Track width advice for 12v&5v rail 100ma


I wondering if someone could give me advice in relation to track width?

  1. 12v 100ma
  2. 5v 100ma


There is a trace-width calculator in kicad, it’s easy to use.

If you’re not constrained by board size, density of parts or voltage drop along traces, use something convenient to you, maybe 0.3mm (12mil) or larger.


You forgot to mention the “weight” (i.e., thickness) of the copper, the allowable thermal rise, acceptable voltage drop for a given length of trace, and whether you are constrained by any regulatory or safety standards. Oh, and whether or not this trace needs to pass between the pads of, say, an 0805 resistor or some other part. And how rugged the trace needs to be - will it still be adhered to the board after several cycles of rework, repair, etc with hand-soldering methods.

Like many (most?) technical questions, the easy answer is often not best and the best answer is often not easy. Fortunately we live at a time when many valid, authoritative, references are available on-line. The good ones will tell you what criteria they use to determine their suggestions. You don’t have to put yourself at the mercy of the habits, inertia, and prejudice of us grey-haired old guys.

But since you ask . . . many designs successfully push an amp of current through 1-ounce traces of 10 to 12 mil widths.


1 Like

Thanks for the illuminating replies. I should have explained my question better.

I’m taking power via a 25pin Dsub connector. The 5v is right next to the 12v pin. I can either have both (5v&12v) running in parallel, or loop the 12v rail around one of the mounting holes. I’ve already prototyped,(cnc copper milling/no solder mask) and the 12v rail just ‘blew’. (0.30mm).

I’m still on a huge learning curve with pcb design! But glad I stuck it out with KiCad :wink:

I guess if your 0.3mm track burnt, then it was carrying much more than 100mA (short somewhere?), unless your copper weight < 1 oz?

But there are many other factors to consider of course.

I was thinking of the possibility of a short! (I did find soldering on bare copper, rather haphazard). But couldn’t see anything. I’ve checked the data and both are 100mA.

If knowledgeable folk think 0.3mm is good for 12v 100mA? I’ll stick with that.

Thanks for all the advice.

What happens if there is a fault is a key issue. In some situations blowing the track by shorting would be an approval fail Traces should not fail before fuses.
You may also want to have additional clearance around the 12V trace to reduce the possibility of a short to 5V circuitry, a potentially disastrous fault

You really need to determine the fundamental cause of the track failure before you give any more attention to the question of trace width.

  • If it was a design error - either on the schematic, or in your layout - it needs to be corrected at that point. Then, produce a revised layout.

(The “dot convention” on schematics is a common source of errors. The concept is simple: You place a “dot” (filled circle) where there is electrical continuity between wires that touch each other, and no dot where wires cross in the drawing but have no electrical connection. One problem is that graphic engines make the dots too small to be obvious, so a casual inspection indicates no connection but the software generates a netlist showing connections. Or, when drafting the connections in a schematic, the software assumes wires crossing each other are connected when the designer had no such intent.

To reduce the problem, many shops have a “house rule” that connection wires shown as crossing each other should NEVER have electrical connection; and wires intended to have electrical connection are ALWAYS drawn as a “tee”.)

  • If it was a fabrication error you need to meet with the machinist or etching operator and determine the error’s source. It will help if an extra copy or two of the board was fabricated. (An old machinist taught me that the first copy of ANY part is made to get an understanding of the part and its fabrication process, the second copy is for practice, and the third copy is a prototype.) Should the design rules for the board layout be modified (i.e., spacings increased) because of the capabilities and tolerances of the fabrication method? Did the Gerber or CNC file correctly render the layout in the vicinity of the fault? (And if not, are there other faults present.) If an optical photo process was used, did dust or exposure times create the fault?

  • Assembly errors are often the most difficult to pin down after the fact because they may be present on only a few units in a batch, and in your case the error may have been destroyed along with the trace. Was the board carefully inspected by an additional set of eyes after assembly? Is there evidence of solder bridges at ANY point on the board? Are the assumptions for track widths, clearances, and pad sizes compatible with the methods, tools, and abilities of individuals involved in the assembly process? Was a component damaged during assembly?


1 Like

what data do you refer to about the 100mA.
Static? Rush-In currents, capacitors, coils, …