I have seen several designs where there is extra spacing between some traces and the ground plane. For example, see the traces between the points A and B or C and D in the following picture (this is a Raspberry Pi 2, but I have seen it on other boards too):

enter image description here

What is the purpose of this extra spacing?

My guesses:

  1. Reducing ground plane noise.
  2. Controlling trace impedance (for high speed signals).
  3. Perhaps for some EMC reasons.
  • \$\begingroup\$ My bet is on #2. But I can't read the designer's mind. \$\endgroup\$
    – The Photon
    Dec 1, 2015 at 17:24
  • \$\begingroup\$ Or (4) reduce capacitive loading on traces A-B. Or (5) to eliminate tracking between high voltage signals and ground. (Highly unlikely on the R-Pi!) \$\endgroup\$
    – user16324
    Dec 1, 2015 at 17:28
  • \$\begingroup\$ It is probably an impedance thing. As the outer layer GND flood moves closer to the trace, the trace impedance will go down. This could be compensated for by making the trace more narrow. But maybe the trace is already at the minimum for the fab process. \$\endgroup\$
    – user57037
    Dec 1, 2015 at 18:44
  • \$\begingroup\$ Not necessarily in this case but you sometimes see this for isolation requirements. Sometimes you need to guarantee several KV of isolation for a bus signal (Several CAN protocol standards have this in their physical link requirements). Say two traces going from the isolation circuit to the physical connector need spacing like that to pass hipot. For High voltage traces you also see this due to creepage \$\endgroup\$
    – crasic
    Dec 1, 2015 at 20:07

2 Answers 2


I would put money on #2.

That is clearly a differential pair between A and B, referenced, no doubt, to a plane on the next layer. Between C and D appears to be a single ended signal.

That is a microstrip configuration, and if the surface plane gets too close it would change it to a coplanar waveguide with ground, which apart from changing track and gap for a given impedance, also induces (if you are not careful) propagation mode differences.

No hyperlinks - on mobile. Maybe tomorrow.

Edit: updated with simple picture.

Two different transmission lines

Looking at the top picture, we have the classic differential microstrip configuration. The required clearance is beyond the scope of this post, but we do not want to couple the fields to anything other than the pair and the reference below.

If we allow the same reference to approach from the sides, we get a coplanar waveguide with ground, a very different beast indeed. I am not going to post the equations, but they are easily available with a search.


For most designs, the ground is shared with peripherals and (expected to) has a lot of noise. If the circuit has some low voltage high freq components and lines , it is a good practice to keep away those lines from noisy ground planes.


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.