PCB Trace Width Calculator

Calculate the minimum PCB trace width to carry a given current within a specified temperature rise using IPC-2221 formulas. Supports internal and external (outer-layer) traces in 1oz, 2oz, and 3oz copper.

Calculator Electronics Updated Oct 15, 2026
How to Use
  1. Enter the current your trace needs to carry.
  2. Pick allowed temperature rise (10-30°C typical; never exceed 45°C).
  3. Pick copper weight (1oz = 35µm thickness is standard; 2oz and 3oz for power).
  4. Pick internal (inner layer, less cooling) or external (outer, better cooling).
  5. The tool returns required width in mils and mm with a scale diagram.
Input
A
°C (10-30 typical)
mm
Presets
Trace Width (to scale)
Width (mil)
—mil
Width (mm)
—mm
Cross-Section
—mm²
Voltage Drop
—mV

Worked Example

A 3 A trace on an outer layer of 1 oz copper (1.38 mil thick), allowing a 10 °C rise. IPC-2221: I = 0.048 × ΔT0.44 × A0.725, so the cross-section A = (3 ÷ (0.048 × 100.44))1/0.725 = 74 mil², and the width is 74 ÷ 1.38 = 54 mil (1.37 mm).

On an inner layer the constant halves to 0.024 and the width grows to about 140 mil; in 2 oz copper the outer trace would be half as wide, 27 mil.

The common mistake: using a signal-trace width. A default 10 mil trace in 1 oz copper carries only about 0.9 A for a 10 °C rise. Size every power path, and for currents of several amps use copper pours rather than single traces.

Show Work

Enter values to calculate trace width.

Formulas (IPC-2221)

Required Area
A = (I / (k × ΔT0.44))1/0.725
Cross-section in mil². k: 0.048 external, 0.024 internal.
Width
W = A / (1.378 × oz)
In mils; 1oz copper = 1.378 mil thick.
Copper Thickness
t = 35 µm × oz
1 oz/sqft spread uniformly ≈ 35 µm.
Resistance / length
R/L = ρ / A
ρ(Cu) = 17.24 × 10⁻⁹ Ω·m.
Voltage Drop
V_d = I × R/L × L
Power dropped along the trace.
Constant k
k = 0.048 ext · 0.024 int
Empirical fit from IPC-2221 data.

About IPC-2221

The IPC-2221 standard is the industry reference for PCB current-carrying capacity. The empirical formula dates back to 1950s military research on the temperature rise of PCB conductors. Modern data shows it's quite conservative — most designs can safely carry 50-100% more current. However, for commercial and safety-critical designs, sticking with IPC-2221 values provides a well-documented margin against manufacturing variation, thermal cycling, and mechanical stress.

Key caveats: the formula assumes still air, ambient temperature, and no thermal vias or copper pours nearby. In practice, large ground pours, thermal vias, and even adjacent traces affect heat dissipation. For hot spots, CAD tools with thermal simulation give more accurate predictions.

History of Printed Circuit Boards

The printed circuit board was patented by Austrian engineer Paul Eisler in 1943 while living in the UK, initially for wartime radio manufacture. Early PCBs were single-sided with point-to-point copper etched on phenolic resin. Double-sided boards with plated-through holes followed in the 1950s, and multilayer boards in the 1960s alongside the first integrated circuits.

The current-versus-width chart goes back to measurements made in the 1950s and published in the US military standard MIL-STD-275. It passed into the IPC (Institute of Printed Circuits, now the Association Connecting Electronics Industries) standard IPC-D-275 and then IPC-2221 (1998) essentially unchanged, until IPC-2152 (2009) replaced it with new data.

Modern PCB design routinely violates 1960s-era assumptions: thermal vias act as mini-heatsinks, ground pours spread heat laterally, and high-density interconnect (HDI) boards operate above their nominal derating. Tools like Saturn PCB Design, Polar Si9000, and Altium's built-in calculators still default to IPC-2221 because it's a published, defensible reference — even when conservative.

About This Calculator

Enter the current, temperature rise (10°C conservative, 30°C aggressive), copper weight in ounces (1 oz = 35 µm), and layer type (external dissipates better than internal). The tool solves the IPC-2221 formula A = (I / (k × ΔT^0.44))^(1/0.725) for cross-sectional area, then divides by copper thickness to get width. Constants: k = 0.048 external, 0.024 internal.

Optional trace length adds a voltage drop estimate using copper resistivity ρ = 17.24 nΩ·m. For power-integrity work, allow at least 2× the IPC-2221 minimum on high-di/dt traces (switching converter outputs) so that inductance and skin effect don't dominate. Everything runs client-side; no values leave your browser.

Frequently Asked Questions

What does oz of copper mean?

A unit of PCB copper thickness: 1oz = 1.37 mil = 35µm (the thickness of 1 ounce of copper spread over 1 sq ft). 0.5oz is common for inner layers; 1oz is standard; 2-4oz for power supplies and high-current boards.

Why is internal vs external different?

Outer-layer traces dissipate heat both radiatively and via convection to air. Inner traces are buried in FR4 (a poor thermal conductor) and only conduct heat laterally through copper + vias. In IPC-2221 an inner trace is allowed half the current, which works out to about 2.6 times the width for the same current and temperature rise; the newer IPC-2152 data shows the real penalty is usually much smaller.

How safe is the IPC-2221 formula?

It's a conservative fit to empirical data from the 1950s. Modern boards with polyimide or ceramic substrates, thermal vias, and better copper plating can often handle 2-3× more current. But for safety-critical designs, stick with IPC-2221 and add a safety margin.

What temperature rise is safe?

10°C is a common conservative target — barely warm to the touch. 20°C is aggressive but reliable for intermittent loads. 30°C+ risks cracking solder joints over time due to thermal cycling. Never exceed 45°C for long-term operation.

Is there a newer standard than IPC-2221?

Yes. IPC-2152 (2009) replaced the old chart with new measurements and shows that board material, copper planes and trace length matter a lot; in many layouts inner traces do far better than IPC-2221 assumes. IPC-2221 remains the common quick check because it is simple and errs on the safe side.

How do I use the PCB Trace Width Calculator?

Just type your numbers. The answer shows up right away — there is no button to press. Change anything and it updates by itself.

Do I need to install or sign up for anything?

Not at all — it runs in the browser with nothing to install and no account. After it loads once, it even works without an internet connection.

Is my information private?

Yes. Everything happens in your browser. Nothing you type is sent to a server or saved anywhere.

Common Use Cases

Motor Controller Power Traces

A brushless motor driver carrying 10 A needs about 93 mil (2.4 mm) of 2 oz outer-layer copper for a 20 °C rise, or about 242 mil on an inner layer. Copper pours are the usual answer.

USB Power Delivery

USB-C at 5 A (up to 100 W at 20 V) needs about 109 mil (2.8 mm) of 1 oz outer copper for a 10 °C rise: much wider than a signal trace.

Buck Converter Output

A 3 A output needs about 54 mil of 1 oz outer copper for a 10 °C rise, or about 35 mil if a 20 °C rise is acceptable. Keep the high-current loop short and wide anyway, to cut noise.

LED Strip Driver

A 12 V, 60 W LED strip draws 5 A and needs about 71 mil of 1 oz outer copper at a 20 °C rise. Use wide pours near the regulator to spread its heat too.

Battery Charging Circuit

A 5 A Li-ion charger path on 1 oz outer copper needs about 109 mil for a 10 °C rise; add thermal vias under the charger IC's pad as well.

Last updated: