PCB Trace Width Calculator (IPC-2221 Basis)

Background.

A copper trace carrying current gets warm, and how warm depends on how much copper there is to carry it and how easily the heat can leave. Sizing a trace is therefore a thermal question dressed up as an electrical one, and the answer everyone reaches for is the relation published with the IPC-2221 design standard. This page implements that relation in both directions — the width a trace needs for a given current, and the current a trace of a given width can carry — because they are the same equation with different unknowns and there is no reason to make you visit two pages for it.

Three things about that relation deserve to be said before the number, not after it.

The first is that the equation is not printed in the standard. IPC-2221 published charts, drawn from measurements the US National Bureau of Standards made in the 1950s. The closed form everyone uses — current equals a constant, times the temperature rise to the power 0.44, times the cross-sectional area to the power 0.725 — is a published curve fit to those charts, generally attributed to Douglas Brooks of UltraCAD. It reproduces the charts well. It is still a fit to a graph rather than a clause of a standard, and anyone quoting it as "the IPC formula" is skipping a step.

The second is that the edition matters, and the current edition has moved the material. IPC-2221C, published in December 2023, supersedes IPC-2221B of November 2012 in its entirety. Its table of contents shows section 6.2, Conductive Material Requirements, reduced to a surge-current subsection and an example algorithm, the conductor width and thickness material relocated to section 10.1.1, and no conductor current-capacity chart in either its figure list or its table list. The charts this curve fit was fitted to belong to IPC-2221B and to its ancestors IPC-D-275 and MIL-STD-275.

The third is that IPC has published a better standard for this specific question. IPC-2152, released in 2009, is built on new measurements and accounts for board thickness, the thermal conductivity of the dielectric, and whether there is a copper plane nearby — none of which appear anywhere in the IPC-2221 relation. Its charts are sold rather than published, and they were not available for this page. So this calculator implements the older, generally more conservative IPC-2221 basis, says so beside every result, and does not pretend to be IPC-2152.

What the equation does capture is the part that matters most in practice. Only the cross-sectional area counts, so width and copper weight trade off directly against each other: double the copper and you halve the width. The layer matters enormously — an internal trace has no air to shed heat into, so the constant halves and the trace needs about 2.6 times the width for the same current. And the temperature rise is a design choice rather than a fixed limit: allowing 20 °C instead of 10 °C shrinks the copper needed by about a third, which is often the difference between a routable board and a redesign.

The conditions the original data were taken under are worth knowing, because they are not your board. A bare trace, in still air at standard temperature and pressure, on a thick substrate, with no copper pour and no plane anywhere near it. A real trace surrounded by ground plane runs cooler than the charts predict; a real trace in a sealed enclosure beside a hot regulator runs hotter. The result here is a starting point for a design, not a rating.

The page states the boundaries of the underlying data explicitly and tells you when you have left them. The charts cover temperature rises from 10 to 100 °C, currents up to 35 A, widths up to 400 mil and copper from 0.5 to 3 oz/ft². Outside those the equation still returns a number, because arithmetic always does, but there is no measurement behind it — and this calculator names every limit you have passed rather than quietly extrapolating.

Finally, and this belongs in the first screen rather than an appendix: trace sizing is a safety calculation whenever the current is large enough to start a fire. Battery packs, mains-connected sections, motor drives and anything where a fault current can flow through a trace should be reviewed by a qualified engineer against the standard your product must actually meet, in the edition your jurisdiction or customer has adopted. This calculator is an input to that review, not a substitute for it.

What is pcb trace width calculator?

The current-carrying capacity of a printed conductor is the current at which it settles at some agreed temperature above the board around it. It is not a fusing current and not a hard limit: a trace does not stop working when it exceeds this figure, it simply runs hotter, which ages the laminate, shifts nearby component values and eventually delaminates or opens the copper.

The IPC-2221 relation states that current equals k times the temperature rise raised to the power 0.44, times the conductor cross-sectional area raised to the power 0.725, with the area in square mils, the current in amperes and the rise in degrees Celsius. The constant k is 0.048 for an external conductor on the surface of a board and 0.024 for an internal one buried between layers.

Both exponents are less than one, and that is the physically important part. Doubling the area does not double the current — it multiplies it by two to the power 0.725, which is about 1.65. Doubling the allowed temperature rise multiplies the current by two to the power 0.44, about 1.36. Copper gets progressively less effective as you add it, because a wider trace sheds heat from its edges no better than a narrow one does and the middle has to conduct sideways to reach the surface.

Copper thickness enters through the weight of the foil, which is quoted in ounces per square foot rather than in microns. One ounce per square foot spread over that area is 34.798 µm, or 1.37 mil, at the IPC-4562 nominal. That nominal is a starting point rather than a guarantee: IPC-4562 permits the base foil to be up to 10 % thinner, plating adds copper to outer layers so the finished thickness is usually greater than the base foil, and etching leaves the trace trapezoidal in section rather than rectangular, so the true cross-section is a little smaller than width times thickness.

How to use this calculator.

1. 01Choose the direction. Sizing a trace for a known current is the usual design task; rating a trace you already have is the usual review task.
2. 02Enter the steady current, or the width in mils. A mil is a thousandth of an inch — 10 mil is 0.254 mm — and it is what most PCB tools use for track widths.
3. 03Set the temperature rise you are prepared to accept, above the surrounding board. Ten degrees is a conservative default and a good starting point. Twenty to thirty degrees is common where space is tight, and it buys a lot: the copper needed falls by about a third going from 10 °C to 20 °C.
4. 04Pick the copper weight from your stack-up, not from habit. One ounce per square foot is the usual default for signal layers, but power layers and heavy-current boards are often two or four. If your fabricator has quoted a finished thickness in microns, choose custom and enter it.
5. 05Choose external or internal correctly. This is the input people get wrong, and it is not a small error: an internal trace needs about 2.6 times the width of a surface trace for the same current, because it has no air to shed heat into.
6. 06Read the validity line under the result. If it says the answer is extrapolated, the equation has been pushed past the data behind it and the number should not be trusted without a simulation or a measurement.
7. 07Add margin for your own layout. The charts were measured on a bare trace in still air with no copper nearby. A trace against a ground plane runs cooler; a trace in a sealed box next to a regulator runs hotter; a trace under a component runs hotter still.
8. 08Treat the answer as a floor, and have anything mains-connected, battery-fed or otherwise capable of starting a fire reviewed by a qualified engineer against the standard and edition your product must actually meet.

The formula.

The relation is I = k · ΔT^0.44 · A^0.725, with A in square mils, I in amperes and ΔT in degrees Celsius above ambient. To size a trace, invert it: A = (I / (k · ΔT^0.44))^(1/0.725), and then divide the area by the copper thickness to get a width. Both directions on this page use exactly these two expressions, which is why the two questions are not two calculators.

The constant k carries the layer: 0.048 on the surface, 0.024 buried. Halving k halves the right-hand side, so recovering the same current needs the area to grow by a factor of two raised to one over 0.725, which is 2.601. That is where the familiar rule that an internal trace needs about two and a half times the width comes from, and this page's tests assert the ratio explicitly rather than trusting the rule.

Copper weight enters only through the thickness, and only as a product with the width. One ounce per square foot is 34.798 µm — 1.37 mil — at the IPC-4562 nominal quoted by Eurocircuits. Because the equation is written in area, doubling the copper weight exactly halves the width required and leaves the cross-section unchanged, which the tests also check.

The worked example is 2 A on an external layer in 1 oz copper with a 10 °C rise. The thermal term is 0.048 × 10^0.44 = 0.13220. Dividing 2 by it gives 15.128, and raising that to the power 1/0.725 gives a cross-section of 42.393 mil². At 1.37 mil of copper thickness that is 30.94 mil of width, or 0.786 mm. The same inputs on an internal layer give 80.50 mil — 2.601 times as wide, exactly as the constants predict.

A useful sanity check falls out of the same arithmetic: 1 A at a 10 °C rise in 1 oz external copper needs 11.89 mil, which is the familiar "about 12 mil per amp" rule of thumb that circulates in PCB design. It is not a coincidence; it is this equation evaluated at that point.

Rounding happens once, at the return boundary, to ten decimal places, and all internal arithmetic is exact decimal at forty significant digits. The validity classification reads the unrounded values, and its edges are the published limits of the chart data — 10 and 100 °C of rise, 35 A, 400 mil of width, 0.5 and 3 oz/ft² of copper — rather than anyone's opinion about what is reasonable. Those limits interact: 35 A is inside the current limit but, in 1 oz copper at a 10 °C rise, wants a trace over 1500 mil wide, so it fails the width limit instead. The page names every limit that was passed rather than only the first.

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.