What is PCB trace width calculation
Every copper trace on a printed circuit board acts as a thin, flat wire. When electrical current flows through a trace, the copper resists that flow and generates heat. If the trace is too narrow for the current it carries, the temperature can rise high enough to damage solder joints, delaminate the board, or cause outright failure. PCB trace width calculation is the engineering process of determining how wide a copper trace must be to safely carry a given current without exceeding a specified temperature rise above the ambient environment.
The relationship between trace width and current-carrying capacity depends on several physical factors: the cross-sectional area of the copper, the thickness of the copper layer, whether the trace is on an external or internal layer, and how much heat the trace is allowed to generate. External traces sit on the outer surface of the board where convective cooling from the surrounding air helps dissipate heat. Internal traces are buried between insulating layers of the PCB stackup, so they have far less ability to shed heat and require wider widths for the same current.
Copper thickness on a PCB is traditionally specified in ounces per square foot. One ounce of copper spread over one square foot produces a layer approximately 1.378 mils (0.035 mm) thick. Common PCB specifications use 0.5 oz, 1 oz, 2 oz, or 3 oz copper, with 1 oz being the most common for standard designs and heavier weights reserved for power delivery and high-current applications.
Getting the trace width right matters at every stage of a product's life. An undersized trace creates a hidden reliability risk that may not appear during initial testing but can cause field failures under sustained load or elevated ambient temperatures. An oversized trace wastes board area that could be used for routing other signals or reducing the overall PCB size. Accurate calculation ensures the design is both safe and space-efficient.
The IPC-2221 standard
IPC-2221 is the generic standard on printed board design published by IPC (formerly the Institute for Printed Circuits). Section 6.2 of IPC-2221 provides the empirical formulas and charts that relate current, temperature rise, and copper cross-section to determine minimum trace widths for both internal and external layers.
The standard was developed from experimental data gathered by testing copper traces of various widths and thicknesses at different current levels and measuring the resulting temperature rise. Because it is based on empirical measurements rather than purely theoretical models, IPC-2221 includes built-in safety factors that account for real-world manufacturing tolerances. It remains the most widely referenced standard for PCB trace width sizing across the electronics industry.
The IPC-2221 constants differ between external and internal layers. External layers use k1 = 0.048, while internal layers use k1 = 0.024 (half the value), reflecting the reduced cooling capacity of buried traces. The exponents k2 = 0.44 and k3 = 0.725 are the same for both layer types.
How the formula works
The IPC-2221 calculation proceeds in two steps. First, determine the required cross-sectional area of copper:
**Cross-sectional area (mils squared):** \`\`\` Area = (Current / (k1 x DeltaT^k2))^(1/k3) \`\`\`
Where: - Current is in Amps - DeltaT is the allowable temperature rise in degrees Celsius - k1 = 0.048 for external layers, 0.024 for internal layers - k2 = 0.44 - k3 = 0.725
Second, convert the cross-sectional area into a trace width by dividing by the copper thickness:
**Trace width (mils):** \`\`\` Width = Area / (CopperOz x 1.378) \`\`\`
Where CopperOz is the copper weight in oz/ft squared and 1.378 converts ounces to mils of thickness.
To convert from mils to millimeters, multiply by 0.0254 (since 1 mil = 0.001 inch = 0.0254 mm).
The calculator also computes trace resistance per inch using the resistivity of copper (approximately 678.7 micro-ohm-mil-squared per inch) divided by the cross-sectional area, and the resulting voltage drop per inch as the product of current and resistance.
How to use this calculator
1. Enter the maximum current the trace must carry in Amps. Use the peak continuous current, not an average value, to ensure adequate margin. 2. Select the copper thickness from the dropdown. If unsure, 1 oz/ft squared is the most common choice for standard two-layer and four-layer boards. 3. Set the allowable temperature rise above ambient. A 10 degree Celsius rise is a common conservative default. Higher values allow narrower traces but reduce thermal margin. 4. Choose External or Internal layer using the toggle to see results for that layer type. 5. Review the hero result showing the required trace width in both mils and millimeters. 6. Check the practicality badge indicating whether the trace width is standard, very narrow, wide, or impractical. 7. Compare external and internal layer widths in the comparison section to understand how layer choice affects your design. 8. Use the resistance and voltage drop values to evaluate whether the trace introduces unacceptable losses in your power delivery path.
Design tips for high-current traces
- **Use thicker copper:** Moving from 1 oz to 2 oz copper cuts the required trace width nearly in half for the same current and temperature rise. If board space is tight, request heavier copper from your fabricator. - **Route on external layers when possible:** External traces benefit from convective cooling and require significantly less width than internal traces for the same current. - **Allow generous temperature rise:** A 10 degree Celsius rise is conservative. Many designs safely allow 20 to 30 degrees, which substantially reduces trace width. Verify that the total temperature (ambient plus rise) stays within component and solder joint ratings. - **Use multiple vias for layer transitions:** When a high-current trace changes layers, use multiple vias in parallel to reduce via resistance and improve current distribution. - **Add copper pours:** For very high currents, a solid copper pour (polygon fill) provides far more cross-sectional area than a single trace and improves thermal performance. - **Consider trace length:** The IPC formula gives width per unit of current and temperature rise. Long traces accumulate more voltage drop, so check total drop across the full trace path, not just per-inch values. - **Verify with your fabricator:** Manufacturing tolerances vary. Discuss minimum trace widths, copper weight options, and impedance requirements with your PCB manufacturer before finalizing the design.
FAQs
Q: What temperature rise should I use for my PCB design? A: A 10 degree Celsius rise is a common conservative starting point for most applications. Consumer electronics often use 10 to 20 degrees. Industrial and automotive designs may allow up to 30 degrees or more depending on the operating environment. The key constraint is that the total temperature (ambient plus trace rise) must remain within the ratings of all components and solder joints on the board.
Q: Why do internal layers require wider traces than external layers? A: Internal layers are sandwiched between insulating layers of the PCB laminate (typically FR-4). This insulation acts as a thermal blanket, trapping heat and preventing it from dissipating into the surrounding air. External layers are exposed to convective airflow, which removes heat much more efficiently. The IPC-2221 standard accounts for this by using a k1 constant for internal layers that is exactly half the external layer value, resulting in wider required widths.
Q: Is IPC-2221 accurate for very high currents above 35 Amps? A: The original IPC-2221 charts and formulas were derived from test data that primarily covered currents up to about 35 Amps. For higher currents, the extrapolated values may be less accurate. IPC-2152 is a newer standard that extends the data range and includes corrections for board thickness, copper plane proximity, and thermal conductivity. For designs above 35 Amps, consider using IPC-2152 or adding significant margin to IPC-2221 results.
Q: Can I use this calculator for flexible PCBs or metal-core boards? A: The IPC-2221 formula is based on standard rigid FR-4 boards. Flexible circuits (polyimide substrates) and metal-core PCBs (aluminum or copper base) have different thermal characteristics. Flexible circuits tend to be thinner with less thermal mass, while metal-core boards dissipate heat much more effectively. For these board types, the IPC-2221 results can serve as a rough starting point, but you should consult the specific material datasheets and consider thermal simulation for accurate results.
Q: What does the resistance per inch value tell me? A: Trace resistance per inch indicates how much electrical resistance each inch of trace adds to your circuit. Multiplying this by the total trace length gives the total trace resistance, and multiplying by current gives total voltage drop. This is critical for power delivery networks where even small voltage drops can affect regulator performance, battery charging accuracy, or signal integrity.
Explore Similar Tools
Explore more tools like this one:
- Ohm’s Law Calculator — Calculate Voltage, Current, or Resistance using Ohm's... - Current Calculator — Calculate electric current using Ohm's Law formulas: I =... - LED Resistor Calculator — Calculate the correct resistor value needed to safely... - Parallel Resistor Calculator — Calculate the total resistance of resistors connected in... - Resistance Calculator — Calculate electrical resistance, voltage, current, and...