From netlist to copper: four nouns
By the end of guide 2 you had a finished schematic, a netlist — the machine-readable list of which pin connects to which — and your parts roughly placed on the board outline. Now comes the moment the design stops being a diagram and becomes a physical thing: every wire in that netlist must turn into real copper that you can hold. To talk about that copper you need just four nouns, and the whole language of layout is built from them: the trace, the pad, the footprint, and the via.
Picture a town. A trace is a road: a thin strip of copper that carries current from one place to another. A pad is a parking spot: a small patch of exposed copper where a component's leg actually solders down. A footprint is the whole parking lot painted for one building — the complete set of pads (plus an outline and a name) that one specific part will land on. And a via is a stairwell: a plated hole that lets a trace leave one copper layer and continue on another. Get fluent in these four and the rest of layout is mostly arranging them well.
Footprints and pads: where a real part lands
A symbol on a schematic is an idea — 'a 10 k resistor goes here'. A footprint is its body made physical: the exact arrangement of pads that matches the real part's legs, drawn from the numbers in its datasheet. A footprint also carries a courtyard (a keep-out boundary so neighbours do not collide) and a silkscreen outline (the printed cartoon of the part you met in guide 1). If the pad spacing does not match the part's lead pitch by a fraction of a millimetre, the part will not sit down — and a wrong footprint is the single most painful beginner mistake, because you usually discover it only after the boards arrive.
Pads come in two great families, matching the two ways parts attach. A through-hole pad is a drilled, copper-plated hole with a ring of copper around it; the part's wire leg pokes through and is soldered on the far side. Through-hole parts are sturdy and forgiving to hand-solder, but they eat space on every layer the hole passes through. A surface-mount pad is a flat patch of copper on one face of the board; the part simply sits on top, its metal ends resting on the pads. Surface-mount parts are tiny, cheap in volume, and dominate every modern board — at the cost of being fiddly to place by hand.
Here is the subtlety that trips people: one logical part exists in many physical packages. A 10 k resistor might be a fat through-hole cylinder, or a surface-mount chip in an 0805, 0603, or 0402 size barely larger than a grain of sand. They are the same value on the schematic but utterly different footprints. So the footprint you choose must match the exact part you intend to buy — the one named in your bill of materials. Pick the package first, then drop the matching footprint; never the reverse.
Traces carry current, and width is not free
A trace is copper, and copper, though an excellent conductor, is not a perfect one — it has a little resistance set by its width, its length, and how thick the copper layer is. Copper thickness is quoted in ounces: '1 oz copper' means about 35 micrometres thick, the most common default. A handy figure is that 1 oz copper has a sheet resistance of roughly 0.5 milliohm per square, where a 'square' is any length of trace as long as it is wide. Stack the squares: a trace 0.25 mm wide and 50 mm long is 50 / 0.25 = 200 squares, so about 200 times 0.5 mΩ = 100 mΩ, or 0.1 ohm.
That 0.1 ohm sounds tiny until current flows. Push 0.5 A through it and the trace drops V = I times R = 0.5 times 0.1 = 0.05 V, and it dissipates P = I^2 times R = 0.25 times 0.1 = 0.025 W as heat in the copper itself. For a signal that carries microamps, none of this matters and a hair-thin trace is fine. For a power rail or a ground return carrying an amp or more, that voltage drop and self-heating are real: too thin a power trace sags the rail and warms up, exactly the kind of fault that hides until the board is under full load.
Rough trace-width guide (1 oz outer copper, ~10 C rise) --------------------------------------------------------- width approx. continuous current 0.25 mm ~ 0.7 A <- fine for signals 0.5 mm ~ 1.2 A 1.0 mm ~ 2.0 A <- a typical power rail 2.0 mm ~ 3.5 A --------------------------------------------------------- inner layers carry ~half (no air to cool them) higher copper weight (2 oz) carries more bigger allowed temp rise carries more THESE ARE ESTIMATES - use an IPC-2221 calculator to be sure
- Find the worst-case continuous current the trace must carry — read it from the part's datasheet or your own power budget, not a guess.
- Choose how much temperature rise you will allow (10 C is a common, conservative target) and your copper weight (1 oz unless you asked for more).
- Read the width from a chart or an IPC-2221 calculator. The table above is enough to start; the calculator is what you trust for the final number.
- Now check the voltage drop over the trace's full length with V = I times R. Heat may be fine while the drop is not — a long, thin 3.3 V rail can lose too much before it even reaches the far chip.
- Round up for margin. Copper is cheap and space is usually available; a power trace one size wider than the minimum is honest insurance, the derating habit from earlier rungs.
Vias and planes: using all the floors
A two-layer or multilayer board is a sandwich: copper layers separated by sheets of insulating FR-4 (guide 1's stackup). A via is the elevator between those floors — a small drilled hole whose walls are plated with copper, electrically joining the layers it touches. With vias a trace that hits a traffic jam on the top layer can dive down, run across on the bottom layer where it is clear, and pop back up to finish. On a multilayer board this freedom is what lets dense designs route at all.
Once you can move between layers, you stop thinking only in skinny roads. Flood a whole region of a layer with solid copper and you have a copper pour; give a layer over almost entirely to one net and you have a plane — a ground plane or a power plane. A plane offers every chip a fat, nearby, low-impedance connection back to ground or up to the supply, instead of a long thin trace. This is why a decoupling capacitor stitched straight into a ground plane works so well, and it is the heart of the next guide.
Be honest, though: a via is not free. Each one adds a little resistance and a little inductance, takes up space, and punches a hole through any plane it passes (which can break a return path you were relying on). One via easily carries a signal, but a high-current rail wants several vias in parallel, and a hot part dumps its heat down a cluster of thermal vias into an inner plane or a heat sink below. Vias are tools, not confetti — use as many as you need and no more.
The layout itself is a circuit element
Here is the honest heart of this whole rung. Every trace is also, quietly, a tiny resistor, a tiny inductor, and a tiny capacitor with respect to its neighbours — its parasitics. At DC and low speed you may ignore them and the copper is 'just wire'. But push the frequency up and the copper's shape starts to matter as much as the part values: a fast enough edge sees a trace as a controlled-impedance transmission line with its own characteristic impedance, and a mismatch there throws part of the signal back as a reflection — the topic of the AC/RF rung and the next guide here. The same drawing that is fine at 1 kHz can ring and misbehave at 100 MHz.
That single truth is where every layout reflex comes from. Keep current loops small, because loop area is inductance. Put each decoupling capacitor right at its chip's pins, so the fast current never travels far. Keep noisy returns separate from quiet ones. Hold controlled impedance on fast nets. Pour fat copper and stitch thermal vias under anything that heats. The schematic fixes none of this — two engineers handed the same netlist can produce one board that works and one that does not, purely in the layout. The copper is not a wiring afterthought; it is a component you design.