3
\$\begingroup\$

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.

enter image description here

Thank you.

\$\endgroup\$
3
  • \$\begingroup\$ electronics.stackexchange.com/questions/255981/… for ideas \$\endgroup\$ Jul 19, 2017 at 14:20
  • \$\begingroup\$ My two cents: if the stackup allows it, use multiple layers in parallel. Inner traces heat up more, but you benefit from decreased series resistance. \$\endgroup\$ Jul 19, 2017 at 14:56
  • \$\begingroup\$ Instead of a track you could try a "plane-pool" (a small plane for that particular connection) to make the area as big as possible (within reason). \$\endgroup\$
    – R.Joshi
    Jul 19, 2017 at 15:01

3 Answers 3

3
\$\begingroup\$

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.

\$\endgroup\$
2
  • \$\begingroup\$ I can't connect two tracks on Altium I don't know why, they are just moving around each other but can't connect. And how do you fill your polygon? Mine look like a polygon line that can't connect to any tracks. Thank you ! \$\endgroup\$
    – Ultra67
    Jul 21, 2017 at 7:32
  • \$\begingroup\$ The polygon initially doesn't have a net name. You need to assign the net name for it to attach to your 10A net. You can also consider removing the solder mask from the 10A line and manually filling it up with solder if it heats up too much during testing or consider a thicker PCB \$\endgroup\$
    – Sachin
    Jul 21, 2017 at 8:34
2
\$\begingroup\$

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...

\$\endgroup\$
2
  • \$\begingroup\$ Thanks a lot :) Are you talking about Polygon Pour ? \$\endgroup\$
    – Ultra67
    Jul 19, 2017 at 14:46
  • \$\begingroup\$ Yes, polygon pours. Altium handles these quite well. \$\endgroup\$
    – bobflux
    Jul 19, 2017 at 19:00
0
\$\begingroup\$

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)

enter image description here

\$\endgroup\$
1
  • \$\begingroup\$ In Altium, a shape like this on a positive layer is called a polygon or a region. The term plane or split plane is used to refer to shapes on a negative layer (which could indeed be part of a solution to OP's problem, but wouldn't look like what you showed in your picture). \$\endgroup\$
    – The Photon
    Jul 19, 2017 at 16:07

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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