PCB Trace Current Calculator: Max Current, Width and Temp Rise
Enter your trace width, copper weight, layer position, and allowable temperature rise to find the maximum current your PCB trace can safely carry. The calculator follows the IPC-2221 standard and also computes trace resistance, voltage drop, and power dissipation. Switch the mode to solve for trace width or temperature rise instead, and toggle between metric and imperial units.
What is the IPC-2221 PCB trace current formula?
The IPC-2221 standard (Generic Standard on Printed Board Design) provides a widely used empirical formula for estimating how much current a PCB copper trace can carry before its temperature exceeds an acceptable limit. The formula is I = k x dT^0.44 x A^0.725, where I is the current in amperes, k is a layer coefficient (0.048 for outer layers, 0.024 for inner layers), dT is the allowable temperature rise in degrees Celsius, and A is the trace cross-sectional area in square mils. The IPC-2221 coefficients were derived from a curve-fit to empirical chart data that first appeared in IPC-D-275 and have been carried forward through IPC-2221A and subsequent revisions. A newer standard, IPC-2152, extends the model with additional parameters such as copper plane proximity and substrate thermal conductivity; this calculator implements the widely adopted IPC-2221 version, which is sufficient for most standard FR4 designs.
How to use this calculator
Select your calculation mode at the top. "Maximum current" finds how many amperes a trace of a given width can carry. "Required trace width" finds the minimum width for a target current. "Temperature rise" finds how hot a specific trace will get at a given current. Enter the trace width (or target current for the width mode), the copper weight, whether the trace is on an outer or inner layer, and the allowable temperature rise. Optionally add trace length and ambient temperature to compute resistance, voltage drop, and power dissipation. Switch between metric (millimetres) and imperial (mils) using the width units selector. The "Show your work" panel below the results walks through every formula step with your actual numbers.
Copper weight, thickness, and why they matter
Copper weight is specified in ounces per square foot (oz/ft^2). One ounce corresponds to a thickness of about 35 micrometres (1.378 mils). The cross-sectional area of a trace is simply its width multiplied by its copper thickness. A larger area means lower resistance and higher current capacity. Doubling the copper weight from 1 oz to 2 oz roughly doubles the cross-sectional area and increases current capacity by about 65% (because of the 0.725 exponent on area in the formula). Standard copper weights for commercial PCBs are 0.5, 1, and 2 oz/ft^2; 3 and 4 oz are used for high-power boards but add cost and reduce etch precision.
Design guidelines and safety margins
IPC-2221 is an empirical approximation, not a guaranteed limit. Industry practice is to apply a derating factor of 20-50% below the calculated maximum. Use a 10 deg C temperature rise for conservative signal-integrity applications; 20-30 deg C is acceptable for power traces where a bit of thermal headroom exists. Always verify that the final trace temperature (ambient plus rise) stays well below your PCB material's glass-transition temperature (Tg). Standard FR4 has a Tg of roughly 130-170 deg C. For parallel traces or dense trace bundles, current capacity is reduced because heat dissipation is impaired; increase width or spacing in those areas. Internal layers run hotter than outer layers at the same current because they lack convective air cooling, which is why the IPC-2221 coefficient for internal layers is half that for external layers.
IPC-2221 current capacity reference (1 oz copper, 10 deg C rise)
| Width (mm) | Width (mil) | Outer layer (A) | Inner layer (A) |
|---|---|---|---|
| 0.13 | 5 | 0.35 | 0.18 |
| 0.25 | 10 | 0.71 | 0.36 |
| 0.5 | 20 | 1.31 | 0.66 |
| 0.76 | 30 | 1.78 | 0.89 |
| 1 | 39 | 2.22 | 1.11 |
| 1.27 | 50 | 2.69 | 1.35 |
| 1.5 | 59 | 3.06 | 1.53 |
| 2 | 79 | 3.82 | 1.91 |
| 2.54 | 100 | 4.56 | 2.28 |
| 3 | 118 | 5.18 | 2.59 |
Approximate maximum current in amperes for common trace widths per IPC-2221. Outer layers use k = 0.048, inner layers k = 0.024.
Frequently asked questions
What is the difference between IPC-2221 and IPC-2152?
IPC-2221 is an older standard whose current-capacity chart data was curve-fitted into the formula I = k x dT^0.44 x A^0.725. It is simple and widely used but does not account for nearby copper planes, PCB thickness, or substrate thermal conductivity. IPC-2152 is a newer standard that provides more accurate results by incorporating these parameters through additional correction factors. For most standard FR4 boards without embedded copper planes directly adjacent to the trace, IPC-2221 gives a reasonable estimate. For high-density boards with internal copper pour layers, IPC-2152 is more accurate.
How do I convert copper weight (oz/ft^2) to thickness?
Multiply the copper weight in ounces per square foot by 1.378 to get the thickness in mils, or by 34.975 to get it in micrometres. So 1 oz copper is approximately 1.378 mil (35 µm), 2 oz is about 2.756 mil (70 µm), and 0.5 oz is about 0.689 mil (17.5 µm). This conversion is the starting point for calculating the trace cross-sectional area.
Why does layer position (internal vs external) matter so much?
Outer (external) traces are exposed to air, so they dissipate heat by convection. Inner traces are surrounded by FR4 substrate, which is a poor thermal conductor, so heat has fewer escape paths. The IPC-2221 formula captures this with the coefficient k: 0.048 for outer layers and 0.024 for inner layers. This means an inner trace carries only about half the current of an outer trace of the same dimensions at the same allowable temperature rise.
What allowable temperature rise should I use?
IPC-2221 originally presented charts at 10 deg C and 30 deg C rises. For most commercial designs, 10 deg C is the conservative, widely accepted default. A 20-30 deg C rise is used for power planes and high-current traces where cost or space is a constraint and a full thermal budget analysis has been done. Values above 30 deg C are generally discouraged because they approach the limits of the solder joint and substrate materials, especially in high-ambient-temperature environments such as automotive or industrial applications.
What is voltage drop and why does it matter for PCB traces?
Every copper trace has a small DC resistance determined by its cross-section and length. When current flows through this resistance, the voltage at the far end of the trace is slightly lower than at the source end. This voltage drop equals the current times the resistance (V = I x R). For power traces, a large voltage drop means less voltage reaches the load, which can cause malfunction or performance degradation. A good design target for supply rails is a voltage drop below 1-3% of the supply voltage. This calculator computes the drop across the trace at the maximum or specified current.
How do I calculate trace resistance at elevated temperatures?
Copper resistance increases with temperature. The formula is R_op = R_20 x (1 + alpha x (T_op - 20)), where alpha = 0.00393 per degree Celsius for copper and T_op is the operating temperature in degrees Celsius. The base resistance R_20 = rho x L / A, where rho is the resistivity of copper (about 1.724e-8 ohm-m) and L and A are the length and cross-sectional area of the trace. This calculator applies the temperature correction automatically using the ambient temperature and the computed or entered temperature rise.
Should I add a design margin to the IPC-2221 result?
Yes. IPC-2221 is an empirical approximation that does not account for every real-world factor: trace surface finish, solder mask coverage, proximity to other traces, board orientation, or convection conditions. Standard practice is to derate by 20-50% below the IPC-2221 maximum. For a simple way to add margin, calculate the width for a target current at a 10 deg C rise instead of the typical 20-30 deg C, which naturally gives a wider, lower-resistance trace.