PCB Trace Width Calculator (IPC-2221 Basis)

Background.

How wide does a trace need to be for 2 A? On the outer layer of a board in ordinary 1 oz copper, if you accept that it will run 10 °C warmer than the board around it, about 31 mil, or 0.79 mm. Bury the same trace on an inner layer and it needs about 80 mil. Let it run 20 °C warm instead of 10 and the surface trace drops to about 20 mil. There is no single answer because a trace is not limited by current as such. It is limited by how hot it gets, and that depends on how much copper carries the current and how easily the heat can leave.

The figures come from the relation nearly every trace-width tool uses: a curve fitted to the current-capacity charts that went with IPC-2221 and its predecessors, IPC-D-275 and MIL-STD-275. Behind those charts are measurements the US National Bureau of Standards made in the 1950s on bare traces in still air, on thick boards, with no copper plane nearby. The standard printed charts, not an equation; the closed form is usually credited to Douglas Brooks of UltraCAD.

That history sets how far to trust the number. IPC-2221C, published in December 2023, replaced IPC-2221B, and its table of contents lists no current-capacity chart at all. The standard IPC now publishes for this question is IPC-2152, from 2009, built on newer measurements that take in board thickness, the laminate's thermal conductivity and nearby copper planes. Its charts are sold by IPC and are not used here.

What you get, then, is a sound first width for layout and not a rating. A trace that runs over a solid plane will usually be cooler than predicted; one in a sealed box beside a hot regulator, warmer. Anything that carries mains, feeds a battery, or could start a fire if a trace overheats should be checked by a qualified engineer against the standard and edition the product actually has to meet.

What is pcb trace width calculator?

The current-carrying capacity of a printed trace is the steady current at which it settles at a chosen temperature above its surroundings. It is a design limit, not a breaking point. Push more current through and the copper simply runs hotter, which ages the laminate, shifts the values of nearby components and, taken far enough, lifts or opens the trace.

Two units dominate the subject. Widths are given in mils, thousandths of an inch: 10 mil is 0.254 mm and 1 mm is about 39.37 mil. Copper is specified by weight, in ounces per square foot of board, rather than by thickness; one ounce spread over a square foot is 34.798 µm, or 1.37 mil, at the IPC-4562 nominal.

The relation behind the calculator has the current proportional to the cross-sectional area raised to the power 0.725 and the temperature rise raised to 0.44. Both exponents are below one, so copper gives diminishing returns: doubling the area multiplies the current a trace can carry by only about 1.65. The usual explanation is that a narrow trace also spreads heat sideways into the laminate around it, so it is better cooled for its size than a wide one.

How to use this calculator.

1. 01Pick what you want to find: the width for a known current, which is the layout question, or the current for a width you already have, which is the review question. Only the field for the chosen direction is read.
2. 02Enter the steady current in amperes, or the width in mils. For a load that switches or pulses, use its average current; inrush and fault currents are a separate question.
3. 03Set the allowed temperature rise above the surrounding board. 10 °C is a cautious everyday choice and 20–30 °C is common where routing space is tight; the fitted data cover 10 to 100 °C.
4. 04Choose the copper weight from your stack-up. If your fabricator quotes a finished thickness in micrometres, or you want to model foil 10% under nominal, choose custom and type it in.
5. 05Choose external for a trace on the top or bottom surface and internal for one buried between layers. At the same current an internal trace needs about 2.6 times the width, so this choice matters more than any other.
6. 06Read the validity line. If it says the result is extrapolated, you are outside the measured data and the number needs IPC-2152, a thermal simulation or a measurement to back it.

The formula.

The fitted relation is I = k × ΔT^0.44 × A^0.725, with the current I in amperes, the temperature rise ΔT in °C and the cross-section A in square mils. The constant k is 0.048 for a surface trace and 0.024 for a buried one. Solving for area gives A = (I ÷ (k × ΔT^0.44))^(1/0.725), and the width is that area divided by the copper thickness: W = A ÷ t, with t = 1.37 mil per ounce at the nominal. Rating an existing trace runs the first form directly, with A = W × t.

The exponent on area shapes almost everything that follows. Because 1 ÷ 0.725 is about 1.379, the area needed grows faster than the current: double the current and you need 2^1.379 = 2.601 times the copper. Halving k for an internal layer has exactly the same effect, which is why an inner trace needs 2.601 times the width of a surface one. Doubling the current and moving the trace inside cost the same.

The temperature rise works the other way, with an exponent of 0.44 ÷ 0.725 = 0.607 on the area. Allowing 20 °C instead of 10 °C cuts the copper needed by about 34%. Thickness enters only through the product W × t, so 2 oz copper exactly halves the width that 1 oz would need and leaves the cross-section unchanged.

The edges of the underlying charts, 10–100 °C of rise, up to 35 A, up to 400 mil wide and 0.5–3 oz/ft² of copper, are checked on every result, and each limit that is passed is named. The equation still returns a number beyond them, but no measurement stands behind it.

Two simplifications are built in. The cross-section is taken as a rectangle, whereas etching leaves a trace slightly trapezoidal and a little smaller in section. And nothing describes the board itself: its thickness, its laminate, and any copper pour or plane beside the trace all change the real temperature.

A worked example.

Frequently asked questions.

References& sources.

1. [1]IPC-2221C, "Generic Standard on Printed Board Design", December 2023, developed by the IPC-2221/2222 Task Group (D-31b) of the Rigid Printed Board Committee (D-30). Published table of contents read directly on 2026-07-29; the standard itself is sold by IPC and was NOT opened. Source of the supersession statement ("Supersedes: IPC-2221B, November 2012"), of the current contents of §6.2 Conductive Material Requirements — §6.2.1 Surge Current and §6.2.1.1 Example Algorithm Calculation Within an Application — of the relocation of conductor width and thickness to §10.1.1, and of Table 10-2 "Thickness of External Conductor of the Finished Printed Board after Plating". Neither the figure list nor the table list of this edition contains a conductor current-capacity chart. Nothing on this page is attributed to a clause of the standard's body.
2. [2]IPC-2152, "Standard for Determining Current Carrying Capacity in Printed Board Design", 2009. Named on this page as the standard IPC now publishes for this specific question and as the reason the IPC-2221 basis is described as the older one. Access: gated — sold by IPC; its charts were not available and are not implemented here. No figure from it is used or quoted anywhere on this page.
3. [3]Multi Circuit Boards Ltd, "Conductor / Ampacity" PCB design-aid page. Retrieved and read 2026-07-29. The source of this page's central caveat: "In the original IPC documentation no formulas are given, these were derived by e.g. Douglas Brooks." It also records that the underlying data originate in 1950s National Bureau of Standards measurements on 1.6 mm boards, and that they do not consider the surrounding medium — air pressure or movement — or the layout density.
4. [4]Altium, "IPC-2221 Calculator for PCB Trace Current and Heating". Retrieved and read 2026-07-29. Attributes the cross-section relation to IPC-2221 §6.2 and Appendix B, and states the conditions the underlying test boards were measured under: air at standard temperature and pressure, and "a trace on a thick board, there was no additional copper nearby (planes or pour)". Also notes that thinner boards call for greater derating and that substrates with higher thermal conductivity behave differently.
5. [5]DigiKey, "PCB Trace Width Conversion Calculator" resource page. Retrieved and read 2026-07-29. An independent statement of the same curve-fit constants used here — k = 0.024, b = 0.44, c = 0.725 for internal layers and k = 0.048 with the same exponents for external layers in air — from a distributor rather than a fabricator or a standards body. Used as the confirmation that the constants implemented in this calculator are the ones in general use.
6. [6]Eurocircuits, "Tolerances on Copper Thickness" technical guideline. Retrieved and read 2026-07-29. Source of the copper weight to thickness conversion used throughout this page: "1oz/ft² has a thickness of 1.37 mil (0.00137 Inch) or 34.798 µm", citing IPC-4562. Also the source of two caveats stated on the page: that IPC-4562 allows up to a 10 % reduction in base copper thickness, and that on outer layers the start copper must be less than the required end copper because plating adds roughly 20 µm.