0
\$\begingroup\$

I see a lot of discussion about using copper pours on the outer layers of a multi-layer PCB, as well as a single continuous ground plane on a multi-layer board, but there isn't a lot of information out there about ground pours on the internal signal layers.

For example, take a standard 6-layer PCB stackup:

Signal
Prepreg
Ground Plane
Core
Signal
Prepreg
Signal
Core
Power Plane
Signal

Where the top internal signal layer looks like this:

enter image description here

This signal layer contains the high-speed signals (SQI, USB, and Ethernet), as well as some other low-speed digital traces (GPIO). Should this layer also have a ground pour? Would this help isolate the digital traces, or would it cause more interference/coupling?

\$\endgroup\$
4
  • \$\begingroup\$ I thought it was a given that internal layers should have pours wherever possible too. After all, most boards don't relay on their two outermost layers as a shield. It does increase capacitance though. Sometimes good, sometimes not. \$\endgroup\$
    – DKNguyen
    Feb 12, 2020 at 23:53
  • \$\begingroup\$ I don't think internal layer ground pours are a given. None of the digital boards I've been associated with recently have had ground pours on internal layers. A typical set of internal layers for a 12 or 16 layer board looks more like this: GND:Sx:Sy:VCC, where Sx and Sy are X-direction and Y-direction (predominately) signal routing. One exception is when there's RF traces involved. \$\endgroup\$
    – SteveSh
    Feb 13, 2020 at 14:28
  • \$\begingroup\$ @SteveSh Those sound like pretty high speed digital boards though, right? \$\endgroup\$
    – DKNguyen
    Feb 13, 2020 at 15:27
  • \$\begingroup\$ Speeds vary all over the place, from couple of MHz to 500+ MHz (ADC or DAC clocking). It's as much about giving the PWB layout/routing tool & the manufacturer the ability to easily meet single ended trace impedance guidelines, 50-65 ohms. \$\endgroup\$
    – SteveSh
    Feb 13, 2020 at 15:48

3 Answers 3

Reset to default
3
\$\begingroup\$

I would not add ground pours to your inner signal layers.

The impedance of the traces on those inner layers is determined by the parameters of the stripline construction – trace width and distance to adjacent planes. Adding ground pours would just mess that up.

Isolation between signals on the same layer is better handled by trace separation. Adding ground pours in an arbitrary fashion can in some cases make things worse by creating cavities that can be excited at high frequencies.

If your analysis shows that you need more isolation between signals on the same layer than can be acheved with separation, you need to stich the ground traces/pours to the GND planes with closely spaced vias, as Bonnevie said.

\$\endgroup\$
2
\$\begingroup\$

It could be due to limited space for grounding vias. If you had ground pour around your shown layer it would be a very cut-up ground plane. This is okay if you could connect most of it down to your main ground plane. Rule of thumb is the via spacing should be 1/10 of the wavelength of the frequency used on the line. If you cannot connect the dangly-ground plane this well, you might be better without from an spurious emissions standpoint.

Another thing is, if you have more highspeed lines on your bottom internal signal layer your newly introduced ground plane on the top-internal would change the characteristic impedance of transmission lines on the bottom-internal.

\$\endgroup\$
2
  • \$\begingroup\$ There are no high speed signals on the inner-bottom layer, but there are some on the bottom layer. Everything was individually grounded with a via to the continuous ground layer before any copper pours were made on the top/bottom layers. Since the internal signals on the upper inner layer are impedance controlled, I don't want to change the impedance of those traces, so is it better to leave it off, or to add it on? The boards are expensive to produce (about \$260/ea in Qty 2) and I'd rather not get a couple paperweights back... \$\endgroup\$
    – Ron Beyer
    Feb 13, 2020 at 14:02
  • \$\begingroup\$ Ehh, well right off the bat, I think you are better off without it. Then you only have to think about microstrip impedance, and not routing sensible lines next-to/on-top-of each other. If you add it you should look at impedance going from microstrip to now being coplanar waveguide. This ground plane NEEDS to be properly stiched with vias to your "main"-ground plane. If it is meant to be large scale manufactured, you might get comments on copper balancing. Because so much copper is removed, it might be harder to plate your vias. \$\endgroup\$
    – EmilBonnevie
    Feb 14, 2020 at 7:31
1
\$\begingroup\$

My guess is that a ground pour on the high speed signal layer would reduce the variation in the characteristic impedance of the high speed signals, thus (slightly?) improving signal integrity. Might also reduce the thermal resistance from one side of the board to the other, which can help a tiny bit will thermal management options.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge that you have read and understand our privacy policy and code of conduct.

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