0

enter image description hereCurrently working on a 4 layer pcb-card where I need to trace for 50 amps, any ideas how I can design it?

Any tips would be appreciated. Thanks!

razz
  • 1
  • 1
  • try to use as wide traces as possible it's usually better than using more layers, due to less power density hence less local heating – user103776 Feb 07 '19 at 10:18
  • Is the 50 amps continues or not? – user103776 Feb 07 '19 at 10:18
  • Yes its continues. According to online trace width calculator i would need about 50mm width which is huge – razz Feb 07 '19 at 10:22
  • 5
    Have you thought about not directly carrying this current on a PCB? Sometimes it's better to use an additional, external piece of copper – Tom L. Feb 07 '19 at 10:30
  • Do you mean a high-current PCB bus for example? – razz Feb 07 '19 at 10:34
  • You should think about special PCBs with different copper plating, 35 µm for standard low current signals and for instance 350 µm for the traces loaded with 50 A. In my former job we produced some of such PCBs. There are some PCB manufacturers offering those. But think about soldering, you might need to use very powerful soldering guns and even more than one. One large gun to preheat the trace and one medium size for soldering at the parts pins. – Uwe Feb 07 '19 at 11:24
  • See this other questions about high current PCBs: [(1)](https://electronics.stackexchange.com/questions/8418/sizing-a-trace-on-a-pcb-to-carry-2-5-amps?rq=1), [(2)](https://electronics.stackexchange.com/questions/135714/pcb-trace-width-calculation?rq=1), [(3)](https://electronics.stackexchange.com/questions/414480/increasing-pcb-trace-current-capability-by-duplicating-on-other-layer?rq=1). – Uwe Feb 07 '19 at 14:58

1 Answers1

4

Some work was done by years ago on this and the relevant standard is IPC2221

The basic concepts are as follows the thicker the copper the better, the wider the copper the better. Putting high current tracks on external layers is better as heat can escape easier.

That said for really high currents supplementing the tracks with external conductors helps. I have left an area free of solder resist for this and soldered of copper braid (e.g. solder-wick) in the past for home or low volume products. For higher volumes I have used copper bus-bars.

That said the maths: Note 1 mil = 0.001 inch

Let \$I\$ be the track current \$[\text{amp}]\$
Let \$A\$ be the cross-sectional area if the track \$[\text{mil}^2]\$
Let \$T\$ be the allowable track temperature rise \$[\text{ }^oC]\$
Let \$W\$ be the required track width \$[\text{mil}]\$
Let \$M\$ be the mass of copper on the PCB \$ [\text{oz} / \text{ft}^2]\$
Let \$k\$, \$b\$ and \$c\$ be constants defined by the IPC standard.

\$ A = \dfrac{I}{k \cdot T^b}^{1/c}\$

Then, the Width is calculated:

\$ W = \dfrac{A}{M \cdot 1.378} \$

where k, b, and c are constants resulting from curve fitting to the IPC-2221 curves

For IPC-2221 internal layers, \$k = 0.024\$, \$b = 0.44\$, \$c = 0.725\$

For IPC-2221 external layers, \$k = 0.048\$, \$b = 0.44\$, \$c = 0.725\$

If you do not feel like doing the the maths yourself there are many online tools

Assuming 2oz copper, 10C rise I would go with some kind of bus-bar as track is of the order of 1.3 inch wide.

Bunny Girl43
  • 3
  • 3
Warren Hill
  • 4,780
  • 20
  • 32
  • Thanks for answer, I understand the calculations but my problem still exist. Lets say I use 2 oz thickness and 50 amps at 60C ambient Temperature with 20 temp rise.Trace width will then be about 22mm on external layer(top layer) which is still huge. I need to solve this somehow – razz Feb 07 '19 at 11:41
  • You can get 4oz copper from many PCB vendors, solder links (or copper braid) in parallel with the track or use both sides of the board. – Warren Hill Feb 07 '19 at 11:48
  • Can you give me any example of a bus-bar that will fit perfect for my problem? – razz Feb 07 '19 at 11:57
  • 4
    @LinusJönsson Recommendations for specific products are off-topic for this site. This answer has given what you asked, which was how to size the trace. – Elliot Alderson Feb 07 '19 at 12:39
  • 3
    @LinusJönsson if 2 oz or 70 µm thickness and 22 mm track width is not what you like, you may use 140 µm and 12 mm or 210 µm and 8 mm. But you can't get a solution with 35 µm and less than 5 mm track width made with unobtainium superconductive plating. – Uwe Feb 07 '19 at 14:38
  • [PCB Trace Width Calculator](https://www.7pcb.com/trace-width-calculator.php). – StainlessSteelRat Feb 07 '19 at 16:12
  • Old question and old answer, but I have in the past carried 100 amps by using parallel traces on both sides of the board (stitched together with many vias on both ends) using 6oz copper (yeah, some manufacturers offer that! it starts to get expensive though). This was on a very small PCB that had to go in line with a larger cable, in a system used for research purposes (meaning not under continuous load). Running two parallel traces on both layers will require some creative layout decisions in any complex 2-layer boards. – Hearth Jun 16 '20 at 13:57
  • NOTE: IPC-2221 and associated calculators are not recomended –  Jun 16 '20 at 14:18
  • @JonRB IPC-2221 is the best data I have. What should we use instead? – Warren Hill Jun 17 '20 at 09:35
  • @WarrenHill IPC-2152 superceeds IPC-2221 with regards to current handling –  Jun 17 '20 at 10:31