17

I have been reading up on the EMI issues in Electromagnetic Compatibility Engineering by Henry Ott. (wonderful book btw).

One of the topics "PCB Layout and Stackup" (aka Ch 16) there is section about ground fill (16.3.6). Basically what it states, that to minimize the "return current path" filling the areas between connector pads with ground fill should be done. Quite understandable, however in the same section at the end it states "Although often used with analog circuits on double-sided boards, copper fill is not recommended for high-speed digital circuits, because it can cause impedance discontinuities, which can lead to possible functional problems.". That last part confused me a bit, since I would expect that for high frequency signals (that try and follow the signal trace) a longer path would be decremental. Can anyone explain why this remark is made?

Voltage Spike
  • 75,799
  • 36
  • 80
  • 208
Wally4u
  • 323
  • 2
  • 7
  • It says possible problems- most likely in certain circuits. All designs I have made for high speed circuits, mostly RF the ground fill (plane) is essential. But it does cause issues in trying to match certain components for RF and digital signals if need to fine tune signals - which requires expensive equipment anyway. Using helper calculations provided by some schematics is 'good' enough. But this comment is not good enough for an answer though. Just some of my experience that does not match the rest of the people on here. – Piotr Kula Nov 09 '12 at 14:53

2 Answers2

10

Sure, lets take the common case of a microstrip. Its impedance is a combination of itself and its return path (and the dielectric but lets keep it simple). In a microstrip's case this will be the reference plane underneath.

Now if you go and throw a piece of grounded copper right next to that microstrip, its impedance is now a combination of itself, its reference plane and that grounded copper next to it. You usually can't get a 100% symmetrical fill around the microstrip, because of vias, other lines or just going into a pin on a package. So in short anywhere you have this copper fill changing your impedance you are going to get discontinuities or changes in impedance.

For example in the image below there'd be a discontinuity for the main trace where the flood is interrupted by a via.

enter image description here

To be fair though there is a type of transmission line we sometimes use called a co-planar wave guide which essentially looks like a trace with two wide copper fills along its sides (symmetrically along its sides).

Neil_UK
  • 158,152
  • 3
  • 173
  • 387
Some Hardware Guy
  • 15,815
  • 1
  • 31
  • 44
  • 4
    What you drew is not stripline, it's microstrip. Stripline has two ground planes, one below and one above. Otherwise, excellent illustration of the issue OP asked about. – The Photon Nov 09 '12 at 16:59
  • Bah! True I meant microstrip, I'll fix that ;) +1 – Some Hardware Guy Nov 09 '12 at 17:04
  • So basically what you are saying is that by adding the Ground-fill beneath the connector (and because of the skin effect preventing the signal entering the ground-plane) it will need to go to the edge of the ground-plane and back to find its optimal route (similar to a segmented plain causing to route via decoupling capacitors ) – Wally4u Nov 09 '12 at 19:03
  • 1
    @Wally4u, you need the plane layer beneath the track to form an impedance controlled microstrip. Adding the fill area on the top layer gives the possibility of creating discontinuities (if you aren't extremely careful about it). This is what leads to the Ott quote (2nd in your question) that you asked about. – The Photon Nov 09 '12 at 22:02
1

There is a lot of misunderstanding, and not a great consensus on ground pours. From a high speed signal standpoint, here are the key considerations:

1 - PCB manufacturing can be inconsistent when there are large areas without copper. Hence we use thieving to provide fill. This could also be served with a large ground pour but we use small structure patterns for the reasons outlined below.

2 - Coupling to adjacent structures can result in increased crosstalk, or resonances in a signal path. I've seen low level resonances/reflections/discontinuities from structures that are, say 20mil away from my main signal line. Structures need to be small enough and/or far enough to avoid this.

2 - EMI due to Radiation. This can be produced by signals coupling to a structure which then radiates. A ground pour, while tied to ground through vias, can still receive a coupled signal and radiate.

3 - EMI due to ground (return path) disruption. In high speed, or RF, you have to think about routing ground just as you do the signal. They are one in the same. If you have a path for your signal that is 10mm long, you also have a return path that is 10mm long and just as important. If you have breaks or discontinuities in your return path, it's nearly identical to doing the same in your signal path. Ground pours can create additional return paths which are not consistent along a signal path. The inconsistencies can cause mode conversion, reflections, and EMI.

Ground pours are controversial, there are religious battles, and all that goes along with it. The key is to continue to refine your understanding so you can use all of these tools effectively.

But as a general rule of thumb, avoid ground pours in high speed. You're more likely to cause problems than avoid them. And most of all, you have to route ground, just as you route your signal.

65Roadster
  • 1,255
  • 5
  • 9
  • I’ve been a firm believer in number 3 for a while now; power is the original differential signal! – Bryan May 15 '22 at 19:23