0
\$\begingroup\$

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

\$\endgroup\$
  • \$\begingroup\$ I am not sure about Proteus, but there are numerous online calculators. PS 60 amp track will be super wide! \$\endgroup\$ – Tyler Mar 3 at 15:01
  • \$\begingroup\$ For traces on 2 oz copper board at 10 degree temperature rise from 25 degrees ambient, you'll want 111mm wide internal traces and 42.6 mm wide external traces. For 4 oz copper board, half that. Perhaps consider using wires instead. \$\endgroup\$ – K H Mar 4 at 4:29
2
\$\begingroup\$

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.

\$\endgroup\$
1
\$\begingroup\$

If you do this, you will melt the track

schematic

simulate this circuit – Schematic created using CircuitLab

\$\endgroup\$
0
\$\begingroup\$

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.

\$\endgroup\$
  • \$\begingroup\$ That formula does not depend on trace length, but a long trace will get hotter than a very short one. \$\endgroup\$ – Uwe Mar 4 at 20:44
  • \$\begingroup\$ @Uwe Source? You may be right, but the formula used above is what is called out in what can be considered THE bible of PCB design. \$\endgroup\$ – DerStrom8 Mar 4 at 22:12
  • \$\begingroup\$ If it is a good bible of PCB design, there should be some sentences about the conditions when this formula is applicable. A large PCB filled with a high current coil with many windings would get much hotter than calculated. \$\endgroup\$ – Uwe Mar 5 at 11:04

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.