How to calculate PCB track width on proteus?

Question

The current in my circuit is 60A and voltage is 36V. How wide should the tracks on my PCB be?

Answer 1

You'll need it wide, and thick if you can (2 oz copper vs 1 oz copper). There are calculators like this one https://www.4pcb.com/trace-width-calculator.html that take into account current, copper thickness, allowed heat rise, internal or external trace, trace length into account and calculate a trace width. Other board houses have calculators also.

Answer 2

If you do this, you will melt the track

^{simulate this circuit – Schematic created using CircuitLab}

Answer 3

This is not determined by board houses or PCB design software, but by IPC standards. IPC-2221A Section 6.2 states:

The minimum width and thickness of conductors on the finished board shall be determined primarily on the basis of the current-carrying capacity required, and the maximum permissible conductor temperature rise.

The formula provided in the standard is:

$$ I=k\Delta T^{0.44}A^{0.725} $$

where:

• \$I\$ is the current handling requirement in amperes
• \$\Delta T\$ is the allowed temperature rise of the trace in degrees Celsius
• \$A\$ is the the cross-sectional area of the trace in square mils
• \$k\$ is a constant which equals 0.048 for outer layer traces, or 0.024 for inner layer traces.

The cross-sectional area is determined by your trace width and your copper weight (measured in mils, millimeters, or oz/ft^2). If you don't want to do the math by hand, there are certainly plenty of calculators out there on the net. My point is that it is not a custom value depending on your board house, your design software, or anything of that sort. They will all point to this formula, so I simply prefer to skip the middle man and calculate the required trace widths myself from the start.