0
\$\begingroup\$

I am designing a 4 layer PCB with a separate power and ground plane. The electronics is all low speed. The majority of my design is 3.3V low power but the left side requires 24V and the right side has connectors that provide a connection to the 24V for power, alongside SPI and I2C. Can I just extend the 24V power plane, similar to the image: enter image description here

Usually I keep the power planes as simple as possible and stick to a rectangular outline. In this case the plane width reduces to a 3mm L shape (could be wider but I want to avoid signal traces crossing the plane gap) and would reduce some layout effort if I didn't need to use traces. I could also just route the power on the bottom signal layer as this is 4 layers, but how is that any different except having to use vias to get to the bottom signal plane? Is there any obvious shortcomings with simply extending the internal power plane as seen in the image? Would this affect the electronics (some analogue) in the 3.3V plane?

\$\endgroup\$
9
  • \$\begingroup\$ How much load do you have in the right side corner? How much decoupling is there for the 24 V? \$\endgroup\$
    – winny
    Nov 26, 2021 at 12:44
  • \$\begingroup\$ The right side corner could potentially be a fairly large load, as it is intended for future expansion boards that are powered from the 24V. The present 24V supply is is decoupled with 200uF and each board will have also have it's own decoupling. \$\endgroup\$
    – ChrisD91
    Nov 26, 2021 at 12:50
  • \$\begingroup\$ How high is "fairly large"? Are you switching it or is it just a DC flowing though the board? \$\endgroup\$
    – winny
    Nov 26, 2021 at 12:58
  • \$\begingroup\$ The 24VDC can supply up to 2A. The main board can draw up to 1A, so there's basically 1A shared between any expansions. There are no specs for future designs yet, but any potential switching will be done on the respective expansion board, so the power plane will be just DC \$\endgroup\$
    – ChrisD91
    Nov 26, 2021 at 13:02
  • \$\begingroup\$ Then you only need to worry about resistive heating. \$\endgroup\$
    – winny
    Nov 26, 2021 at 13:07

2 Answers 2

2
\$\begingroup\$

You can split the power plane exactly as you suggest. Absolutely do not break the ground plane up, as that causes return paths of signals that cross any ground plane gaps to have to jump those gaps somehow.

The specifics of your application, sensitivity to noise,EMI, stack up, etc. can impact these recommendations. But from your description, I don’t think there’s anything to worry about here.

Good luck!

\$\endgroup\$
0
\$\begingroup\$

That looks okay.

  1. Pair the ground with 24V.
  2. Split the ground where 24V splits.
  3. Make that splitting point very close to the 24V-in.
  4. Filtering & debouncing after the split.
  5. Add capacitors right where 24V exits to the extension board.

Edited.
Ultimate solution would be: Move the 24V_in connector and 24V-3V power circuitry to the right side all together.

enter image description here

\$\endgroup\$
5
  • 2
    \$\begingroup\$ I disagree. Don't split ground. Basically never do. If you are worried about common impedance coupling from 24V and 3V stuff from current in the ground plane, then use return traces for high current stuff. \$\endgroup\$
    – tobalt
    Nov 26, 2021 at 15:06
  • \$\begingroup\$ @tobalt , thanks for the comment. :-) I thought my posting was not yet visible. Yes, I agree with you, Meantime, power TRACE is a signal trace as well in a larger.. picking a word... scope. Probably, you are already over at the "exit side", which may need to take signals from the extension board, I am just guessing. And, I did not assume anything about it. :-) \$\endgroup\$
    – jay
    Nov 26, 2021 at 15:12
  • 1
    \$\begingroup\$ The problem with splitting the ground plane is that there are data lines (SPI, etc) crossing the 3.3 and 24v planes. If you split the planes that you will force the digital return currents to take a very ugly path through the board before they even get to the cabling. If there is concern about ground currents overlapping between the domains the solution is to route the board better so they don't overlap, but in this case I doubt there is a problem. \$\endgroup\$ Nov 26, 2021 at 17:27
  • \$\begingroup\$ -1- @user1850479 I understand what you & tobalt are looking at. I absolutely agree all the points. Meantime, when it is power (VDD-24V-to-extension & GND pair), EMI coupling is less concern. Separating VDD does not really give much advantage, while 3.3V not using it at all, except at the very input. The priority is the current, and controlling the path of it. I'd rather not give it to influence to the larger part of processing, low level, sensitive signal path, whatever amount it is, by passing through common ground current path, unless; The idea tobalt suggest is something I do, too, for \$\endgroup\$
    – jay
    Nov 26, 2021 at 18:11
  • \$\begingroup\$ -2- I do, too, for some cases, when the VDD (in this case) side behavior is deterministic/stable/low-current/etc. The concern is "if we don't give enough copper for the VDD side GND", and that easily leads to "well, we give all that we have, the whole ground plan.". Meantime, what I try is: controlling the path, design to have the signal domains are in the common mode range, and analog signal - that cross over domains- to have good common reference. "How" is only a technical matter. \$\endgroup\$
    – jay
    Nov 26, 2021 at 18:12

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.