PCB Trace Inductance Calculator

The PCB Trace Inductance Calculator computes the partial self-inductance of a straight, rectangular PCB trace from its length, width and copper thickness — essential for power distribution network (PDN) design, decoupling capacitor placement, and high-frequency signal integrity. Partial inductance is the trace's own share of the inductance of whatever loop its current flows in; at 100 MHz, every nanohenry of it between a capacitor and an IC pin adds 0.63 Ω of reactance. The calculator models the trace on its own: it has no input for the height above a ground plane, so it gives the same result for a microstrip, a stripline or a trace with no plane at all.

It uses Ruehli's closed form for a rectangular conductor: $L = \frac{\mu_0 l}{2\pi}\left[\ln\frac{2l}{w+t} + 0.5 + \frac{w+t}{3l}\right]$, where l is the trace length, w the trace width and t the copper thickness. A 50 mm trace, 0.3 mm wide in 1 oz (35 µm) copper, comes to 62.0 nH, or 1.24 nH/mm. At 100 MHz that is 39.0 Ω of reactance, far above the trace's DC resistance of 82 mΩ.

Inductance dominates a trace's impedance above the crossover frequency $f_c = R/(2\pi L)$, where R is its DC resistance. In 1 oz copper that is about 210 kHz for the 50 mm, 0.3 mm trace above, 50 kHz for the worked example's 30 mm, 2 mm power trace and 395 kHz for the calculator's default 10 mm, 0.2 mm trace. Above it, shortening a trace or adding parallel paths (copper pours) lowers impedance more than widening does: width enters only through the logarithm, while each parallel path divides the inductance, provided the paths are far enough apart that their mutual inductance is small.

Loop inductance is a different quantity, and the calculator does not report it. A trace's current returns through the reference plane beneath it, and what sets ground bounce and radiated emissions is the inductance of the whole loop: the closer the plane, the more of the trace's field the return current cancels. Per unit length, the loop inductance of a microstrip is $L' = Z_0\sqrt{\varepsilon_{eff}}/c$, its impedance times its propagation delay per unit length, both of which the microstrip impedance calculator reports. For the 0.3 mm trace above, that is 0.62 nH/mm with the plane 1 mm below and 0.22 nH/mm at 0.1 mm, a 65% reduction, against 1.24 nH/mm of partial inductance. For a trace much wider than its height above the plane, $L' \approx \mu_0 h/w$ is a quick estimate, as in the worked example; it reads somewhat high because it ignores the fringing field. This is why controlled impedance designs place signal layers next to ground planes.