Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. It only takes a minute to sign up.
Sign up to join this community
I'm designing a PCB in Altium and I need to trace tracks that can support 20A. I used a PCB Track Width Calculator and I need a width of 10mm for my tracks. The problem is, how do you link the pads of component to such a large trace? Can I make a small trace at the end of the large one? Do you have a solution for this problem? Here is a screenshot so you can see the size.
Thank you.
The rules for track width are for long tracks, and they are meant to achieve a certain limit on the temperature rise (typically 10 C) of the track due to self-heating.
A small length of short track connected to a wide track will heat up more, but it will also (because it's short) get the benefit of thermal transfer to the wide track, so it won't heat up as much as a long narrow track.
Calculating the "exact" (nothing is really exact in thermal analysis) temperature rise of the short track (or the long track, for that matter) is a job for a heat-transfer simulation.
Can I make a small trace at the end of the large one? Do you have a solution for this problem?
Yes. Either extend the wide trace with a narrow trace, or make a polygon around the pad you're connecting to that extends to somewhere you can attach the wide trace. Make this section as short as possible. You could also widen the wide trace near where it connects to the narrow trace (or use a polygon) to give it more surface area and allow it to provide greater heat-sinking to the narrow trace.
If you only have a few such traces, use polygons instead. It is much easier to adjust the shape according to your needs.
Since PCB traces current carrying capacity is determined by heating and temperature limits, using polygon fills spreads the heat and cools the trace better if you can expand the fill into some unused space. Beware though, large copper areas have extra capacitance, so if you have a high dv/dt node, like the switching node of a DC-DC converter, make sure to keep it short.
You can also use thicker copper. Even if you use standard thickness, make sure you know what thickness your PCB fab uses...
In addition to what others have said. If your tracks is hitting the the adjacent pins, you could try placing a "plane" instead. You could make the plane larger for better heat dissipation.
See example below. (Imagine the two holes are actually connected)
