25
\$\begingroup\$

I need a trace on my PCB to carry up to 2.5 amps (average) current, with 5-6 amp spikes (it's going to a switch mode power supply.) How wide should the traces be? I've got a trade off between reliability and size, as the product is space constrained. Any tips would be appreciated.

\$\endgroup\$
1
  • 1
    \$\begingroup\$ Copper thickness/weight? \$\endgroup\$
    – tyblu
    Dec 30, 2010 at 4:02

4 Answers 4

24
\$\begingroup\$

After doing a quick google of "PCB Current Calculator", I found a PCB Current Calculator based on IPC-2152. It bases the width of the track on how much of a temperature rise the trace is allowed to have. It's nice in that it shows how much power you waste through your trace. I would design for your worst-case RMS current, since it's going to be a periodic signal.

If you use 2 oz/ft2 copper instead of the standard 1 oz/ft2 copper, you won't need as wide of a trace to achieve the same resistance. For example, allowing for a 10 oC rise, you can get away with these numbers at 3 A with no copper plane nearby:

  • 177 mil (4.50 mm) on 1/2 oz/ft2 copper
  • 89 mil (2.26 mm) on 1 oz/ft2 (35µm) copper
  • 47 mil (1.19 mm) on 2 oz/ft2 (70µm) copper

Note: IPC-2221 (The standard used in the original answer) uses old measured values for its design charts, and these charts are implemented in many calculators. As best as I can tell, this data was claimed to be 50 years old, which makes IPC-ML-910 (1968) a possible source. As @AlcubierreDrive pointed out, a new standard, IPC-2152, contains new measured data, and presumably is more accurate. More importantly, a comparison of IPC-2221 values gives the following result for trace widths: IPC-2221 (internal) > IPC-2152 > IPC-2221 (external). Actual numbers for the example above (1oz copper) are

IPC-2152:             89 mil 
IPC-2221 (internal): 143 mil (+60%)
IPC-2221 (external):  55 mil (-38%)

Also note that the original numbers in this answer were based on the IPC-2221 internal calculations, which will provide a conservative estimate for all values.

\$\endgroup\$
3
  • \$\begingroup\$ This calculator is incorrect! It is based on IPC-2221, which is incorrect and has been superseded by IPC-2152. Using IPC-2221 will result in undersizing your outer layer traces by a factor of 2!! For historical background, google IPC-2152, or see the section titled "The Historical Chart" in this document: frontdoor.biz/PCBportal/HowTo2152.pdf \$\endgroup\$ Jan 22, 2016 at 6:17
  • \$\begingroup\$ @AlcubierreDrive Interestingly, this was written around the time IPC-2152 came out. I'll update my answer accordingly. Do you know if the more recent IPC-2221B (2013) addresses this issue? \$\endgroup\$
    – W5VO
    Jan 22, 2016 at 16:23
  • \$\begingroup\$ NinjaCalc includes a track current calculator based on the IPC-2152 standard. Disclaimer: I am the author. \$\endgroup\$
    – gbmhunter
    Mar 30, 2016 at 3:19
21
\$\begingroup\$

Common practice for high-current devices is to solder thick copper wire on top of your 2-3mm trace. 1mm^2 wire can handle 10A easily.

\$\endgroup\$
3
  • 3
    \$\begingroup\$ Came here to say that \$\endgroup\$
    – Linker3000
    Dec 30, 2010 at 21:11
  • 1
    \$\begingroup\$ Wrong button ) Could you please edit anything in your answer? :-) \$\endgroup\$ Dec 30, 2010 at 22:00
  • 1
    \$\begingroup\$ NOP edit complete! \$\endgroup\$
    – tyblu
    Dec 31, 2010 at 0:44
10
\$\begingroup\$

I remember having seen this nomogram in another answer:

enter image description here

Select 2.5A on the vertical axis of the top graph. Move to the line indicating the allowed temperature rise. Move downward to the PCB's copper thickness in the bottom graph. This intersection gives you the required width on the vertical axis.

\$\endgroup\$
2
2
\$\begingroup\$

Another option would be to use PCB Busbar soldered into the PCB - they would also add some nice rigidity to your PCB should it need it

\$\endgroup\$
4
  • \$\begingroup\$ A 1.6mm FR4 PCB is many times stiffer than a Busbar! \$\endgroup\$
    – stevenvh
    Apr 13, 2012 at 7:45
  • 1
    \$\begingroup\$ @stevenvh - What? No they're not. Plus, a buss-bar is generally perpendicular to a PCB, so it is far more rigid. In fact, they're actually sold specifically as PCB stiffeners. \$\endgroup\$ Apr 13, 2012 at 9:02
  • \$\begingroup\$ @Fake - Yes, I've seen them sold as stiffeners, but I'm not sure that's a good idea: you want as little force as possible exerted on soldering connections. \$\endgroup\$
    – stevenvh
    Apr 13, 2012 at 9:08
  • \$\begingroup\$ @Fake - just asked this question about it. \$\endgroup\$
    – stevenvh
    Apr 13, 2012 at 9:22

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.