5
\$\begingroup\$

When designing a PCB, I understand that it's often good to design the ground signals so that:

  1. They follow the signal in reverse (make return path be same as out path.)
  2. They do not daisy chain, but instead connect back in a "star."
  3. They minimize the return path length.
  4. They have the same trace width as the signal.

These are sometimes contrary to each other, but that's OK -- if it was always straightforward, it wouldn't be called "engineering" :-)

Here's what I don't understand, though: I also see the recommendation to do a polygon pour for the GND net, on both sides of the PCB. I mainly work with through-hole components on two-sided boards at <= 20 MHz frequencies; 1 oz copper; FR-4; 1.6mm thickness; ENIG.

So, once I pour the copper, the traces I designed for the four original points kind-of go out the window, right? If I know I'll have ground pours, do I not need to pay attention to the "no daisy-chaining of ground" anymore?

Also, I try to route most signals on the top layer, and keep the ground layer somewhat less crowded; is this actually worth anything, or is a snake pit of traces equally distributed on both sides about just as good?

And would there be any benefit to pouring VCC instead of GND on the top layer? Especially if that layer is pretty dense with signal traces anyway?

\$\endgroup\$
  • \$\begingroup\$ I think these sorts of "should I do [design practice] or [conflicting design practice]?" questions are better addressed by understanding the underlying reasons the design practices exist. The answers to your questions really depend on the nature of the signals carried on the board and traces, and your performance and cost requirements. \$\endgroup\$ – Phil Frost Sep 2 '13 at 12:52
8
\$\begingroup\$

It's a common design strategy to have a GND copper pour, which covers most of the bottom copper layer. In this strategy, the bottom layer is used for routing as little as practical in order to keep the GND copper pour uninterrupted. The goal is to mimic a ground plane like in a 4-layer board.

Here's an example: enter image description here

Let's see how this would agree with the design rules in the O.P. I treat them as general rules. I'm ignoring more specific things, such as low noise circuits or power circuits, which may require a different interpretation of these rules.

  1. A ground plane is under the signal trace. The DC component of the return current follows the path of least resistance. The AC component of the return current follows the path of least impedance, and it runs under the signal trace.
  2. Star ground. Each sub-circuit can sit on its own local GND copper pour. Local GND pours are connected to one point, which will be the center of the star. Alternatively, slits can be made in the GND pour between the sub-circuits.
  3. Minimize the return path length may conflict with rule 1. Which would it be: minimal path or same as the signal?
  4. Ground connection should have low impedance. Usually, ground traces are wider than signal traces. I doubt that "same trace width as the signal" is a good rule for the general case.

Design rules similar to the ones in the O.P. are also discussed here and here. (Analog devices has quite a few application notes on grounding. Search their site.)

\$\endgroup\$
  • \$\begingroup\$ Thank you for a good answer! The one thing I still don't know how to trade is star-ground versus filled ground pour. (Or a full ground plane on a 4-layer for that matter.) It seems to me that ground planes and star grounds are not compatible -- when do I choose which? \$\endgroup\$ – Jon Watte Sep 2 '13 at 4:52
  • \$\begingroup\$ @JonWatte: I think the idea with point #2 is that current should have ways of getting from each device to ground without having to go through the copper that's feeding other devices. Using a ground plane can help accomplish this by providing multiple paths. \$\endgroup\$ – supercat Sep 2 '13 at 13:21
  • \$\begingroup\$ I'm of the opinion that star grounds and ground pours aren't really compatible. If you do use ground pours, make sure that each ground island has multiple ground vias to the rest of the grounds. \$\endgroup\$ – rfdave Sep 3 '13 at 2:14
  • \$\begingroup\$ @Dave Star ground usually works on the level of sub-circuit. It's usually not practical to have a star ground connection for each individual component. The idea behind the star ground is to prevent the return current of on sub-circuit from interfering with another sub-circuit. Power supply, digital circuitry, analog circuitry, each can have it's own ground. It makes sense to have separate copper pours for each of them (especially power and analog). Then, these copper pours are connected to one point, which is a the center of the star. \$\endgroup\$ – Nick Alexeev Sep 3 '13 at 2:50
  • \$\begingroup\$ @Dave In the example, which I've posted in the answer, there are two GND pours (red areas). The small left-hand-side pour is digital ground. The larger right-hand-side pour is analog ground. There red trace connecting them is one of the star ground rays. \$\endgroup\$ – Nick Alexeev Sep 3 '13 at 3:01

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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