I'm designing a PCB for a 10A relay and am trying to determine what the trace width should be.

According to this trace width calculator, the biggest factors in the width are copper thickness, maximum current, and temperature rise. I would like to use 1oz for the copper thickness since that makes the PCB cheaper, so that leaves temperature rise as the most desirable variable to change.

Using the above calculator with these settings:

Current: 10 amps
Thickness: 1 oz/ft^2
Temperature Rise: 10 C
Trace Length: 1 in

The calculated trace width is 283 mils, which is too wide.

If I change the Temperature Rise to 100 C, the calculated trace width is 70 mils, which isn't bad at all. However, I don't know what kind of temperature rise is acceptable. How do I determine this?

  • 4
    \$\begingroup\$ 70 mil may not be bad, but a trace delaminating itself from the substrate is... \$\endgroup\$
    – Matt Young
    Commented May 19, 2014 at 20:03
  • \$\begingroup\$ related, but not duplicate: How to carry high current on PCB? \$\endgroup\$ Commented May 19, 2014 at 22:01

3 Answers 3


Temperature rise is something you have to consider, but usually the resistance and the resulting voltage drop at full current have been the limiting factors when I've gone through this. That said, 100°C is a large temperature rise. That's not enough to be a problem for a copper trace on a FR4 board by itself, but that's going to affect the apparent ambient temperature for nearby components.

If you have that much temperature rise, you're dissipating significant power in the trace, which means power loss in your system. Again, the first concern should be how much voltage drop you can tolerate. Once you get that to acceptable levels, the temperature rise is usually low enough.

Also consider that 2 oz copper and more is widely available. The extra cost of specifying 2 oz copper for outer layers may be less than making the board larger or dealing with the heat or voltage drop. 2 oz on outer layers doesn't usually add that much cost. If you stitch together a trace on both outer layers, you have 4x the copper cross section than for a single trace of 1 oz thickness. If it's only one or two traces in a otherwise low current design, you can leave the soldermask off the trace and have a copper wire soldered over the trace. There are actually bus bars meant for this. However, consider the manufacturing cost. 2 oz copper may start to look like the cheap option when you consider the total cost of alternatives.

Again, look at all the options and all the criteria for deciding on trace width. Don't just focus on temperature rise, or assume that thicker copper is more expensive once the whole system is considered.

  • \$\begingroup\$ Stitching together two traces is a great idea! How do you get "4x the copper cross section," though? It seems like it would be double the cross section. \$\endgroup\$
    – Nate
    Commented May 19, 2014 at 20:48
  • 2
    \$\begingroup\$ @Nate: For 4x I was referring to using 2 oz copper and stitching top and bottom together. \$\endgroup\$ Commented May 19, 2014 at 20:59
  • \$\begingroup\$ If I do two traces, one on the top layer and one on the bottom, is there a reason to use vias to connect them? I've been thinking about it and it seems like this would actually reduce the cross-sectional area of the trace. With vias, this is what it looks like: imagizer.imageshack.us/a/img838/5508/n1el.png \$\endgroup\$
    – Nate
    Commented May 20, 2014 at 15:48
  • \$\begingroup\$ @Nate: You need to connect them at the ends at least. Yes, vias in the middle of the trace eat into the conductive width somewhat. If the trace is carrying only low frequencies, then identical traces on opposite sides of the board connected only at their ends is good enough. Note that you might need several vias for the connections at each end. \$\endgroup\$ Commented May 20, 2014 at 16:01

The number you need is called "MOT" (maximum operating temperature) for the laminate you have in mind. You also need to know what the internal temperature will be in your product (including the heat the relay connections add). For FR-4 to maintain electrical properties, that might be 130°C (a bit higher for mechanical properties). If the maximum temperature in the vicinity of your PCB will not exceed 60°C you could conceivably allow for 70°C rise. For FR-2 it might be 105°C, so the limit might be 35°C rise.

More normal practice is to allow for 20-30°C to keep the PCB from getting all discolored and weak over time and there might be issues with component life if you add too much heat. It's conceivable UL approvals might be complicated with internal temperatures exceeding 105°C.

There are some very nice higher temperature laminates with Tg = 170°C available, and commensurately higher MOT, but it's cheaper to use 2oz copper.

Other options are to pull back the solder mask and parallel the conductors with solder (assuming wave soldering), or to solder a jumper wire in place of, or in parallel to, the conductor. If you can keep the conductors short in length, most of the heat will get sunk out of the pins. Look at the design of any PC power supply for ideas, just about every penny has been pinched in their design.


100C is a lot of heat and power wasted. As a customer, I'd not accept a product that was so hot in its wires (traces).

I'd say 50-75C would be MAX acceptable amount for me. (But I still would not be happy). Do you have other options? As Olin stated, if you are creating heat you have resistance and are wasting too much power doing nothing useful.

  • 13
    \$\begingroup\$ As a customer, how would know how hot a trace on a board inside a sealed unit actually gets? You might notice the overall unit getting warm, but that is nothing unusual. This is not a level of detail about which a customer should be making judgemnts. \$\endgroup\$ Commented May 19, 2014 at 20:15

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.