Is there a standard for the sizes of PCB traces?

That is are some 25 mil and others 10 mil or is can you choose your own?

I plan to run 400mA through some thicker traces, but less than 30mA for all other traces. About what size would I need?

  • 1
    \$\begingroup\$ You don't arbitrarily select trace widths. Whether they are power traces or controlled impedance, you calculate them using a tool like this. \$\endgroup\$
    – Matt Young
    Commented Feb 19, 2015 at 20:22

6 Answers 6


Your traces can be any size you want as long as you stay within the minimum feature size and spacing that your PCB fab supports for your particular price point.

These will cover basic needs, the trace width one is a best fit calculation to the chart Engen posted:

PCB Trace Width Calculator

PCB Via Calculator

Neither of those cover controlled impedance calculations, if you need those look elsewhere.

  • \$\begingroup\$ go with these - IPC based :) \$\endgroup\$ Commented Oct 22, 2010 at 22:24
  • \$\begingroup\$ For fab houses its worth mentioning that many of them have drc rules files for common CADs on their websites \$\endgroup\$
    – jaskij
    Commented Oct 26, 2017 at 6:46

You can use this nomograph to determine the width according with current:

alt text

Using the nomograph

  1. Locate the width of the conductor on the left side of the bottom chart.

  2. Move right horizontally, until you intersect the line of the appropriate conductor thickness. Move down vertically to the bottom of the chart to determine the cross-sectional area of the conductor.

  3. Move up vertically, until you intersect the line of the appropriate allowable temperature rise. This is the increase in temperature of the current-carrying conductor. Conductor temperature should not exceed 105°C. For example, if the ambient temperature might reach 80°C, the temperature rise above ambient of the conductor should be less than 25°C (105°C - 80°C). In this case use the 20°C curve.

  4. Move left horizontally, to the left side if the chart to determine the maximum allowable current.

Reverse the order of these steps to calculate required conductor width for a given current.

More informations at this site: http://www.minco.com/products/flex.aspx?id=1124

This graph is from IPC, but I cannot find it there.

  • \$\begingroup\$ Nice graph, easy enough to figure out, but you should probably explain how the examples work for completeness. \$\endgroup\$
    – Nick T
    Commented Oct 21, 2010 at 19:18
  • 3
    \$\begingroup\$ Dead link at minco.com \$\endgroup\$
    – JYelton
    Commented Dec 11, 2012 at 16:35
  • \$\begingroup\$ The graph mentioned above can be found in IPC-2152 . \$\endgroup\$
    – user45504
    Commented Jun 12, 2014 at 18:54
  • 1
    \$\begingroup\$ NB: This is fairly different for higher-frequency! \$\endgroup\$
    – meawoppl
    Commented Jan 19, 2016 at 18:33

PCB makers sometimes produce swag that has this kind of thing on it, because it's common to want to get a feel for PCB traces that are out of one's comfort zone.

Here's a photo of one such trade-show give-away, with a dime for scale (as well as the ruler scales). Trace/space widths are in inches.

enter image description here

  • \$\begingroup\$ These also exist for SMT pads, through hole vias, and other things. Here is Dave Jones' version: pbs.twimg.com/media/BRcA7XjCQAEhO71.jpg \$\endgroup\$
    – Greg d'Eon
    Commented Feb 19, 2015 at 21:32
  • \$\begingroup\$ Shouldn't the spaces between these traces be the same as the widths of the tracks? The traces look much wider that the spaces between them. \$\endgroup\$
    – Chupo_cro
    Commented Feb 5, 2023 at 19:24
  • \$\begingroup\$ @Chupo_cro Looks like they only cared about the trace widths. You're supposed to imagine the space as being the same width as the trace. Wow, 8 years ago. \$\endgroup\$ Commented Feb 5, 2023 at 20:25
  • 1
    \$\begingroup\$ I saw it's an old answer and thought you won't notice the comment but I posted it anyway and you answered in just an hour :-) \$\endgroup\$
    – Chupo_cro
    Commented Feb 6, 2023 at 4:16

If you are making your own boards, then you want traces as large as you can get by with -- perhaps 15 mils (0.015") for signal traces, and 30 mils for power. Note: with traces that large, you will typically have to narrow the traces down a bit before connecting to IC's pins with fine pitch pads.

If you are having a board house make your boards, then you can use smaller traces for signal traces, say 8 or 10 mils if you have room. Most PCB fabricators that do fast and inexpensive boards have a minimum trace width of 5 or 6 mils, but if you can go a little larger, the better. (For military and other high-tech boards, they can now go as small as 2.5 mils or even smaller.)

For power traces, then I agree with other posts that you should use a trace width calculator like this one. I generally end up using 20 or 25 mil traces for power rails. But the calculator will give you ridiculously small trace widths for signal traces that might carry only a few milliamps.

Note that in addition to trace widths, you will also want to space your traces apart, typically by the same distance as the trace width.

You can enter these rules such as minimum trace widths and minimum distances between traces, between traces and vias etc. into Design Rule Checks in programs like Eagle layout software, and when you run a DRC the program will point out violations.


IPC standard 2221 "Generic Standard on Printed Board Design" (pdf, IPC web-site paid) (page 41) provides the following relationships between current carrying capacity and copper trace width:

enter image description here Figure 1: Cross section area to current. External layer.

Notes for the figure (also applicable for the Figure 2):
1) Temperature stands for temperature of the trace relative to ambient. That is, if, for instance, ambient temperature is 80C, 20C stands for 100C temperature of the trace.
2) The curves include a nominal 10% derating (on a current basis) to allow for normal variations in etching techniques, copper thickness, conductor width estimates and cross-sectional area.
3) Additional derating of 15% (current-wise) is suggested under the following conditions:
. a) for panel thickness of 0.8 mm or less,
. b) for conductor thickness of 108 um or thicker.

enter image description here Figure 2: Cross section area to current. Internal layer.

enter image description here Figure 3: Cross section area to trace width.

What is 1 oz copper?
The measure for the copper thickness on a printed circuit board. It's the resulting thickness (height) when 1 oz of copper is pressed flat and spread evenly over a one square foot area. It corresponds to copper thickness of 1.37 mils (34.79 um).

Explaining the relationship between cross section area and trace width (Figure 3)
1) Every curve corresponds to a particular copper thickness (trace height).
2) Area (horizontal axis) is calculated as product of trace width and thickness.

Below is a Matlab script with a calculation example. It shows that for 1 oz copper trace with the area of 9 sq. mils, trace width is 6.6 mils:

area=9*(1E-3)^2;%square inches
width=(area/thickness)*(1/1E-3) %in mils
% result is 6.6 mils

Example of usage of the charts
1) Internal layer, current 400 mA, copper thickness 1 oz, ambient temperature 80C, trace temperature 100C. What is the appropriate trace width?
2) Look at Figure 2 (internal layer). Find the curve 20C (100C-80C). Find the point (9 sq. mils, 400 mA).
3) Look at Figure 3. Find the curve 1 oz. Find the point (9 sq. mils, 0.07 inches).

The answer is about 7 mils (0.007 inches).

  • 1
    \$\begingroup\$ What do you include as your safety factor? For example if I need to pass 1A through my traces I always add 25% extra (Calculate for 1.25A) \$\endgroup\$
    – user103993
    Commented Aug 15, 2016 at 13:47
  • \$\begingroup\$ @Hayman Thanks for the comment. According to the standard (page 41, notes for the figure) 10% safety cushion is already included in the charts. Additional 15% should be added under some circumstances: pls, see the updated answer (Notes 2 and 3 for the Figure 1). \$\endgroup\$ Commented Aug 15, 2016 at 14:03

The easiest way to do this is to use a PCB design program and draw traces of various widths. Then print your copper layer onto paper in "true size". Exactly as if you were going to make your circuit board at home with a toner-transfer method.

What prints out on the paper should be exactly what you would see if you actually ordered the PCB.

moderator note: This answer have arrived to this thread as a result of a merge.


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