.9 A for a 10 °C rise. Our LED needs far less.
This board has two copper layers, top and bottom. A via is a small hole drilled through the board and plated with copper inside, so a connection can hop from one layer to the other. Each ground pin drops through a via.
The bottom layer is one big sheet of copper tied to ground: a ground plane. Every ground pin reaches it through a via, so return current has a short, wide path. The board is shown see-through so you can spot it.
Finishing
Each factory has limits, called design rules. A typical 2-layer service needs traces at least 0.15 mm wide, 0.15 mm apart, and holes at least 0.25 mm. The design rule check (DRC) scans the board and flags anything that breaks them.
Solder mask is a thin coloured coating over the copper, open only at the pads, so solder cannot bridge two traces. Silkscreen prints labels on top, such as U1 for the chip and R1 for the resistor.
Manufacturing
The design goes to the factory as manufacturing files. Each layer (top copper, bottom copper, solder mask, silkscreen) is saved as a Gerber file, and a drill file lists every hole. The factory builds the board from them.
Assembly: a stencil spreads solder paste on the pads, a pick-and-place machine sets each part on its pads, and an oven melts the paste. When it cools, every part is soldered in place.
Power on. Current flows from the 3.3 V header into the chip, out of pin 5, through the resistor and the LED, then back through a via to the ground plane. The LED lights: the schematic is now hardware.
In detail
;; step 1/12 · schematic Parts (reference names): U1 microcontroller, 8 pins (e.g. ATtiny85) R1 resistor (limits the LED current) D1 LED J1 2-pin power header, 3.3 V Nets: VCC J1+ -> U1 pin 8 LED U1 pin 5 -> R1 -> D1 GND J1-, U1 pin 4, D1 cathode
The drawing is not to scale: traces, pads and parts are enlarged so they read at lesson size. The 50 × 30 mm outline is a teaching choice. Pin numbers follow the ATtiny85 datasheet: pin 8 is VCC, pin 4 is GND and pin 5 is PB0; the SOIC-8 package has a 1.27 mm lead pitch. The ATtiny85 runs from 2.7 to 5.5 V, so 3.3 V is in range. Trace current uses the IPC-2221 curve fit published by Advanced Circuits (outer layer, k = 0.048, 1 oz = 1.378 mil of copper): 0.25 mm ≈ 0.88 A and 0.5 mm ≈ 1.45 A for a 10 °C rise. IPC-2152 is the newer standard; it gives different values. Design rules are OSH Park's 2-layer limits: 6 mil (0.15 mm) trace and space, 10 mil (0.25 mm) drill, 1.6 mm board, 1 oz copper. Other factories publish their own.