Skip to content
LumenaryAcademy
Embedded 70 min

Printed circuit boards

From a schematic to a manufactured board that works, keeps quiet, passes its tests and is safe to sell.

Code tested · 5AI-draftedAwaiting review by an electrical engineer

Your guides: Chloe · The Physicist, Margaret · The Bench Engineer, Gideon · The Design Reviewer

MotivationH

From a breadboard to a product

Every circuit in Lumenary EE so far could be built on a breadboard: plug in parts, add wires, measure. A breadboard is wonderful for learning and hopeless for a product. Its contacts loosen, its long wires act as antennas and inductors, it falls apart in a pocket, and it cannot hold a chip with a hundred pins spaced half a millimetre apart. Almost every electronic product is instead built on a printed circuit board (PCB): layers of copper patterned into conductors, laminated with insulating glass-epoxy, drilled, plated and coated, with components soldered to its surface by machine.

A PCB is not just a tidy way to connect parts. At the speeds of modern electronics, every copper trace is itself a component, with resistance, inductance and capacitance, and a board designed carelessly will drop voltage, ring, radiate radio noise or fail its certification tests. This lesson follows a board from schematic to finished product and explains the physics that decides whether it works: current and heat, decoupling, return paths and impedance, electromagnetic compatibility, manufacture, and safety. Designing a board is now open to anyone with a laptop: the tools are free, and fabricators in many countries make small batches cheaply.

DefinitionsH

From schematic to layout

Definition— Schematic, netlist, footprint, layout

A schematic is the circuit drawn as symbols and connections; each set of connected pins is a net. The netlist lists every component and every net. A footprint is the pattern of copper pads (and holes, outlines and markings) on which one physical component is soldered. The layout places the footprints on the board and draws the copper that realises every net, on one or more layers.

1. Schematicsymbols, nets, ERC2. Footprintsand netlist3. Placementboard outline, parts4. Routingtraces, vias, planes5. DRC and reviewfab rules, checklists6. OutputsGerber, drill, BOM,pick-and-place → fab
The design flow of a printed circuit board. Each arrow is a check point: an electrical rules check on the schematic, a design-rules check against the fabricator's capabilities on the layout, and a review of the manufacturing files before ordering.

The flow runs like this. Draw the schematic and run the electrical rules check (ERC), which catches outputs wired together and pins left unconnected. Assign a footprint to every symbol, checking each against the part's datasheet, since a footprint that is mirrored or a pin off produces a board that can never work; land patterns follow the conventions of IPC-7351. On the board, draw the outline and mounting holes, then place the parts. Placement decides most of the outcome: connectors at the edges, decoupling capacitors next to their pins, the crystal next to the microcontroller, noisy switching circuits away from sensitive analogue inputs, and short paths for the signals that matter. Then route the copper, run the design rules check (DRC) against the fabricator's minimum trace widths, spacings and drill sizes, review, and generate the outputs: Gerber files (one per copper, mask and silkscreen layer), a drill file, the bill of materials (BOM) and a pick-and-place file giving each part's position and rotation for the assembly machine.

IntuitionH

Layers, traces and vias

The usual board material is FR-4, woven glass fibre in flame-retardant epoxy, about 1.6 mm thick in total. Copper thickness is quoted as weight per area: 1 oz copper (one ounce per square foot) is about 35 µm thick, and 2 oz about 70 µm. A two-layer board has copper on both faces; a four-layer board adds two inner layers, separated by a central core and bonded on each side by prepreg (glass cloth with partly cured resin). A solder mask (usually green, but any colour) covers the copper except at pads, so solder stays where it belongs; a silkscreen prints the labels; and a surface finish protects the exposed pads — lead-free hot-air levelled solder (HASL), electroless nickel immersion gold (ENIG) for flat fine-pitch pads, or an organic coating (OSP).

solder masktop copper: signalsprepreg (≈ 0.2 mm)inner 1: ground planecore (≈ 1.1 mm)inner 2: power planeprepregbottom copper and maskviatracedashed: the trace's return current, in the plane just beneath it
Cross-section of a common four-layer stack-up (not to scale). Signals run on the outer layers; the first inner layer is a solid ground plane directly under the top signals, so each top trace and the plane form a controlled transmission line, and its return current flows in the plane just beneath it. A plated through-hole via joins the top and bottom layers, with clearance holes (antipads) where it passes through the planes.

Vias connect layers. The common plated through-hole via is a drilled hole, typically 0.2 to 0.4 mm, copper-plated inside, running through the whole board. Dense boards use blind vias (from an outer layer to an inner one), buried vias (between inner layers) and laser-drilled microvias, at extra cost. A via is not free electrically: it adds roughly a nanohenry of inductance and a fraction of a picofarad, and carries only so much current, so power connections use several in parallel. Four layers cost more than two, but for any board with a fast microcontroller or a radio they are usually worth it, because a solid ground plane solves more problems than any other single decision.

ComputationC

How wide should a trace be?

A trace is a resistor: R=ρL/(wt)R = \rho L / (w t), with copper's resistivity ρ≈1.72×10−8 Ω m\rho \approx 1.72 \times 10^{-8}\ \Omega\,\mathrm{m} at 20 °C, rising about 0.39% per kelvin. The current heats it by I2RI^2R, and the voltage drop IRIR is lost to the load. The program computes both for a 50 mm trace carrying 2 A.

python
RHO_CU = 1.72e-8            # resistivity of copper at 20 C, ohm metres
ALPHA = 0.0039              # its temperature coefficient, per kelvin
OZ = 35e-6                  # "1 oz" copper (one ounce per square foot) is about 35 micrometres thick

def trace(width_mm, length_mm, oz, current, temp_c=20.0):
    """Resistance, voltage drop and heat of a straight copper trace."""
    area = width_mm * 1e-3 * oz * OZ
    r = RHO_CU * (1 + ALPHA * (temp_c - 20)) * (length_mm * 1e-3) / area
    return r, current * r, current**2 * r

print("A 50 mm trace carrying 2 A:")
print(" width   copper   resistance   drop      heat     current density")
for w, oz in [(0.25, 1), (0.5, 1), (1.0, 1), (2.0, 1), (1.0, 2)]:
    r, v, p = trace(w, 50, oz, 2.0)
    j = 2.0 / (w * oz * OZ * 1e3)          # amps per square millimetre
    print(f"{w:5.2f} mm  {oz} oz  {r * 1e3:8.1f} mOhm {v * 1e3:7.1f} mV {p * 1e3:7.1f} mW {j:9.0f} A/mm2")

# The legacy IPC-2221 chart, as its widely quoted curve fit: I = k * dT^0.44 * A^0.725,
# with A the cross-section in square mils and k = 0.048 for outer layers. IPC-2152 replaced
# the chart with measurements; use this only as a first, rough estimate.
def legacy_width_mm(current, rise_c, oz, k=0.048):
    area_mil2 = (current / (k * rise_c**0.44)) ** (1 / 0.725)
    thickness_mil = oz * OZ / 25.4e-6
    return area_mil2 / thickness_mil * 0.0254

print("\nRough outer-layer width for a 10 C rise (legacy curve fit, 1 oz copper):")
for amps in (0.5, 1, 2, 3, 5):
    print(f"  {amps:3} A -> {legacy_width_mm(amps, 10, 1):.2f} mm")
Runs entirely in your browser, in an isolated worker. Nothing is sent to a server.

A 0.25 mm trace, fine for signals, drops 0.2 V and dissipates 0.4 W at 2 A: on a 3.3 V rail that drop alone is 6% of the supply. Doubling the width or the copper weight halves both. How hot the trace gets is harder, because it depends on where the heat goes: into the board, into nearby copper planes, into the air. The old chart in IPC-2221, from measurements made decades ago, related current, cross-section and temperature rise; its widely quoted curve fit is the second table, and many calculators, including the one built into KiCad, still use it. IPC-2152 (2009) replaced it with new measurements that account for board thickness and material, copper weight, and above all nearby copper planes, which spread heat and let traces run much cooler than the old chart assumed — especially inner traces, which the old chart treated very conservatively. Treat any single formula as a first estimate, prefer copper pours and planes for currents of amps, use several vias to change layers, and check the temperature rise of a prototype with a thermal camera or a thermocouple.

ComputationC

Decoupling capacitors and ground planes

A digital chip draws current in sharp spikes: every clock edge, thousands of transistors switch at once for a fraction of a nanosecond. The regulator is centimetres away, behind traces with nanohenries of inductance, and V=L dI/dtV = L\,dI/dt is merciless: 10 nH carrying a current that rises by 0.1 A in 1 ns develops 1 V. Decoupling capacitors (or bypass capacitors) next to each supply pin supply that charge locally, so the spikes circulate in a tiny loop between the capacitor and the chip instead of across the board.

A real capacitor is a series RLC circuit (RLC circuits): its capacitance, its equivalent series inductance (ESL, from the package, pads and vias) and its equivalent series resistance (ESR). Below its self-resonant frequency f0=1/(2πLC)f_0 = 1/(2\pi\sqrt{LC}) it behaves as a capacitor; above it, as an inductor. Designers aim to keep the impedance of the supply network, seen from the chip, below a target impedance Zt=V×(allowed ripple)/(current step)Z_t = V \times (\text{allowed ripple}) / (\text{current step}) at every frequency the chip's current contains.

python
import numpy as np

# A real capacitor is a series R-L-C: its plates (C), its leads, pads and vias (L, "ESL"),
# and its losses (R, "ESR"). Values are typical for small ceramic parts once mounted.
CAPS = {
    "10 uF":  (10e-6,  2.0e-9, 0.005),
    "1 uF":   (1e-6,   1.5e-9, 0.010),
    "100 nF": (100e-9, 1.0e-9, 0.030),
}

def z(f, c, l, r):
    w = 2 * np.pi * f
    return r + 1j * (w * l - 1 / (w * c))

V, RIPPLE, STEP = 3.3, 0.03, 0.5            # supply, allowed ripple (3%), load step (A)
z_target = V * RIPPLE / STEP
print(f"target impedance = {V} V x {RIPPLE:.0%} / {STEP} A = {z_target * 1e3:.0f} mOhm\n")

for name, (c, l, r) in CAPS.items():
    print(f"{name:>7}: self-resonant at {1 / (2 * np.pi * np.sqrt(l * c)) / 1e6:6.2f} MHz, where |Z| = ESR = {r * 1e3:.0f} mOhm")

freqs = [1e5, 1e6, 3e6, 1e7, 3e7, 1e8, 3e8]
print(f"\n{'f (MHz)':>8} " + " ".join(f"{n:>9}" for n in CAPS) + "   all three in parallel")
for f in freqs:
    zs = [z(f, *v) for v in CAPS.values()]
    zp = 1 / sum(1 / x for x in zs)
    cells = " ".join(f"{abs(x) * 1e3:7.0f} m" for x in zs)
    flag = "ok" if abs(zp) <= z_target else "too high"
    print(f"{f / 1e6:8.1f} {cells}   {abs(zp) * 1e3:7.0f} mOhm  {flag}")

# Between two self-resonances the parallel combination peaks (an anti-resonance):
f = np.logspace(5, 9, 4001)
mag = np.abs(1 / sum(1 / z(f, *v) for v in CAPS.values()))
peaks = [i for i in range(1, len(f) - 1) if mag[i] > mag[i - 1] and mag[i] > mag[i + 1]]
for i in peaks:
    print(f"anti-resonance peak: {mag[i] * 1e3:.0f} mOhm at {f[i] / 1e6:.2f} MHz")
Runs entirely in your browser, in an isolated worker. Nothing is sent to a server.

Three common values in parallel keep this 3.3 V rail below its 198 mΩ target from 100 kHz to beyond 30 MHz, with modest anti-resonance peaks where one capacitor has turned inductive and the next is still capacitive. Above about 100 MHz every capacitor is an inductor and no board-level part can help; there the chip relies on capacitance inside its own package and silicon. Two lessons follow. The inductance, set by the package size and above all by the mounting — short, wide connections, a via straight down to the plane, the capacitor right at the pin — matters more than the capacitance. And the classic recipe of "100 nF per supply pin plus a bulk capacitor" works because it spreads resonances across the range where a microcontroller's currents live.

Ground planes do for the whole board what decoupling does for one chip. A solid copper layer gives every signal and every supply current a low-impedance path home, gives every trace above it a defined impedance, and shields one side of the board from the other. Splitting the ground plane into "analogue" and "digital" halves was once common advice; with modern mixed-signal parts, a single solid plane with careful placement — analogue parts and their traces kept away from the digital switching currents — is usually better. The rule that matters is the next section's: never make a return current go the long way round.

Worked examplesH

Signal integrity: return paths, impedance and crosstalk

Current flows in loops. Every signal trace carries current out, and the same current must come back. At DC the return spreads out along the path of least resistance; above a few tens of kilohertz it follows the path of least inductance, which is the path that encloses the smallest loop area: directly under the trace, in the nearest plane. A small loop has low inductance, radiates little and picks up little.

solid planeplane with a slotsignalreturn, just beneathreturn detoursaround the slotdriverreceiver
Return current seen from above. Left: over a solid plane, the return current flows directly beneath the trace and the loop is tiny. Right: a slot in the plane under the trace forces the return current to detour around the end of the slot, creating a large loop that radiates, picks up noise and adds inductance.

So: route fast signals over an unbroken plane; do not run them across gaps, slots or the boundary between two planes; when a signal changes layers and therefore reference planes, put a ground via (or a capacitor between the planes) beside the signal via so the return current can follow; and keep every high-current switching loop, such as a switching regulator's (Power supplies and noise), as small as possible.

When is a trace a transmission line? A signal edge travels along the board at roughly half the speed of light. Once a trace is long compared with the distance the edge travels during its rise time, the trace behaves as a transmission line: the edge sees the trace's characteristic impedance Z0Z_0, and if the load does not match it, part of the edge reflects and the signal rings. (Transmission lines, in the next level, develops the theory.) For a microstrip — a trace over a plane — Z0Z_0 depends on the trace width, the dielectric thickness and its permittivity. The program uses Hammerstad's classic closed-form approximations:

python
import math

C0 = 299_792_458.0           # speed of light, m/s

def microstrip(w, h, er):
    """Characteristic impedance (ohms) and effective permittivity of a thin microstrip:
    a trace of width w on a dielectric of thickness h over a plane (Hammerstad's closed forms)."""
    u = w / h
    if u <= 1:
        e_eff = (er + 1) / 2 + (er - 1) / 2 * ((1 + 12 / u) ** -0.5 + 0.04 * (1 - u) ** 2)
        z0 = 60 / math.sqrt(e_eff) * math.log(8 / u + u / 4)
    else:
        e_eff = (er + 1) / 2 + (er - 1) / 2 * (1 + 12 / u) ** -0.5
        z0 = 120 * math.pi / (math.sqrt(e_eff) * (u + 1.393 + 0.667 * math.log(u + 1.444)))
    return z0, e_eff

ER = 4.3                     # FR-4 glass-epoxy, roughly, at around 1 GHz
width_50 = {}
for h in (0.2, 1.5):         # outer layer of a 4-layer board; a 2-layer board 1.5 mm thick
    print(f"dielectric {h} mm thick:")
    for w in (0.1, 0.2, 0.3, 0.4, 1.0, 2.0, 3.0):
        z0, e_eff = microstrip(w, h, ER)
        print(f"   width {w:3.1f} mm -> Z0 = {z0:5.1f} ohm")
    lo, hi = 0.01, 10.0      # bisect for the 50-ohm width (Z0 falls as the trace widens)
    for _ in range(60):
        mid = (lo + hi) / 2
        lo, hi = (mid, hi) if microstrip(mid, h, ER)[0] > 50 else (lo, mid)
    width_50[h] = lo
    z0, e_eff = microstrip(lo, h, ER)
    print(f"   50 ohm needs a width of {lo:.3f} mm; e_eff = {e_eff:.2f}\n")

z0, e_eff = microstrip(width_50[0.2], 0.2, ER)
v = C0 / math.sqrt(e_eff)
print(f"signals travel at {v / C0:.2f} c = {v * 1e-9 * 100:.1f} cm per ns ({1e12 / v / 1000:.1f} ps per mm)")
print("rule of thumb: treat a trace as a transmission line if it is longer than about rise time x speed / 6")
for name, tr in [("slow logic, 10 ns edges", 10e-9), ("microcontroller GPIO, 2 ns", 2e-9),
                 ("USB 2.0 high speed, 0.5 ns", 0.5e-9), ("multi-gigabit link, 0.05 ns", 0.05e-9)]:
    print(f"   {name:28} {100 * tr * v / 6:6.1f} cm")
Runs entirely in your browser, in an isolated worker. Nothing is sent to a server.

Two conclusions stand out. On the outer layer of a four-layer board, with 0.2 mm of prepreg to the plane, a 50 Ω trace is about 0.39 mm wide, a comfortable width; on a 1.5 mm two-layer board it would be nearly 3 mm, which is why controlled-impedance designs need a close plane. And edges, not clock frequencies, decide when the line effects matter: a microcontroller pin with 2 ns edges needs care beyond about 5 cm even if it toggles only once a second. Interfaces that need controlled impedance specify it: 90 Ω differential for USB, 100 Ω differential for Ethernet, 50 Ω single-ended for most radio-frequency traces. The fabricator then adjusts the widths to hit the target on its actual materials, usually within ±10%, and a series termination resistor of a few tens of ohms at a fast driver tames reflections on short unmatched traces. Field-solver tools, free ones included, replace closed-form approximations for final designs.

Crosstalk is the coupling of one trace's signal into a neighbour through their mutual capacitance and inductance. It grows with the length of the parallel run and with edge speed, and falls quickly with spacing and with a closer reference plane. Rules of thumb: space fast traces at least three trace widths apart (the "3W rule"), run traces on adjacent layers at right angles, keep the plane close, and keep sensitive analogue inputs well away from clocks.

ExplanationH

EMC: why products are tested and certified

Every electronic product is, unintentionally, a radio transmitter and a radio receiver. Its clocks and switching regulators emit energy at their frequencies and harmonics, and its cables are antennas that pick up whatever is around. Electromagnetic compatibility (EMC) means that a product neither disturbs other equipment, from broadcast radio to aircraft navigation to a neighbour's pacemaker, nor is disturbed by its environment: electrostatic discharge from a finger, nearby transmitters, surges on cables. Because one badly designed product can interfere with services everyone relies on, governments require products to meet EMC limits before they may be sold.

Products are tested against two kinds of standard. Emissions tests measure radiated fields in a shielded, absorber-lined chamber or on an open-area test site, and conducted noise on power cables, against limits such as those of CISPR 32 for multimedia and IT equipment. Immunity tests subject the product to the IEC 61000-4 series: electrostatic discharges (61000-4-2), radiated radio fields (61000-4-3), fast transients and surges on cables (61000-4-4 and -5). The legal frameworks differ by market:

  • European Union: the manufacturer declares conformity with the EMC Directive (2014/30/EU), the Radio Equipment Directive (2014/53/EU) for anything with a radio, and the Low Voltage Directive (2014/35/EU) for electrical safety, usually by testing to harmonised standards, and applies the CE marking. The United Kingdom has the parallel UKCA marking.
  • United States: the FCC's Part 15 rules set limits for unintentional radiators (Class B for homes, stricter than Class A for commercial and industrial use) and require certification for intentional radiators such as Wi-Fi devices.
  • Elsewhere: ISED in Canada, MIC (radio) and VCCI (EMC) in Japan, KC in South Korea, CCC and SRRC in China, RCM in Australia and New Zealand, WPC and BIS in India, and many more.

Passing is designed in, not tested in: solid ground planes and short return paths, decoupling, slow edges wherever speed is not needed, spread-spectrum clocking, filtering and ESD protection at every connector where cables enter, a metal or coated enclosure where needed, and, for radios, a pre-certified module whose radio approvals the product can largely reuse. Teams rent time at a test laboratory for formal tests, but first find their problems cheaply with pre-compliance checks: a near-field probe and a spectrum analyser on the bench, a few weeks before the expensive chamber.

Worked examplesH

Design for manufacture, KiCad, and ordering boards

A board that works on the designer's bench must also be built a thousand times by machines without defects. Design for manufacture (DFM) and design for assembly (DFA) mean, among much else:

  • staying inside the fabricator's capabilities (for low-cost fabs, typically traces and spaces of at least 0.1 to 0.15 mm, drills of 0.2 to 0.3 mm, and an annular ring of copper around each hole);
  • thermal reliefs, spokes that join pads to planes so a soldering iron or reflow oven can heat the pad, and solder mask between fine-pitch pads so solder does not bridge them;
  • fiducial marks for the assembly machine's camera, parts placed with consistent orientation and clear polarity markings, components kept clear of the board edge and of each other's rework space;
  • tiny passive parts with symmetric pads and traces, so surface tension does not stand them on end ("tombstoning") during reflow;
  • test points on power rails and key signals, and the debug and JTAG connections of Microcontrollers, so every board can be programmed and tested in production (design for test);
  • preferring common, available parts, with second sources, over exotic ones.

KiCad is the open-source suite (GPL) that most hobbyists, many universities and a growing number of companies use for all of this: schematic capture, footprint and symbol libraries, a layout editor with interactive and differential-pair routing, a 3D viewer, design-rule checks, a calculator for track widths and impedances, and Gerber, drill, BOM and pick-and-place export. It was started in 1992 by Jean-Pierre Charras in Grenoble, received major contributions from CERN engineers from 2013, and releases a new major version about once a year (version 9 appeared in 2025). Commercial tools — Altium Designer, Cadence OrCAD and Allegro, Siemens Xpedition and PADS, Autodesk Fusion — dominate large companies; LibrePCB and Horizon EDA are other open-source options. Open-hardware projects publish their KiCad files under licences such as the CERN Open Hardware Licence.

Ordering boards has become easy. Export the Gerber and drill files (most fabricators also accept KiCad files directly), upload them, choose layers, thickness, copper weight, finish and colour, and read the fabricator's automatic DFM report before paying. Prototype fabricators include JLCPCB and PCBWay in China, Aisler in Germany, Eurocircuits in Belgium and OSH Park in the United States, among many others; most offer assembly too, from their own stock of parts. Two-layer prototypes typically arrive within one to two weeks. When they do, bring them up carefully: inspect, check the supply rails for shorts with a multimeter before connecting power, power them first from a bench supply with its current limit set low, and only then program the microcontroller.

ExplanationH

Product safety, briefly

EMC keeps products from disturbing each other; product-safety standards keep them from hurting people or starting fires. The main families are hazard-based: IEC 62368-1 for audio, video, IT and communication equipment; IEC 61010-1 for laboratory and measurement equipment; IEC 60601-1 for medical devices; IEC 60335-1 for household appliances. They govern insulation and the spacing between hazardous voltages and anything a person can touch — clearance, the distance through air, and creepage, the distance along a surface, which can be several millimetres for mains circuits — as well as fire enclosures, flammability ratings of materials, temperature limits on touchable surfaces, and how the product behaves under single faults. Certification bodies such as UL Solutions, TÜV, Intertek, BSI and CSA test against them. Environmental rules apply as well: the EU's RoHS directive restricts lead and other hazardous substances, which is why lead-free solder is now the norm, and WEEE governs take-back and recycling.

For learners and small projects, the rule that keeps you safe is simple. Keep your boards at low voltage, powered from a certified USB charger, a certified wall adapter or a current-limited bench supply, so that every hazardous voltage stays inside a product someone else has designed, tested and certified. Never design, build or probe a board connected to mains electricity without professional training and supervision.

Common misconceptionsH

Common misconceptions

Misconception

"If the schematic is right, the board will work." The layout is part of the circuit. A decoupling capacitor 3 cm from its pin, a fast trace across a plane split or a regulator's switching loop drawn large can make a correct schematic fail.

Misconception

"Current returns through ground by the shortest route." At DC it takes the path of least resistance; at the frequencies that matter for noise and signals, it takes the path of least inductance, directly under the trace, wherever that leads.

Misconception

"Only high-frequency designs need to worry about impedance and EMC." A slow clock with fast edges has harmonics far above its frequency. A 1 MHz signal with 2 ns edges carries significant energy beyond 100 MHz, and its traces radiate there.

Misconception

"More decoupling capacitance is always better." Above its self-resonance a capacitor is an inductor, so what matters at high frequency is low mounting inductance and placement, and many identical large capacitors can create a sharp anti-resonance with the plane.

Exercises

Exercises

1. Printed circuit boards

Warm-upHuman

A fabricator offers 2 oz copper on the outer layers. About how thick is that copper, in micrometres?

2. Printed circuit boards

CoreComputational

Write trace_drop_mv(width_mm, length_mm, oz, current_a, temp_c=20.0) returning the voltage drop in millivolts along a straight copper trace, using R=ρL/(wt)R = \rho L/(wt) with ρ=1.72×10−8 Ω m\rho = 1.72 \times 10^{-8}\ \Omega\,\mathrm{m} at 20 °C, a temperature coefficient of 0.0039 per kelvin, and 35 µm of thickness per ounce of copper. (The starter mixes up its units.)

Runs entirely in your browser, in an isolated worker. Nothing is sent to a server.

3. Printed circuit boards

CoreHuman

A 100 nF ceramic capacitor, once mounted, has about 1 nH of series inductance. At what frequency does it self-resonate? Give the answer in megahertz, rounded to the nearest whole number.

4. Printed circuit boards

CoreHuman

A processor's 1.8 V core rail may vary by at most 5%, and the processor's current can step by 2 A. What is the target impedance of the power-distribution network, in milliohms?

5. Printed circuit boards

Warm-upHuman

Where should a microcontroller's 100 nF decoupling capacitor go?

Choose one

6. Printed circuit boards

CoreHuman

A 25 MHz clock trace on the top layer crosses a long slot cut in the ground plane beneath it (left to separate two regions). The board fails its radiated-emissions test near 25 MHz and its harmonics. What is the best fix?

Choose one

7. Printed circuit boards

StretchComputational

The starter contains the lesson's microstrip(w, h, er) function (Hammerstad's approximation, returning the impedance and effective permittivity). Write width_for(z_target, h, er) that returns the trace width giving z_target ohms to within 0.01 Ω, for any reasonable target between about 30 and 120 Ω. The impedance falls as the trace widens.

Runs entirely in your browser, in an isolated worker. Nothing is sent to a server.

8. Printed circuit boards

CoreHuman

A start-up wants to sell a small battery-powered Bluetooth speaker in the European Union. Under which EU legislation does it declare conformity for its radio, and which marking does it then apply?

Choose one

Further reading and resources