You're laying out a PCB and need to run 3 amps through a power trace. How wide does it need to be? Too narrow and the trace overheats, maybe even delaminates your board. Too wide and you're wasting real estate that could be used for routing.
The answer comes from IPC-2221, the industry standard for PCB trace current capacity. Let's walk through how it works and how to apply it to your designs.
What Is IPC-2221?
IPC-2221 is the generic standard for PCB design published by the IPC (Association Connecting Electronics Industries, formerly the Institute for Printed Circuits). It's titled "Generic Standard on Printed Board Design" and covers everything from trace width to via sizes to board stackup.
Section 6 of IPC-2221 addresses conductive traces, and the charts in that section relate trace width, copper weight, and current-carrying capacity to temperature rise. These charts are what most online trace width calculators are based on.
There's also IPC-2152, "Standard for Determining Current-Carrying Capacity in Printed Board Design," published in 2009 as a more accurate replacement for the IPC-2221 charts. IPC-2152 accounts for more variables (board material, adjacent copper planes, etc.) and generally gives less conservative results. We'll cover the differences later, but IPC-2221 remains the most widely used reference because it's simpler and has a built-in safety margin.
The IPC-2221 Trace Width Formula
The IPC-2221 charts were curve-fitted to produce equations. For external traces (on outer layers), the most commonly used approximation is:
I = k × ΔT^0.44 × (W × T)^0.725
Where:
- I = current in amps
- ΔT = allowable temperature rise above ambient in °C
- W = trace width in mils (1 mil = 0.001 inch = 0.0254 mm)
- T = copper thickness in mils
- k = constant (0.048 for external traces, 0.024 for internal traces)
Rearranging to solve for width:
W = [I / (k × ΔT^0.44)]^(1/0.725) / T
Internal traces have a lower k value because they can't dissipate heat as well — they're surrounded by FR-4 dielectric instead of air. As a rule of thumb, an internal trace needs to be roughly 2× wider than an external trace for the same current.
A Real Example: 3 Amps on an External Layer
Let's calculate the trace width for a 3A power trace on an external layer with 1 oz copper:
- Current = 3A
- ΔT = 10°C (we're allowing a 10°C rise above ambient)
- Copper weight = 1 oz (standard), which equals 1.37 mils (34.8 µm) thickness
- Layer = external (k = 0.048)
W = [3 / (0.048 × 10^0.44)]^(1/0.725) / 1.37
W = [3 / (0.048 × 2.754)]^(1.379) / 1.37
W = [3 / 0.1322]^1.379 / 1.37
W = [22.69]^1.379 / 1.37
W = 59.1 / 1.37
W = 43.1 mils ≈ 1.1 mm
So you need roughly a 43 mil (1.1 mm) trace for 3A with a 10°C temperature rise on 1 oz external copper. That's a reasonable width for most board layouts.
What If It's on an Internal Layer?
Same parameters but k = 0.024:
W = [3 / (0.024 × 2.754)]^(1.379) / 1.37
W = [45.38]^1.379 / 1.37
W = 145.7 / 1.37
W = 106.3 mils ≈ 2.7 mm
Over 100 mils — more than double. This is why power routing is usually done on external layers when possible.
Temperature Rise: How to Choose ΔT
The ΔT you select depends on your application:
| ΔT | When to Use |
|---|---|
| 10°C | Tight thermal budget, dense boards, enclosed products with limited airflow |
| 20°C | General purpose — most consumer electronics |
| 30°C | Open-air designs, industrial equipment with good ventilation |
A 10°C rise is conservative and works for almost everything. But if you're designing a tiny IoT device in a sealed plastic enclosure, even 10°C might be too much. You need to think about the total thermal budget — trace heating plus component heating plus ambient temperature.
For context: FR-4 glass transition temperature (Tg) is typically 130-180°C. If your board runs at 70°C ambient and you allow a 30°C rise, you're at 100°C — well within limits. But stack up enough heat sources and a high ambient, and you can get uncomfortable.
Copper Weight Reference
Standard copper weights and their actual thicknesses:
| Copper Weight | Thickness (µm) | Thickness (mils) | Use Case |
|---|---|---|---|
| 0.5 oz | 17.5 | 0.69 | Signal layers, fine-pitch routing |
| 1 oz | 35 µm | 1.37 | Default for most layers |
| 2 oz | 70 µm | 2.74 | Power distribution, high current |
| 3 oz | 105 µm | 4.13 | Very high current (rare in standard boards) |
If you're running heavy current (5A+), moving from 1 oz to 2 oz copper can halve your required trace width. The board cost goes up, but you save routing space.
Quick Reference: Trace Width vs Current (1 oz External, ΔT = 10°C)
| Current (A) | Width (mils) | Width (mm) |
|---|---|---|
| 0.5 | 10 | 0.25 |
| 1.0 | 18 | 0.46 |
| 1.5 | 26 | 0.66 |
| 2.0 | 34 | 0.86 |
| 3.0 | 43 | 1.1 |
| 4.0 | 57 | 1.4 |
| 5.0 | 70 | 1.8 |
| 7.0 | 100 | 2.5 |
| 10.0 | 152 | 3.9 |
Use this as a sanity check during layout. If your 5A trace is 20 mils wide, stop and recalculate.
IPC-2221 vs IPC-2152: What Changed?
IPC-2152, published in 2009, replaced the original IPC-2221 current charts with more accurate data. Key differences:
IPC-2152 accounts for:
- Board material (FR-4 vs. polyimide vs. flexible substrates)
- Copper plane proximity (a ground plane under your trace dramatically improves heat dissipation)
- Board thickness
- Whether the trace is in still air, forced air, or vacuum
Practical impact: IPC-2152 typically allows narrower traces than IPC-2221 for the same current, especially when you have copper planes nearby. The IPC-2221 charts are conservative — they assume worst-case conditions with no heat sinking from adjacent copper.
For production designs where trace width impacts board size or cost, IPC-2152 can save you real estate. For prototyping or quick-turn designs, IPC-2221's built-in safety margin is a feature, not a bug.
Practical Tips
Add margin. Don't design to the exact calculated width. Add 20-30% margin for manufacturing variations, copper etch tolerance, and unexpected current spikes. Copper thickness can vary ±10% from the nominal value.
Check your fab house specs. Most PCB manufacturers have minimum trace width requirements (typically 4-6 mils for standard 1 oz). But the minimum recommended width for current-carrying traces is much wider.
Use copper pours for high current. Instead of a single wide trace, flood unused areas with copper pour connected to your power net. This is standard practice for power supplies and motor driver boards.
Consider thermal reliefs. When connecting wide power traces to component pads, thermal reliefs (those spoke-like connections) make soldering easier but add resistance. For high-current pads, consider solid connections instead.
Don't forget vias. A standard via has limited current capacity — roughly 0.5A for a 10-mil via with 1 oz plating. For power transitions between layers, use multiple vias in parallel (via stitching) or larger vias with heavier plating.
A Note on Transient Currents
The IPC formulas assume steady-state current. If your trace carries pulsed current (like a motor driver or switching regulator output), the average current is what matters for heating. A 10A pulse at 10% duty cycle has the same thermal impact as 1A continuous.
But check the peak current too — a narrow trace acts like a fuse during a short circuit. If you need fault protection, trace width alone isn't enough. Add a proper fuse or current-limiting device.
Don't want to work through these formulas by hand? The PCB Trace Width Calculator lets you enter your current, copper weight, and allowed temperature rise, then gives you the minimum trace width for both internal and external layers. It uses the IPC-2221 curve-fit equations and handles unit conversions automatically — mils, mm, or inches, whatever you prefer. Give it a try on your next board layout.