How this instrument works
Every copper trace on a PCB has resistance, and current flowing through resistance generates heat (I squared R heating). Too much current for too little copper and a trace can overheat — degrading the board, lifting the copper, or in extreme cases burning the trace open. IPC-2221, the industry-standard PCB design guideline, provides an empirical formula (derived from physical test data, not first-principles thermodynamics) relating a trace's cross-sectional area and an allowed temperature rise to the maximum current it can carry.
The formula treats external traces (on an outer layer, exposed to air) differently from internal traces (buried between layers of laminate): external traces cool by convection into the surrounding air and can carry more current for the same cross-section, while internal traces are thermally insulated by the surrounding board material and need more copper for the same current. That's why the same trace geometry produces roughly double the current rating on an external layer versus an internal one — not because the physics of resistive heating changed, but because the internal trace has nowhere for that heat to go.
Allowed temperature rise (deltaT) is a design choice, not a fixed constant — 10 degrees C is a common conservative default for general-purpose traces, while power traces or traces near heat-sensitive components might use a tighter (lower) allowance, and traces where a higher operating temperature is acceptable might use a looser one. Doubling the allowed rise doesn't double the current rating, since deltaT enters the formula raised to the 0.44 power, not linearly.
- Enter Trace width in mils — the copper trace's width as drawn (1 mil = 0.001 inch).
- Enter Trace thickness in mils — 1oz copper is about 1.378 mils, 2oz about 2.756 mils, common PCB copper weights.
- Enter Allowed temperature rise deltaT in degrees C — how much hotter the trace is allowed to get above ambient (10C is a common default).
- Select Layer — External (exposed to air, cools better) or Internal (buried, insulated by the board).
- Read Maximum current in amps — the highest current this trace can carry without exceeding the allowed temperature rise.
Worked example — a 20-mil trace at 1oz copper
A 20-mil-wide, 1oz-copper (1.378-mil) external trace with a 10C allowed temperature rise: cross-sectional area A = 20 x 1.378 = 27.56 mils squared. Current I = 0.048 x 10^0.44 x 27.56^0.725 = 0.048 x 2.7542 x 11.0714 = 1.4637A — in line with commonly published IPC-2221 trace-current charts for exactly this width, weight, and layer combination.
Move that identical trace to an internal layer, everything else unchanged, and the constant k halves (0.024 instead of 0.048): I = 0.024 x 2.7542 x 11.0714 = 0.7318A — exactly half the external-layer result, since only k changed. That factor-of-two is the concrete, memorable version of "internal traces need roughly double the copper for the same current" that this formula produces.
Questions
Why can an external trace carry more current than an internal one of the same size?
Because it can cool itself better. An external trace sits on an outer layer exposed to open air and loses heat by convection; an internal trace is sandwiched inside the board's laminate, which is a much poorer conductor of heat, so the same resistive heating raises the trace's temperature more for the same current. IPC-2221 captures this with two different empirical constants — k=0.048 for external, k=0.024 for internal — which is why an internal trace needs roughly double the cross-sectional area to carry the same current as an external one.
What allowed temperature rise (deltaT) should I use?
10C is a commonly used general-purpose default, and it's this calculator's default too. Tighter designs near heat-sensitive components, or boards operating in already-hot enclosures, often use a lower deltaT (5C, for example) to leave more thermal margin; power electronics where some extra warmth is acceptable sometimes use a higher one (20C+). There's no single correct value — it's a design trade-off between trace width (and therefore board space) and thermal margin.
Does doubling the temperature rise double the current rating?
No — deltaT enters the IPC-2221 formula raised to the 0.44 power, a sublinear relationship, so doubling deltaT increases the current rating by only about 2^0.44, roughly 1.36 times, not 2 times. Cross-sectional area has a bigger, though still sublinear, effect at the 0.725 power.
What copper thickness should I use for 1oz or 2oz copper?
1oz copper (the most common PCB copper weight) is about 1.378 mils thick (0.0348mm); 2oz copper is about 2.756 mils. "Ounce" here refers to the weight of copper per square foot of board, a standard PCB-industry way of specifying copper thickness rather than a direct thickness measurement — 1oz per square foot of solid copper spreads out to 1.378 mils thick.
Is IPC-2221 the only current-carrying-capacity standard for PCBs?
It's the most widely used industry reference, originally based on physical test data collected decades ago and still the default most PCB design tools and fabricators cite. Some designers and tools use updated or software-modeled current-capacity curves that account for more variables (trace length, board thickness, nearby copper pours), which can differ somewhat from IPC-2221's simplified two-constant formula — for a safety-critical or high-current design, cross-check against your fabricator's own guidance.