PCB Trace Width Calculator
Trace width for a given current and temperature rise, to IPC-2221.
IPC-2221 is an external-air, single-trace model. Dense boards, thermal vias, adjacent heat sources and conformal coating all change the real temperature rise.
How it works
IPC-2221 gives an empirical curve fitted to measured data rather than a derivation from first principles:
A = (I ÷ (k × ΔT^0.44))^(1÷0.725)
with A the cross-section in square mils, and k = 0.048 for external traces and 0.024 for internal ones. Width follows by dividing by the copper thickness — one ounce of copper is 1.378 mil, about 35 µm.
That factor of two in k is the part people miss. An inner layer is buried in laminate, which is a thermal insulator, so it can only shed heat sideways through the copper itself. Because the exponent is 1/0.725 rather than 1, halving k does not halve the width — it costs about two and a half times: 2 A at a 10 °C rise wants 0.78 mm on an outer layer and 2.03 mm on an inner one. A design that routes power through internal planes without accounting for that runs hot in a way no amount of bench testing at room temperature reveals.
The standard is also conservative for a reason: it assumes a trace alone in still air on a board that is not doing anything else. Real boards have adjacent traces warming each other, components dumping heat into the copper, and enclosures that trap it. Ten degrees of rise is the usual design allowance; going to 20 or 30 is acceptable when nothing nearby is temperature-sensitive, and the width required falls sharply because of that 0.44 exponent.
Resistance matters separately from heating. A 0.5 mm trace in 1 oz copper is about 1 mΩ per millimetre, which is nothing on a signal and quite a lot on a 10 A power rail — and in a switching supply, trace resistance in the wrong loop is a measurable efficiency loss and a source of ground bounce.
Common questions
Why do internal traces need to be wider?
They are surrounded by laminate, which insulates rather than conducts heat away. IPC handles this with a k value half that of an external trace — and because the width exponent is 1/0.725, that works out at about two and a half times the width, not twice.
What temperature rise should I allow?
10 °C is the usual default and leaves margin. 20 °C is fine if nothing heat-sensitive is nearby and the board is not already hot. Remember it is a rise above ambient — a 20 °C rise inside a 60 °C enclosure puts the copper at 80.
Is a wider trace always better?
For power, yes. For high-speed signals, no — width is set by the impedance the trace has to present, which depends on the dielectric height beneath it. Widening a controlled-impedance trace breaks it.
What about vias?
A via is a much smaller conductor than the trace it joins, so it is often the real limit. A rough rule is one 0.3 mm via per amp, and use several in parallel for a power connection rather than relying on one.