PCB Trace Width Calculator
Trace width, current, temperature rise, resistance and vias — every formula shown.
| Result | Outer layer | Inner layer |
|---|
How it was calculated
Outer layer (k = 0.048)
Inner layer (k = 0.024)
Width for each copper weight
When to use IPC-2152 instead
Vias
Results are estimates from the formulas shown, not a professional design or certification. Have a qualified engineer verify anything safety-critical (structures, electrical installations, gas or pressure systems).
About the PCB Trace Width Calculator
Enter the current and the temperature rise you allow, choose the copper weight, and the calculator gives the trace width IPC-2221 asks for on an outer and an inner layer, in millimetres and mils. It also works the other way: the current a trace of a given width can carry, or how hot it runs at a given current.
Add the trace length to get its resistance at its working temperature, the voltage drop and the power it dissipates. A second section rates plated vias from the hole size and plating thickness and counts how many you need in parallel. Every result shows the formula and the numbers, and a note says when IPC-2152 — the newer, more detailed standard — should decide instead.
How to use it
- Choose what to solve for: the width for a current, the current for a width, or the temperature rise for a width and current.
- Enter the current and the temperature rise you accept above the board temperature — 10 °C is a common, conservative choice.
- Pick the copper weight (1 oz/ft² ≈ 35 µm) or enter the finished thickness your fabricator quotes. Outer layers are plated, so their finished copper is often thicker than the base foil.
- Optionally enter the trace length and the ambient temperature to see the resistance, voltage drop and power loss of that trace.
- Under Vias, enter the hole size, plating thickness and board thickness to see the current one via carries and how many you need. Copy result copies everything; Download CSV saves the copper-weight table.
Examples
Solve for width: 1 A, ΔT = 10 °C, 35 µm
A = (1 ÷ (0.048 × 10^0.44))^(1/0.725) = 16.30 mil² → outer layer 11.83 mil (0.300 mm); inner layer 30.77 mil (0.781 mm)
Solve for current: 0.508 mm (20 mil), 1 oz, ΔT = 10 °C
Outer layer 1.46 A · inner layer 0.73 A
0.300 mm × 35 µm, 50 mm long, ambient 25 °C
At 35 °C: ρ = 0.018258 Ω·mm²/m → R = 86.8 mΩ, so 86.8 mV drop and 86.8 mW loss at 1 A
0.3 mm finished hole, 25 µm plating, 1.6 mm board, ΔT = 10 °C
Barrel 0.0255 mm² (39.6 mil²) → about 1.9 A per via; 1.14 mΩ each
The formulas
- IPC-2221 (curve fit to its conductor charts): I = k × ΔT^0.44 × A^0.725, with I in amps, ΔT the temperature rise in °C and A the cross-section in square mils; k = 0.048 for outer layers and 0.024 for inner layers
- Cross-section for a current: A = (I ÷ (k × ΔT^0.44))^(1/0.725); the width is W = A ÷ t, with t the copper thickness in mils
- Temperature rise: ΔT = (I ÷ (k × A^0.725))^(1/0.44)
- Resistance: R = ρ20 × (1 + α × (T − 20)) × L ÷ (W × t), with the IEC 60028 values for annealed copper ρ20 = 1/58 Ω·mm²/m (0.017241) and α = 0.00393 per °C, and T = ambient + rise
- Voltage drop and loss: V = I × R, P = I² × R
Copper weight and thickness
Copper weight is the mass of copper on one square foot: 1 oz/ft² is about 35 µm (1.38 mil) thick, so 0.5 oz ≈ 17.5 µm, 2 oz ≈ 70 µm and 3 oz ≈ 105 µm. This calculator uses 35 µm per ounce. Outer layers are usually built from thinner foil and then plated, and etching leaves a trace slightly narrower at the top than at the bottom — use the finished thickness from your fabricator for the most accurate result.
IPC-2221 or IPC-2152?
The IPC-2221 charts go back to tests the US National Bureau of Standards made in 1956 on outer-layer conductors; the inner-layer chart is the outer one derated to half the current. IPC-2152 (2009) replaced them with new measurements and correction factors for board thickness, copper planes nearby, board material and vacuum. Its data shows inner traces generally run no hotter than outer traces of the same size.
IPC-2221 is quick and conservative, which is why it is still widely used for first-pass sizing. Use IPC-2152 — or a thermal simulation — when board space matters, on inner layers, for currents above a few amps, on thin boards or boards with planes, and for anything that operates in vacuum.
Vias
IPC-2221 has no formula for vias. A common, conservative convention rates the plated barrel like a trace of the same cross-section: A = π × t × (D − t), where D is the drilled hole (the outside of the plating) and t the plating thickness. A finished hole of 0.3 mm with 25 µm plating has a 0.35 mm drilled hole and carries about 1.9 A at a 10 °C rise. IPC-6012 asks for an average barrel plating of 20 µm for Class 2 boards and 25 µm for Class 3. Spread a high current over several vias.
Sources
- IPC-2221B (2012), Generic Standard on Printed Board Design, §6.2 — conductor current capacity and the curve-fit constants
- IPC-2152 (2009), Standard for Determining Current-Carrying Capacity in Printed Board Design
- IEC 60028, International standard of resistance for copper — ρ20 = 1/58 Ω·mm²/m, α20 = 0.00393 /K
- IPC-6012, Qualification and Performance Specification for Rigid Printed Boards — plating thickness in holes
Limitations
- The IPC-2221 formula is a curve fit to its charts, commonly quoted as valid up to 35 A on outer layers (17.5 A inner), 400 mil wide, 10–100 °C rise and 0.5–3 oz copper; outside that range the tool warns that it is extrapolating.
- It assumes a single trace on its own in still air. Neighbouring traces, copper planes, hot parts, enclosures, forced air and altitude all change the real temperature.
- Currents are steady DC or RMS. Short pulses, fusing current, skin effect at high frequency and inductance are not covered.
- Via ratings use a convention, not a standard formula. Thermal vias, filled vias and vias into planes behave differently.
Privacy
Everything happens in your browser. What you enter or open here is not uploaded or stored by MySmartCoPilot.
Frequently asked questions
How wide should a PCB trace be for 1 amp?
With 1 oz copper and a 10 °C rise, IPC-2221 gives 0.30 mm (11.8 mil) on an outer layer and 0.78 mm (30.8 mil) on an inner layer. Allowing a 20 °C rise or using 2 oz copper makes the trace narrower — try them in the calculator.
What does 1 oz copper mean in a PCB?
One ounce of copper spread over one square foot, which is about 35 µm (1.38 mil) thick. 2 oz copper is about 70 µm and carries the same current in roughly half the width.
Why is the inner-layer trace so much wider?
IPC-2221 rates inner traces at half the current of outer ones, because its inner chart was made by halving the outer chart. For the same current the cross-section then grows by 2^(1/0.725) ≈ 2.6. IPC-2152’s newer data shows this is very conservative for most stack-ups.
How much temperature rise should I allow?
Many designers use 10 °C as a safe default. A larger rise saves width, but the trace runs hotter, its resistance rises by about 0.4% per °C, and it warms the parts around it. Keep ambient plus rise well below the board’s and the parts’ temperature ratings.
How much current can a via carry?
Rated like a trace of the same copper cross-section, a typical via with a 0.3 mm finished hole and 25 µm plating carries about 1.9 A at a 10 °C rise. Use several vias for higher currents; the calculator counts them for you.
Should I use IPC-2221 or IPC-2152?
IPC-2221 is the quick, conservative estimate shown here. IPC-2152 is the newer standard with correction factors for the board, planes and environment; use it for final designs, inner layers and high currents.