Pcb Trace Width Calculator

Sizing a copper trace is a thermal problem, not an electrical one. The trace has resistance, resistance times current squared produces heat, and the width must be large enough that the resulting temperature rise stays acceptable. IPC-2221 expresses this empirically as A = (I / (k x dT raised to b)) raised to 1/c, with A the cross sectional area in square mils, dT the allowable rise above ambient in degrees C, b = 0.44, c = 0.725, and k = 0.048 for external layers or 0.024 for internal layers. Width follows by dividing area by copper thickness, where the standard weights are 0.5 oz at 0.689 mils, 1 oz at 1.378 mils or about 35 micrometers, and 2 oz at 2.756 mils. A representative result is roughly 45 mils, about 1.15 mm, for 3 A on an external 1 oz layer at a 10 degree C rise. Typical design targets are a 10 degree C rise for consumer and signal boards, 20 degrees for industrial work, and up to 40 degrees only where thermal management is deliberate; FR-4 laminate has a glass transition temperature of roughly 130 to 180 degrees C, and rise is measured above ambient, so a 60 degree C enclosure consumes most of the headroom. The formula's weaknesses are well known. It was derived for isolated traces and takes no account of adjacent copper pours, ground planes, board thickness, airflow, or vias, which frequently form the real bottleneck in a current path. The 2:1 internal to external penalty is now considered pessimistic, since buried copper is conducting heat into laminate rather than sitting in still air. Fabrication tolerance on etched width can reach plus or minus 20 percent, so most designers add 10 to 25 percent margin, and more for pulsed or safety critical currents.

The current capacity curves behind this calculation originate in mid twentieth century military printed wiring practice rather than in modern PCB work. MIL-STD-275, the United States military standard for printed wiring for electronic equipment, published nomographs of conductor width against current and temperature rise that were built from empirical measurements on isolated traces, with derating applied for safety. Those charts were carried forward as the industry moved to civilian standards bodies, appearing in IPC-D-275, the joint IPC and military design standard, before being folded into IPC-2221 when IPC published its generic printed board design standard in 1998. IPC itself was founded in 1957 as the Institute of Printed Circuits. Because the underlying data was old and its test conditions were poorly documented, IPC funded a ground up re-measurement program that produced IPC-2152, released in 2009. That study varied copper weight, laminate thickness and material, board size, and environment, including tests in vacuum, and found that the classic charts were conservative in some regimes and optimistic in others. Its most cited conclusion was that the traditional halving of capacity for internal layers is generally wrong, since internal traces are surrounded by laminate that conducts heat away rather than air that insulates them. IPC-2152 replaced simple curves with a family of charts requiring board specific inputs. IPC-2221 nonetheless remains in wide use for quick sizing, precisely because it needs only current, temperature rise, copper weight, and a layer choice.