IPC-2221 vs IPC-2152: Which Trace-Width Standard to Use
Two IPC standards answer the same question - how wide a PCB trace must be to carry a given current without overheating - and they routinely give different numbers. One is a single 50-year-old formula; the other is a modern, chart-based method built from fresh testing. Here is what separates them, why they disagree, and how to decide which to trust for your board.
Short answer. Use IPC-2221 for a fast, conservative first pass - it only needs current, temperature rise and copper weight, and it will never undersize a trace. Reach for IPC-2152 when width actually matters (power traces, dense boards), because it accounts for board thickness, material and nearby copper planes, and usually allows a narrower trace. A good workflow is to size with IPC-2221, and re-check against IPC-2152 before committing.
The two standards at a glance
| IPC-2221 | IPC-2152 | |
|---|---|---|
| Published | Generic design standard; curves trace back to 1950s military data | 2009, from a dedicated modern test program |
| Method | One empirical formula | Charts (nomographs) plus correction factors |
| Inputs | Current, temperature rise, copper cross-section | The above plus board thickness, dielectric, copper weight and plane proximity |
| Tendency | Conservative - sizes wider traces | More accurate - usually allows narrower traces |
| Best for | Quick checks, signal traces, a safe floor | High-current and space-constrained power design |
IPC-2221: the conservative baseline
IPC-2221 is the generic printed-board design standard, and its trace-width method is what almost every quick online calculator uses. Its current-carrying curves descend from work done for the US military in the 1950s, later folded into IPC-D-275 and then IPC-2221. The method reduces to a single equation:
where I is the current in amps, ΔT is the allowed temperature rise in °C, A is the copper cross-sectional area in mil², and k is 0.048 for external (outer-layer) traces and 0.024 for internal ones. Rearranged for area, A = (I / (k · ΔT0.44))1/0.725, and width is simply that area divided by the copper thickness.
Worked example. An external trace carrying 5 A with a 10 °C rise on 1 oz copper:
- k · ΔT0.44 = 0.048 × 100.44 ≈ 0.048 × 2.75 = 0.132
- A = (5 / 0.132)1/0.725 = 37.91.38 ≈ 150 mil²
- 1 oz copper is about 1.37 mil thick, so width ≈ 150 / 1.37 ≈ 110 mil (2.8 mm)
Its strength is speed; its weakness is that it treats every board the same. The formula assumes a bare trace in still air and ignores the board around it, so the trace it asks for is usually wider than a real board needs.
IPC-2152: the measured, modern method
IPC-2152, published in 2009, was built from a fresh and far more thorough test program rather than mid-century data. Instead of one formula it provides a set of charts - more than a hundred figures - because it accounts for the things IPC-2221 ignores: the thickness of the board, the thermal conductivity of the laminate, the copper weight, and, most importantly, whether copper plane sits nearby to spread heat. You read an unadjusted cross-sectional area from the chart for your current and temperature rise, then apply correction factors for your actual situation.
The practical result is that IPC-2152 usually permits a narrower trace than IPC-2221 for the same current - on a typical board with copper pours it can be in the region of 1.5 to 2 times the current at the same temperature rise. A ground or power plane within roughly half a millimetre of the trace acts as a heat sink and raises capacity further, on the order of 40 percent. None of that is visible to IPC-2221.
Internal traces need more width - and why
Both standards agree that a buried internal trace needs more copper than an external one, because it cannot shed heat to the air. In the IPC-2221 formula this shows up as a halved constant, k = 0.024 instead of 0.048. Because of the 0.725 exponent, halving k does not simply double the width - it works out to roughly 2.6 times the width for the same current and temperature rise. One of IPC-2152's notable findings is that on real boards the internal penalty is often smaller than that, because what really governs cooling is how well the whole board moves heat, not just which layer the trace sits on.
So which should you use?
For most general-purpose work, IPC-2221 is a sound starting point. It is conservative, so a trace sized by it will not be too small, and it takes seconds. Use it for signal and light-power traces, where a little extra copper costs nothing, and as a quick sanity check on anything.
Reach for IPC-2152 when the extra width matters: high-current power traces, dense boards where space is tight, or any case where you need to justify a narrower trace with confidence. It takes more effort because it needs board-specific inputs and chart interpolation, but it rewards that effort with a result much closer to how the board will actually behave. A workflow many engineers use: size with IPC-2221 first, and if the result is awkwardly wide, re-check it against IPC-2152 before committing. If both agree, you have comfortable margin; if they disagree, IPC-2152 is the better guide - provided you have characterised your board correctly.
Common misconceptions
- "IPC-2221 is obsolete." No - it is still the right tool for a fast, conservative estimate and a safety floor.
- "IPC-2152 always gives a smaller trace." Usually, but not always. A board with no planes and poor heat spreading benefits far less, and in some isolated cases can even need more.
- "A lower temperature rise is always safer, so always use it." The right ΔT depends on the enclosure, ambient temperature, nearby components and reliability target. 10 to 20 °C is a common starting range; tighten it for sealed, automotive or medical designs.
A practical checklist
- Decide your acceptable temperature rise first, not the width.
- Use the real finished-copper weight, and remember internal traces need much more width.
- Keep heavy current on outer layers, or specify heavier copper, where you can.
- Check the result against your fabricator's minimum trace width before committing.
- Add margin for transient or fault currents, and size vias as deliberately as traces.
You can size a trace by both methods, side by side, with our PCB trace width calculator - it shows internal and external layers together, with resistance, voltage drop and the governing clause.
Frequently asked questions
Why are internal traces wider than external ones?
Internal traces are buried in laminate with no direct path to the air, so they cool far less effectively. IPC-2221 captures this by halving its constant (0.024 versus 0.048), which works out to roughly 2.6 times the width for the same current and temperature rise.
How much narrower can IPC-2152 go?
On a typical board with copper pours or planes, IPC-2152 often allows the same current through a noticeably narrower trace - frequently in the range of 1.5 to 2 times the current capacity of IPC-2221 at the same temperature rise. The exact figure depends on board thickness, copper weight and plane proximity.
What temperature rise should I design for?
10 °C is a safe, common default and 20 °C is acceptable for many designs. Choose the lower end for sealed enclosures, high ambient temperatures, or automotive and medical boards, and for traces running near hot components.
Do I still need to check fabrication limits?
Yes. A calculated width is only useful if the board can be built to it. Confirm the result against your fabricator's minimum trace width and copper-weight capability, and add margin for tolerance.
Sources: IPC-2221C, Generic Standard on Printed Board Design · IPC-2152, Standard for Determining Current-Carrying Capacity in Printed Board Design. Verify against the current edition.