I'm designing a PCB board (low current, low frequency) mainly consisting of low frequency SPI and analog sensors.

Are wider traces better or does it not matter?

And which is better, consistent trace width or varying (to its maximum at its location)?

Also, is wider spacing between two traces better or does it not matter?

  • 1
    \$\begingroup\$ What current and frequency are you thinking when you say "low". \$\endgroup\$ – whatsisname Aug 28 '14 at 15:28

On the Internet there may be 'specification wars' between PCB manufacturers. Track, space, drill holes and vias are a differentiators. Some companies might be conservative and quote figures which are well within capability, and others may be at the edge of their capability.

Laen of OSHpark has run some tests on several services offered over the Internet, designed to reveal manufacturing defects. The test PCB's used the finest tolerances offered, and the boards failed. IIRC some percentage of the boards were supposed to have been electrically tested, and were passed, but you should double check that with Laen.

Advice I was given by some experienced designers is: avoid using the smallest track, space, annular ring, holes and vias offered by your PCB manufacturer, at least until you get comfortable with their capability. The general advice was use an extra couple of mil (thou) above the PCB manufacturer's limits on track, space and annular ring, and one or two drill sizes larger on vias and drill holes to increase the likelihood of it being made correctly every time. Leave an extra margin around board dimensions and routed holes because defects which short copper surfaces are awful to debug.

Other advice included:

  • leave as much copper as you can on the PCB; you paid for it. More importantly, the waste chemical etchant is a material which requires careful handling as a pollutant, so try to minimise the amount of copper removed, and so minimise waste.
  • make annular rings around holes slightly wider, and tracks slightly wider if the board is to be soldered by inexperienced people (e.g. beginners). Beginners make more mistakes than production trained staff. For example they often put parts in the wrong holes. When they remove the part, they are likely to overheat a small pad, and pull it off too, ruining the PCB.

Edit: I defer to Andy aka, and other experienced community members on PCB design.

The advice I have is try to ensure 'islands' are connected to a relatively continuous ground plane using vias, and not disconnected. This is especially true around low analogue voltages and higher frequencies, where 20MHz is definitely 'high frequency'; I do MCU boards, where most high frequencies are internal to the MCU or communication interfaces e.g. USB where I take special care. Disconnected areas which are not in those contexts I might leave, especially if I am worried about heat dissipation, though I rarely have disconnected areas.

However, I do get experienced people to give my PCBs a review. You might consider asking for a review here. I know I feel more confident after someone I respect has a look at my PCBs, not least because they might question an assumption which is no longer valid.


Are wider traces better or doesn't matter?

When it comes to 0V or signal 0V, a ground plane is always better hence the width is as wide as the board. Yes, in this example wider traces are better.

On other tracks (such as SPI) you don't want wide tracks because the capacitance to ground will be high and more power supply current will be needed and potentially this will generate interference into your analogue sections. You mention you use low speed SPI but the clock edges are still fast and can cause problems.


Andy and gbulmer are great answers. Adding this as a long comment:

I keep mine consistent because I'm a neat freak. Looking at my display board, I have 0.3mm SPI trace (10MHz) because the level shifter pads were 0.3mm. They then run about 2mm apart (miles and miles!) because it was hand etched and soldered and I had the space.

On another board, the traces are smaller and much closer together, again for SPI. 0.25mm traces and 0.3mm apart at their closest point. This was because the board was done in a PCB house so I have a solder mask and it's not me personally having to do it. I also happened to read Laen's article and don't want to go to 0.2mm when I don't have any reason to do so. They all say 0.15 is fine but the article I read says shows that not to be the case. (0.2mm is 8 thou by the way).

In your case your analog sensors may require more careful layout and track widths and spacing may be part of that.

Having said all that, I built DACs and amps in the audio range by drilling PCB board and joining up the holes with a marker. Worked just fine.


If this is to be manufactured by a PCB house, you can choose track/space width as you like, as long as you stay above some minimal value. For manufacturing, it is good to have high copper/non-copper area ratio, and to have non-copper with uniform width and uniform distribution across the board.

That is especially true for inner layers, in order to be laminated properly.

In all cases, thin tracks with large blank area around (10-20 times the width) should be avoided because it causes problems with electroplating.


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.