Saved

Press the star next to a tool's name to save it.

All my tools

Pcb Trace Width Calculator

Use this PCB trace width calculator to find the track width for a current, copper weight and temperature rise on an outer or inner layer, with resistance and voltage drop.

Restored your last values ·

A
oz/ft²

Choose US or metric units and an external or internal layer. Enter the current the trace must carry, the copper weight and the temperature rise you accept. You get the width and cross-section. Add a trace length to see the resistance, the voltage drop and the power lost.

Everything is worked out in your browser. Nothing you type is sent anywhere.

–

–

Choose the units and the layer, enter the current, the copper weight and the temperature rise, then press Calculate.

See full result

A PCB trace width calculator tells you how wide a copper track must be to carry a given current without heating more than you allow. Enter the current, the copper weight and the temperature rise, choose an external or internal layer, and the tool gives the width in mil and millimetres, the cross-section and, with a length, the resistance and voltage drop.

How to use the pcb trace width calculator

  1. Choose US or metric units and the layer.
  2. Enter the maximum current in amps.
  3. Enter the copper weight and the temperature rise you accept.
  4. Add a length and an ambient temperature if you want the resistance.
  5. Press Calculate.

The IPC-2221 formula

The tool uses the IPC-2221 relation between current and copper area: I = k × ΔT^0.44 × A^0.725, where I is in amps, ΔT is the rise above ambient in °C and A is the cross-section in square mils [1][2]. NextPCB solves it for the area as A = (I ÷ (k × ΔT^0.44)) to the power 1 ÷ 0.725 [1]. The width then follows by dividing the area by the copper thickness.

The constants

The constant k is 0.048 for a trace on an outer layer and 0.024 for one on an inner layer, which cools less well [1][2]. The exponent on the rise is 0.44 and on the area 0.725 [1]. The width is the area divided by 1.378 times the copper weight in ounces per square foot, because 1 oz copper is 1.378 mil thick [1]. The tool prints the constants it used with every result.

A worked example

For 3 A on an outer layer with 1 oz copper and a 10 °C rise, the area is 74.16 square mils and the width 53.82 mil, or 1.367 mm. On an inner layer, with k = 0.024, the same job needs 192.9 square mils and 140.0 mil. For 1 A on the outer layer the width is 11.83 mil. The 3 A outer-layer width agrees with the reference table in the NextPCB guide, which gives 53.8 mil [1].

External or internal layers

An inner trace is buried in the board and loses heat less easily, so it must be wider for the same current and rise. With the constants above, an internal trace needs about 2.6 times the area of an external one, which is 2 raised to the power 1 ÷ 0.725 and is our own working from the constants [1][2]. Choose the layer where the track will actually run. If a track crosses both, size it for the inner layer.

Copper weight

Copper weight is quoted in ounces per square foot. NextPCB gives 1.378 mil of thickness for 1 oz [1]. Wikipedia gives 34.1 micrometres, or 1.34 mil, for 1 oz, about 3 percent less [3]. The tool uses 1.378. The difference is small compared with the other uncertainties, and a wider track from the larger figure is on the safe side only if the real copper is at least that thick.

Temperature rise

The rise is the temperature of the trace above the surrounding air, not the temperature itself. A larger rise allows a narrower trace but heats the board more. In US units the box takes a rise in degrees Fahrenheit, which the tool divides by 1.8 to get the °C the formula needs. The ambient temperature box matters only for the resistance, where the trace temperature is the ambient plus the rise, which is our assumption.

Resistance, drop and power

With a length, the tool estimates the resistance from R = ρ × L ÷ A′ × (1 + α × (T − 25)), with ρ = 1.7 × 10⁻⁶ ohm cm, the copper resistivity that NextPCB uses [1], and α = 0.0039 per °C, an approximate coefficient for copper that is our own rounding. L is in cm and A′ in cm². For the 3 A example over 60 mm at 35 °C, R is 22.15 milliohm, the drop 66.45 mV and the loss 0.199 W. NextPCB's own example for a 60 mm trace reports about 22 milliohm [1].

The range of the data

NextPCB says the original IPC-2221 test data covers up to 35 A, 400 mil of width, 10 to 100 °C of rise and 0.5 to 3 oz copper [1]. The tool shows a warning when your inputs are outside that range, and calls the result a rough guide. When they are inside the range, the tool says so and notes that copper pours, planes and vias are not modelled.

What the formula leaves out

The Proto Express page notes that the formula ignores large ground planes, copper pours and heat sinks, so it can give wider traces than are needed, and that it was developed from a single board type and one copper weight [2]. It also discusses IPC-2152, a later standard that takes more into account. Our tool does not model board thickness, vias or neighbouring heat sources.

Using the result

Round the width up to a convenient value and add a margin, because manufacturing tolerances, copper thickness and local heating vary. If the answer is wider than the space allows, you can raise the temperature rise, use thicker copper, move the track to an outer layer or split the current across parallel tracks. Then run the calculation again with the new values and compare the widths.

Naming the standard

Some online guides attribute this calculation to IPC-2141A, which is a guide to controlled impedance, while the NextPCB and Proto Express pages give the same equation as IPC-2221 [1][2]. We therefore call it the IPC-2221 formula. We did not open the IPC standards themselves, which are paid documents, so the pages cited are our source for the equation.

Common mistakes

  • Typing the rise as a temperature. It is the increase above ambient, not the final temperature.
  • Using the external layer for an inner trace. Inner traces need to be wider.
  • Forgetting the copper weight. Half-ounce copper needs a track twice as wide as one-ounce copper.
  • Treating the result as a limit. Add a margin and check with your board maker.

What next

Use this often? Add Pcb Trace Wi to your Home screen.

Frequently asked questions

What is a PCB trace width calculator?

A tool that finds the width of a copper track needed to carry a current for a chosen temperature rise, using the IPC-2221 formula.

What are the IPC-2221 constants?

The constant k is 0.048 for external layers and 0.024 for internal layers, with exponents 0.44 for the temperature rise and 0.725 for the copper area.

How wide is a trace for 3 A?

On an outer layer with 1 oz copper and a 10 °C rise, about 53.8 mil or 1.37 mm. On an inner layer it is about 140 mil.

Why is an internal trace wider?

It loses heat less easily than an outer one, so the same current and rise need more copper.

Is the result a safe design value?

It is an estimate that ignores planes, pours and vias. Add a margin and check the design with your board maker.

What went wrong?

We only receive the reason you pick, never what you typed into the tool.

Thanks for your feedback.

More Physics & Science Tools