PCB Trace Width: Why It Matters and How to Calculate It

Why Trace Width Matters

A PCB trace is essentially a resistor. When current flows through it, the trace heats up due to resistive losses — just like a wire. If the trace is too narrow for the current it carries, it will overheat, causing:

Delamination of the copper from the substrate
Increased resistance as the copper oxidises and degrades
Open circuit failure if the trace melts or blows
Thermal stress on nearby components and solder joints

Choosing the correct trace width is a fundamental PCB design task, whether you are building a low-power sensor or a high-current motor driver.

The IPC-2221 Standard

The industry standard for trace width calculation is IPC-2221 (formerly IPC-D-275). It defines empirically derived formulas based on cross-sectional area, current, and acceptable temperature rise.

The standard distinguishes between:

External traces — on the outer layers of the PCB, exposed to air cooling
Internal traces — on inner layers, with less effective heat dissipation

Internal traces require roughly 2.5× the cross-sectional area of external traces for the same current and temperature rise, because they cannot radiate heat as effectively.

The IPC-2221 Formula

Step 1: Cross-Sectional Area

Area (mils²) = (I / (k × ΔT^b))^(1/c)

Where:

I = current in amps
ΔT = allowable temperature rise in °C above ambient
k, b, c = empirical constants from IPC-2221:
- External: k = 0.048, b = 0.44, c = 0.725
- Internal: k = 0.024, b = 0.44, c = 0.725

Step 2: Trace Width

Width (mils) = Area / (copper_thickness × 1.378)

Copper thickness is measured in ounces per square foot (oz/ft²):

Copper weight	Thickness
0.5 oz/ft²	0.7 mil (17.5 µm)
1 oz/ft²	1.4 mil (35 µm)
2 oz/ft²	2.8 mil (70 µm)

Most standard PCBs use 1 oz/ft² copper. Heavy copper boards (2–4 oz) are used for power electronics.

Worked Example

Requirement: Carry 3A on an external trace, maximum 10°C temperature rise, standard 1 oz copper.

Step 1 — Area:

Area = (3 / (0.048 × 10^0.44))^(1/0.725)
     = (3 / (0.048 × 2.754))^1.379
     = (3 / 0.1322)^1.379
     = (22.69)^1.379
     ≈ 90.3 mils²

Step 2 — Width:

Width = 90.3 / (1 × 1.378) ≈ 65.5 mils ≈ 1.66 mm

So you need a trace at least 1.66mm wide to safely carry 3A with a 10°C temperature rise on 1oz copper.

For comparison, the minimum trace width most PCB fabs can reliably manufacture is around 0.1–0.15mm (4–6 mils) — but this is a manufacturing limit, not a current-carrying limit. Power traces are often 1mm or wider.

Temperature Rise: What Is Acceptable?

The IPC-2221 standard typically uses 10°C as the maximum temperature rise for conservative designs. Some designers use 20°C or 30°C for less critical traces, but this should be weighed against:

Ambient temperature — if your board operates in a hot enclosure (50–70°C), adding 30°C brings you close to component limits
Derating — high reliability designs (mil-spec, medical) derate to 50% of calculated current
Adjacent sensitive components — temperature-sensitive components (precision references, crystals) benefit from keeping power traces cool

Resistance and Voltage Drop

Trace width also determines resistance, and therefore voltage drop under load:

R = ρ × L / A

Where:

ρ (resistivity of copper) ≈ 1.72 × 10⁻⁸ Ω·m
L = trace length
A = cross-sectional area

Example: A 50mm long, 1mm wide, 1oz trace (thickness 35µm):

A = 1mm × 0.035mm = 0.035 mm² = 3.5 × 10⁻⁸ m²
R = (1.72e-8 × 0.05) / 3.5e-8 ≈ 0.0246 Ω ≈ 24.6 mΩ

At 3A, the voltage drop is: V = I × R = 3 × 0.0246 ≈ 74mV. Negligible for 12V systems but significant for 3.3V logic.

Practical PCB Design Rules

Power traces (>0.5A): Calculate required width using IPC-2221, then add 20% margin.
Signal traces (<100mA): 0.2–0.25mm is standard; check your fab's minimum.
Return (ground) traces: Should be at least as wide as the supply trace they mirror.
Use polygons (copper pours) for high-current paths — they provide much more cross-section than even wide traces.
Keep power and signal traces separate — route power traces at the edge of the board or on a dedicated layer.
Multiple vias for layer transitions — a single via handles much less current than a trace; use multiple vias in parallel for power transitions between layers.

PCB Stackup and Layer Considerations

Layer type	Heat dissipation	Required width vs external
External (top/bottom)	Good — exposed to air	1×
Inner layers	Poor — sandwiched in FR4	~2.5× wider
Under solder mask	Slightly reduced	+10–15% safety margin

If your design has high-current traces on inner layers, consider bringing them to an outer layer for better heat dissipation, or use heavier copper on those layers.

Use the PCB Trace Width Calculator

The PCB Trace Width Calculator on DevGizmo implements the IPC-2221 formula. Enter your current, allowed temperature rise, copper weight, and layer type to instantly get the minimum trace width in both mils and millimetres.