PCB trace width calculator

How to use the trace width calculator

1. Choose whether you want the width for a current or the current for a width.
2. Enter the current (or width), the copper weight of the layer, and the temperature rise you can accept.
3. Pick an outer or inner layer. Inner layers need much wider traces for the same current.
4. Add the trace length if you also want its resistance, voltage drop and power loss.

The result is the narrowest trace that stays within your temperature rise. Round it up to a value your fab and layout grid like, and leave margin on traces that carry power for long periods. Switch between mm and mil at any time; the calculator keeps the physical size.

How to calculate PCB trace width with IPC-2221

IPC-2221 relates current to the copper cross-section of the trace and the temperature rise it causes:

I = k × ΔT^0.44 × A^0.725

Here I is the current in amps, ΔT the temperature rise in °C, and A the cross-sectional area in square mils. The constant k is 0.048 for outer layers and 0.024 for inner layers. To get a width, solve for the area, A = (I ÷ (k × ΔT^0.44))^1/0.725, then divide by the copper thickness: 1 oz/ft² copper is about 35 µm (1.38 mil) thick.

Worked example 1: 1 A on an outer layer

A = (1 ÷ (0.048 × 10^0.44))^1/0.725 ≈ 16.3 mil². With 1 oz copper that is 16.3 ÷ 1.38 ≈ 11.8 mil, or about 0.30 mm.

Worked example 2: 5 A on an inner layer with 2 oz copper and a 20 °C rise

With k = 0.024, A = (5 ÷ (0.024 × 20^0.44))^1/0.725. 2 oz copper is 2.76 mil thick, so the width comes out at 2.36 mm (93 mil). The same current on an outer layer would need only 0.908 mm (35.7 mil).

Worked example 3: how much current a 0.5 mm trace carries

Run the formula forwards. A 0.5 mm (19.7 mil) trace in 1 oz copper has A ≈ 27.1 mil², so on an outer layer with a 10 °C rise it carries I = 0.048 × 10^0.44 × 27.1^0.725 ≈ 1.45 A.

Trace resistance and voltage drop

Heat is only half the story. A trace that is thermally fine can still drop too much voltage, especially on low-voltage rails. Copper's resistivity is 1.724 × 10^-8 Ω·m at 20 °C and rises by about 0.393 % per °C, so a trace running 10 °C above a 25 °C ambient has roughly 6 % more resistance than at room temperature.

The quickest way to estimate resistance is to count squares. A trace's resistance is its sheet resistance times length ÷ width. 1 oz copper is about 0.5 mΩ per square at 25 °C, so a 10 mil × 1 inch trace is 100 squares, or about 50 mΩ. At 2 A that is about 100 mV of drop, which is fine for 12 V and noticeable on a 1.0 V core rail.

Design guidelines and common mistakes

• Round up. A trace a little wider than the minimum costs nothing and buys margin for etch and copper tolerance.
• For several amps, use a copper pour or polygon instead of a single trace, and keep the path short.
• When a high-current path changes layer, use several vias. One small via can carry far less than the trace feeding it; check with the via current calculator.
• Check the voltage drop as well as the temperature: a long, thin supply trace can drop more than your regulator's headroom.
• Size for the worst sustained current, not the typical one. Motor stall, inrush and fault currents matter.
• Do not use the inner-layer result for a trace on the top or bottom, or the other way round. The factor is about 2.6.
• Don't forget the bottleneck: a wide trace that necks down into a narrow connector pin or a thermal-relief spoke is only as good as its narrowest point.
• Stay at or above your fab's minimum trace width. Many fabs list about 0.1 to 0.127 mm (4 to 5 mil) as standard, so check yours. For the full set of rules, see the PCB design rules guide.

IPC-2221 vs IPC-2152, and where this calculator stops

Outer-layer traces lose heat to the air, while inner traces are wrapped in laminate. That is why IPC-2221 asks for roughly 2.6 times the width on an inner layer for the same current. The newer IPC-2152 standard, built from more measurements, shows that IPC-2221 is conservative for inner layers, and that copper planes near a trace and a thicker board both help it run cooler. If you are tight on space, IPC-2152 charts can justify narrower inner traces; if you have room, the IPC-2221 width is the safe choice.

The IPC-2221 curves were drawn for currents up to 35 A, widths up to 400 mil and temperature rises from 10 to 100 °C. Outside that range the calculator warns you, because the result is an extrapolation. It also assumes an isolated trace carrying steady DC: neighbouring hot traces, enclosed boards, high ambient temperatures and high-frequency AC all change the picture, and a thermal simulation or a measured prototype is the final word.

Trace width for impedance and RF

Current is not the only reason to pick a width. High-speed and RF traces are sized for a characteristic impedance such as 50 Ω single-ended or 90 to 100 Ω differential, which depends on the trace width, copper thickness, dielectric height and material. Those widths are usually far narrower than any current limit, so size controlled-impedance traces with the PCB impedance calculator and use this page for power.

Do this automatically in ProtoFlow

In the ProtoFlow desktop app, current is a property of the net class rather than a number you look up. Set a target current on a class such as Power, and Board Setup computes the IPC-2221 width from the copper weights in your stackup, rounds it up and flags any class whose trace width cannot carry its current. The autorouter then routes each net at its class width, so the 3 A input and the 50 mA sensor line come out right without you sizing them by hand. You can start from a plain-English description of the board, let the AI draft the schematic and layout, and refine from there. Download ProtoFlow free for macOS, Windows or Linux.