0
\$\begingroup\$

I have an FMC Card with analog circuitry containing channels. I've separated the ground for these analog channels into two distinct planes: AGND and PGND.

PGND serves as the ground for the power supplies required to operate the operational amplifiers in the analog channels. Now, I need to route the LVDS outputs of these op-amps to the nearby FMC connector, which is closely tied to PGND.

The LVDS pairs, operating at 500MHz, will need to traverse across both ground planes, AGND and PGND. I'm concerned about potential issues because I've come across literature cautioning against routing single-ended signals over split planes. However, in my case, it's a differential pair, and the return path is nearby. The ground planes are at the same potential but separated by a bead to prevent the return current from entering the analog chain.

Please let me know if you see any problems with my approach.

enter image description here

\$\endgroup\$
5
  • \$\begingroup\$ Why did you split the ground like that? Ignoring the effect on your controlled impedance traces (very bad), logically the connector that an device is driving should be connected the same ground plane as the source or you're going to have problems. \$\endgroup\$ Commented Sep 22, 2023 at 16:21
  • \$\begingroup\$ Redo your board. Either 1) add another layer that can be dedicated to one of the two returns (A or D), or 2) lay the board out differently so the LVDS signals don't have to cross different return planes. \$\endgroup\$
    – SteveSh
    Commented Sep 23, 2023 at 2:54
  • \$\begingroup\$ @user1850479 i want the analog ground to be low noisy, so i dont want the return currents of PGND which is noisy power supply ground not to enter in to AGND \$\endgroup\$
    – kakeh
    Commented Sep 25, 2023 at 9:37
  • \$\begingroup\$ @kakeh - You may be able to do that with a layout change, and having only a single return plane. Keep in mind that currents flow in loops. So you may be able to keep the noisy PGND currents away from the analog stuff, even with a single return plane. \$\endgroup\$
    – SteveSh
    Commented Sep 25, 2023 at 11:50
  • \$\begingroup\$ @kakeh That is not necessarily a good reason to split grounds, and if you do you can't route high frequency signals like that over different grounds. You'll need to carefully think about how to split them to ensure everything stays over its own ground. \$\endgroup\$ Commented Sep 25, 2023 at 12:51

3 Answers 3

5
\$\begingroup\$

Differential pairs over a ground plane are essentially two single ended transmissions lines with maybe a little coupling to each other. So in most practical geometries the majority of the return current flows in the plane and not in the other track of the pair.

What's often done with planes at different DC potential is providing a high frequency return path with capacitors. But that's pointless with a split ground plane since removing the split achieves basically the same thing except providing a return path for frequencies all the way down to DC.

Long story short: You don't split ground, unless you know exactly what you are doing. There are very few cases where a split in a ground plane actually makes sense.

\$\endgroup\$
1
  • \$\begingroup\$ i want the analog ground to be low noisy, so i dont want the return currents of PGND which is noisy power supply ground not to enter in to AGND, what could be better approach, i took this approach after reading analog.com/en/analog-dialogue/articles/… \$\endgroup\$
    – kakeh
    Commented Sep 25, 2023 at 9:29
3
\$\begingroup\$

No no no no no no no!

Do NOT separate grounds like that, whether they're planes or not. This is where ALL your circuit's return-current passes. When you 'break it up' it has to take a longer path, which means a larger loop area, and that creates EMC failures. And that ferrite bead linking them will likely have the opposite effect to what you intend; what is a ferrite bead? It's an inductor within a frequency band. What does an inductor do? It slows down delta-I. Is that what you want? Probably not if it's your 'intended signal'.

You completely avoid this problem by: (a) not having multiple grounds unless there's relatively rare/special circumstances, or actual galvanic-isolation reasons to do so. Your situation doesn't qualify. and... (b) geographically separating analog and digital/power clumps of circuitry so that their return-currents across the adjacent/underlying plane (typically GND) don't cross each other.

Problem solved.

In the rare circumstances where a diff-pair's return-current needs to cross planes (whether they're at the same potential or not i.e. from a GND plane to a Vcc plane) is to add coupling-capacitors directly adjacent to the diff-pair vias. But you need to get that design & coupling-capacitor value right.

\$\endgroup\$
3
  • \$\begingroup\$ my analog chain is with very high gain, any noise entering from power ground to analog ground would appear in output and would make design vulnerable,i wish to seperate both grounds fro this reason, in my case the two different planes are of same potential except that one is less noisy and other is more noisy \$\endgroup\$
    – kakeh
    Commented Sep 25, 2023 at 10:13
  • \$\begingroup\$ @kakeh - If your application is that sensitive, then take my advice (in a comment above) and add another return layer. \$\endgroup\$
    – SteveSh
    Commented Sep 25, 2023 at 11:59
  • \$\begingroup\$ @takeh "Please let me know if you see any problems with my approach." I understand what you're trying to do, but you've come here for advice because somewhere you've probably read that what you want to do is actually a bad idea, and then when everyone does indeed say "don't do that!" you say "but reasons!", probably because you don't want to face the need to change the physical layout of your board so that analog & digital/power return paths don't cross. Tough titties. This is a learning process. \$\endgroup\$ Commented Sep 25, 2023 at 14:08
1
\$\begingroup\$

The return path of a "differential pair" microstrip is still the plane. Using only the traces mutually will bring up impedance greatly and exceed LVDS specs.

You could route the Diff traces in neighboring layers over the split, to bring down impedance.

It may be even fine as is considering the impedance discontinuity is only very short, but still:

  1. question the decision to split these planes. They should be coupled at DC anyway, to still within the CM signal level range of LVDS of a Volt or so.
  2. do (1) again, carefully.
  3. a cap between the planes in the vicinity of these pairs can let HF CM currents flow between the planes.

As you can see the required measures in 3 make the planes joint at both DC and HF. So effectively negating the split apart from at low-medium frequencies. Therefore, return to (1).

\$\endgroup\$

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.