Technology Never Stands Still, and Neither Do We
Validated Mini-ITX platforms engineered for reliable deployment in industrial, edge, and embedded system environments.
PCB CURRENT-CARRYING CAPACITY TOOL
PCB Trace Width Calculator
Calculate a minimum PCB trace width, add an engineering margin, or check the current capacity of an existing trace using an IPC-2221-style empirical model. The tool also estimates resistance, voltage drop, power loss, current density, and conductor temperature.
External and internal layers
mm, mil, °C, and °F
Width sizing and trace checking
COPPER ROUTE
THERMAL SCREEN
MODEL
IPC-2221 STYLE
DEFAULT LAYER
EXTERNAL
RECOMMENDED W
8.99 mm
INTERACTIVE COPPER SIZING
Size a New Trace or Check an Existing Route
Enter finished copper geometry and the permitted temperature rise. Results update immediately and remain a preliminary screening estimate rather than a production thermal guarantee.
DESIGN INPUTS
Electrical and Copper Parameters
A
µm
°C
mm
°C
%
mm
ACTIVE TRACE MODEL
External Copper Trace
W
T
- Minimum W
- 7.194 mm
- Selected W
- 8.993 mm
- Copper T
- 35.0 µm
- Length L
- 150.0 mm
IPC-2221-style screening equation
I = k × ΔT0.44 × A0.725
A is copper cross-sectional area in square mils. The recommended width applies the user-selected design margin after solving the minimum area.
Inputs are within the calculator screening limits
RECOMMENDED ENGINEERING WIDTH
8.99 mm
354.05 mil · 0.3541 in
DESIGN SCREEN
25% width margin applied
Use the recommended width as a layout starting point, then verify the production stackup and thermal environment.
Minimum Width
7.194 mm
Estimated Capacity
11.76 A
Capacity Utilization
85.0%
Trace Resistance
8.700 mΩ
Voltage Drop
87.00 mV
Power Loss
870.03 mW
Current Density
31.77 A/mm²
Conductor Temperature
35.0 °C
CALCULATION BASIS
How the PCB Trace Width Estimate Is Calculated
The calculator uses the familiar IPC-2221 empirical current-capacity relationship for fast trace sizing. It then derives electrical loss from finished copper cross-section and temperature-adjusted copper resistivity.
Required Copper Area
A = [I ÷ (k × ΔT0.44)]1/0.725
The coefficient is 0.048 for an external trace and 0.024 for an internal trace. Area is solved in square mils.
Minimum and Recommended Width
Wmin = A ÷ T · Wrec = Wmin(1 + margin)
Finished copper thickness converts the required area into width. The design margin is explicit and adjustable rather than hidden.
Resistance and DC Loss
R = ρ(T) × L ÷ (W × T)
Resistance is adjusted to ambient plus the selected temperature rise, then used to estimate voltage drop and I²R loss.
Existing Trace Check
Icapacity = k × ΔT0.44 × (W × T)0.725
Check Existing Trace reverses the workflow and compares applied current with the empirical capacity of the entered finished width.
Engineering interpretation:
IPC-2221 is a legacy empirical screening approach. IPC-2152-style correlation, copper planes, nearby conductors, enclosure airflow, substrate construction, solder mask, and board-level thermal spreading can produce different temperatures. Use this result to start layout and fabrication discussion, not to certify a released design.
INPUT QUALITY
Use Finished Copper Values and a Realistic Thermal Boundary
The model is simple, but the result depends strongly on whether current, copper thickness, layer location, and temperature rise reflect the actual PCB construction.
Continuous Current
Enter the sustained route current, not only a typical operating value. Pulsed loads require separate transient and duty-cycle evaluation.
Finished Copper Thickness
Use the finished conductor thickness after fabrication. Nominal copper weight is a convenient preset, but plated outer-layer copper can differ.
Allowed Temperature Rise
This is the permitted rise above ambient, not the maximum component or laminate rating. Lower rise targets produce wider traces.
Finished Route Length
Length does not change the IPC-2221 width result, but it directly changes resistance, voltage drop, and power loss.
ENGINEERING BOUNDARY
What the Calculator Includes and What Still Requires Validation
Included in the Estimate
- External and internal IPC-2221-style coefficients
- Finished copper thickness and explicit width margin
- Metric and imperial geometry conversion
- Celsius and Fahrenheit temperature conversion
- Resistance, voltage drop, power loss, and current density
Verify Outside the Calculator
- IPC-2152 correlation and production thermal testing
- Copper pours, parallel paths, neck-downs, vias, and pads
- Airflow, enclosure temperature, and nearby heat sources
- Plane coupling, substrate thickness, and copper distribution
- Fabrication tolerance, plating, etch profile, and solder mask
FROM CALCULATOR TO RELEASE EVIDENCE
Use the estimate with stackup review, current-path inspection, and system-level thermal validation.
COPPER REFERENCE
Nominal Copper Weight and Thickness Conversion
These common nominal conversions are useful for preliminary input. Confirm the finished copper thickness with the PCB fabricator, especially for plated outer layers.
| Copper Weight | Nominal Thickness | Thickness in mil | Typical Planning Use |
|---|---|---|---|
| 0.5 oz/ft² | 17.5 µm | 0.69 mil | Fine routing and light-current layers |
| 1 oz/ft² | 35 µm | 1.38 mil | General-purpose PCB copper |
| 2 oz/ft² | 70 µm | 2.76 mil | Higher-current power distribution |
| 3 oz/ft² | 105 µm | 4.13 mil | Heavy-copper industrial power paths |
| 4 oz/ft² | 140 µm | 5.51 mil | Specialized high-current construction |
NEXT ENGINEERING CHECKS
Continue the PCB and System Design Workflow
Move from conductor sizing into route loss, copper specification, via capacity, impedance, power planning, thermal screening, and Mini-ITX system validation.
PCB DESIGN
Copper, Loss, and Signal Integrity
POWER AND THERMAL
System Load and Cooling Checks
MINI-ITX SYSTEM
Mechanical, Power, and Reliability
PCB TRACE WIDTH FAQ
Practical Questions Before Releasing a High-Current Route
Use the calculator for early sizing, then verify the complete current path and production stackup.
The answers below explain copper thickness, internal versus external layers, temperature rise, margins, and the limits of an IPC-2221-style estimate.
Discuss a PCB Power PathWhat formula does this PCB trace width calculator use?
It uses the IPC-2221-style empirical relationship between current, allowed temperature rise, copper cross-sectional area, and layer location. The solved area is divided by finished copper thickness to obtain trace width.
Why is the internal-layer trace much wider?
The legacy equation uses a lower coefficient for internal conductors, representing less favorable heat dissipation. Actual multilayer behavior also depends on nearby planes, dielectric thickness, copper distribution, and board construction.
Should I use minimum width or recommended width?
The minimum width is the direct empirical result. The recommended width adds your selected engineering margin and is normally the better starting point when routing space allows.
Does trace length change the required width?
Trace length does not enter the IPC-2221 width equation. It does increase resistance, voltage drop, and power loss, which may require a wider route even when current capacity appears adequate.
Can I split the current across two parallel traces or copper layers?
Parallel paths can share current, but the split may not be equal because of geometry, via resistance, component placement, and thermal coupling. Model and validate the complete current path rather than dividing width by path count automatically.
Can this calculator replace IPC-2152 analysis or thermal testing?
No. This is a preliminary IPC-2221-style screening tool. Final designs should consider IPC-2152 guidance, fabrication tolerances, enclosure conditions, copper spreading, and measured thermal performance.