PCB Trace Width Calculator
Enter your design current, allowable temperature rise, copper weight, and trace length to get the minimum trace width required for safe operation. Results follow the IPC-2221 standard formulas used by professional PCB designers worldwide. The calculator covers both external and internal layers, and outputs trace resistance, voltage drop, and power dissipation so you can make a fully informed layout decision.
How the IPC-2221 formula works
The IPC-2221 standard gives the most widely accepted formula for sizing PCB trace width. It starts from the cross-section area needed to carry a given current without exceeding a maximum temperature rise: A = (I / (k x delta-T^0.44))^(1/0.725), where I is current in amperes, delta-T is the allowed rise in degrees Celsius, and k is a constant that accounts for the layer environment (0.048 for external traces, 0.024 for internal). Once you have the required cross-section area in square mils, the minimum trace width is simply area divided by the copper thickness. A 1 oz copper layer is 1.37 mils (35 micrometres) thick; 2 oz is 2.74 mils, and so on. Heavier copper reduces the required width because more current can flow through the thicker conductor.
External vs. internal layers
Outer layer traces are exposed to the environment and shed heat through convection and radiation. Inner layer traces are sandwiched between FR4 laminate, which is a poor thermal conductor (about 0.25 W/mK), so they run considerably hotter for the same current. The IPC-2221 formula captures this with the constant k: external (k = 0.048) allows roughly twice the current at the same width as internal (k = 0.024). In practical terms, an internal trace often needs to be about 50% wider than an external trace to carry the same current at the same temperature rise. When routing power traces through inner layers, always use the internal-layer formula and consider adding vias to stitch heat to the outer copper.
Resistance, voltage drop, and power loss
A copper trace is not a perfect conductor. Its resistance is R = rho x L / A, where rho is the resistivity of copper (approximately 1.724 x 10^-8 ohm-metres at 20 degrees Celsius), L is the trace length, and A is the cross-section area. As temperature rises, resistivity increases by about 0.393% per degree Celsius, so a trace running at 55 degrees Celsius has about 14% more resistance than at 20 degrees. The voltage drop is simply I x R, and the power dissipated is I squared x R. For a 1 A trace that is 50 mm long and 10 mils wide on 1 oz copper, the resistance is roughly 85 milliohms, the voltage drop is 85 mV, and the power loss is 85 mW. These figures matter most on high-current power rails, where even small voltage drops can fall outside component operating margins.
Safety margins and design practice
IPC-2221 gives the theoretical minimum trace width, but practical designs always add a safety margin. A 20% margin is a common starting point; safety-critical or high-reliability applications may use 40% or more. Other considerations include: manufacturing tolerance (most PCB fabs hold plus or minus 0.5 to 1 mil, so tight traces are more vulnerable), surface finish (thicker finishes can slightly increase current capacity), derating for elevated ambient temperatures (a trace designed for 25 degrees Celsius will run hotter if the board sits inside a warm enclosure), and proximity to other heat sources. Always check your final trace width against the minimum feature rules published by your board house, and round up to the nearest 5 mil increment to stay comfortably within their process window.
Typical trace width by current and copper weight (IPC-2221, external, 10 °C rise)
| Current (A) | 0.5 oz | 1 oz | 2 oz | 3 oz |
|---|---|---|---|---|
| 0.5 | 2.7 | 2.0 | 1.5 | 1.2 |
| 1 | 7.0 | 5.1 | 3.7 | 3.1 |
| 2 | 18.5 | 13.5 | 9.8 | 8.1 |
| 3 | 35.0 | 25.5 | 18.6 | 15.4 |
| 5 | 81.0 | 59.1 | 43.0 | 35.6 |
| 10 | 232.0 | 169.0 | 123.0 | 102.0 |
Minimum widths in mils. These are raw IPC-2221 values with no safety margin applied. Standard 1 oz copper at 10 °C rise is the most common design point.
Frequently asked questions
What is the IPC-2221 standard?
IPC-2221 is the Generic Standard on Printed Board Design published by IPC (the global electronics industry association). It provides the industry-standard empirical formula for calculating the minimum copper trace width needed to carry a specified current without the trace temperature rising above a safe limit. The formula was derived from empirical data and is accepted by PCB designers and manufacturers worldwide as the baseline reference.
How do I choose an allowable temperature rise?
A temperature rise of 10 degrees Celsius above ambient is the most common conservative design point and is appropriate for most signal and moderate-power traces. For rugged or high-reliability designs (automotive, aerospace, medical), 5 degrees is more conservative. For short-duration current bursts or cost-sensitive applications, up to 30 to 40 degrees is often acceptable. Remember that the final trace temperature is the ambient plus the rise, so if your board runs in a 70 degree enclosure and you allow a 30 degree rise, the copper will reach 100 degrees - approaching the lower limits of FR4.
Why does copper weight matter?
1 oz copper is 35 micrometres (about 1.37 mils) thick, which is the standard for most PCBs. 2 oz copper is 70 micrometres thick. Doubling the copper weight roughly halves the required trace width for the same current, because the same cross-section area fits into a narrower, taller profile. Heavier copper also lowers resistance and voltage drop. The trade-off is cost: 2 oz copper boards cost more to fabricate, and very heavy copper (3 oz or 4 oz) is a specialty process with longer lead times.
What is the difference between mils and millimetres in PCB design?
A mil (also written thou) is 1/1000 of an inch, or 0.0254 mm. Most North American PCB tools default to mils, while European and Asian tools often use millimetres. This calculator shows the result in both units. Common minimum trace widths are 3 to 5 mils (0.076 to 0.127 mm) for standard consumer PCBs, though advanced fabs can hold 2 mils or less.
When should I use a copper pour instead of a wide trace?
When your required trace width exceeds about 150 to 200 mils, or when you need to distribute heat evenly across a large area, a copper pour (flood) is usually a better approach. Pours fill the unused areas of a layer with copper, significantly reducing resistance and spreading heat. They also reduce electromagnetic radiation from high-current loops. Most EDA tools let you define a filled zone with a specific net; just ensure the pour is fully connected to the power rail and that thermal relief settings are appropriate for your via and pad sizes.