Solve for the trace width needed to carry your current at the temperature rise you can tolerate. Per IPC-2221 (conservative) or IPC-2152 (modern universal chart), internal or external, any copper weight, with resistance, voltage drop, and power dissipation included.
The IPC formulas treat a trace as if it sits in isolation. A real board has copper pours, vias, ground planes, and components that all affect heat flow. Drop your Gerber zip into the free Gerber Analyzer and run the built-in 3D thermal simulator on the actual layout. Place heat sources where they really sit, set the ambient and convection, and read the steady-state temperature across every copper layer.
Open the Gerber AnalyzerThe calculator solves the IPC current-capacity relationship for trace cross sectional area, then divides by the copper thickness to get the required trace width. Pick the standard you want to size against from the toggle above.
I is the current in amps, ΔT is the temperature rise above ambient in degrees Celsius, A is the cross sectional area in square mils. The constant k is 0.048 for external traces (outer layers, exposed to air) and 0.024 for internal traces (sandwiched between dielectrics). IPC-2221 is conservative: it ignores the cooling effect of nearby copper pours and planes, so it tends to call for wider traces than a real board needs.
IPC-2152 is the modern replacement, based on more recent test data with explicit accounting for substrate, plane proximity, and copper coverage. The full standard is chart-based; this calculator uses a curve-fit approximation of the IPC-2152 universal chart for a trace in still air on FR-4 (k ≈ 0.089 external, k ≈ 0.063 internal). For typical boards IPC-2152 allows about 1.5x to 2x the current of IPC-2221 at the same temperature rise. For exact numbers on a specific stackup, use the full chart or run a thermal simulation.
The "Nearby copper plane" toggle applies the IPC-2152 plane proximity correction. A plane within roughly 0.5 mm of the trace acts as a heat sink and increases ampacity by about 40%, allowing a narrower trace at the same temperature rise. The plane input only affects IPC-2152 results; IPC-2221 doesn't model plane proximity.
Resistance is computed from copper resistivity at 20 degrees Celsius (1.68 × 10-8 Ω·m), trace length, and the cross sectional area produced by the chosen standard. Voltage drop is current times resistance; power is current squared times resistance. At higher operating temperatures resistance grows by about 0.4% per degree.
Two: IPC-2221 (I = k · ΔT0.44 · A0.725, k = 0.048 external or 0.024 internal) and a curve-fit approximation of the IPC-2152 universal chart (I ≈ k · ΔT0.5 · A0.65, k ≈ 0.089 external or 0.063 internal). Toggle which one is used from the radio at the top of the inputs.
IPC-2221 is the conservative baseline and is widely accepted by reviewers. IPC-2152 is the modern revision and gives a more realistic answer for most boards, especially ones with copper pours and plane proximity. If in doubt, size to IPC-2221 and use IPC-2152 as the upper bound on what you can get away with.
Internal traces are surrounded by FR-4 substrate and have fewer paths to dissipate heat to air. Both standards reflect this: IPC-2221 uses roughly half the allowable current for internal traces; IPC-2152 has a smaller penalty (about 70%) because it accounts for heat spreading through nearby copper.
It applies the IPC-2152 plane proximity correction. A copper plane within roughly 0.5 mm of the trace acts as a heat sink, spreading heat away from the trace and allowing about 40% more current at the same temperature rise. The input only affects IPC-2152 (which models plane proximity); it has no effect on IPC-2221 results and is greyed out when IPC-2221 is selected.
10 to 20 degrees Celsius is a common general purpose target. High reliability or temperature sensitive boards should use a lower rise (5 to 10 degrees). The lower the allowed rise, the wider the required trace.
The full IPC-2152 standard is chart-based with adjustments for copper coverage, board thickness, plane proximity, and ambient. This calculator uses the universal chart (in still air on FR-4) which is the conservative IPC-2152 baseline. Real boards with planes and pours can do better. For exact analysis on a specific stackup, run a thermal simulation.
The product of trace width and copper thickness. A 1 mm wide trace on 1 oz copper (35 µm thick) has cross sectional area 0.035 mm². The formulas use square mils internally; the calculator converts for display.
Yes, at 20 degrees Celsius. Copper resistance grows by about 0.4% per degree, so a trace running hot will measure a few percent higher.