Are there reasons *not* to have a copper-pour ground plane on a PCB?

Question

I am taking a first stab at designing a PCB from scratch. I am considering using a CNC mill fabrication process, and it seems like with this process I would want to remove as little copper as possible. A copper-pour-style ground plane would seem to be a good way to address this constraint.

But I have noticed that relatively few PCB designs have a ground plane, and even those that do often have them only in specific areas of the board. Why is that? Are there reasons not to have a copper-pour ground plane that covers most of a PCB?

In case it's relevant, the circuit I am designing is a 6-bit D/A converter plug. A first cut at my PCB layout (which does not include a ground plane) is shown below.

Answer 1

Ground planes in general are almost always a good thing, but if used incorrectly can actually hurt the quality of your board.

A typical board like you have here would have 1 layer dedicated to be a ground pour only with no traces running on it. However, it sounds like you are wanting to make your top layer have a ground pour so that you don't have to remove all of that extra copper. Doing a ground pour on a layer with a lot of traces is not really a ground plane at all, rather you can think of it as a ground trace with varying sizes running all around your board. It is hard to say if it will actually hurt the signal integrity of the design, but I can say for certain that it will not provide the same benefit that a ground plane will.

Typically when I see milled boards like this, the copper will be left unconnected on the unused areas of board. This provides a benefit of knowing that if you accidentally short one line to the unused copper, you don't get a hard short to ground that can kill some ICs. This can also be a negative though as accidentally shorting to a large unused piece of copper can turn into a nice antenna and pick up noise that you may have a hard time hunting the source of.

I realize my answer may not be a direct answer to what you are wanting to know, but it is very difficult to predict what configuration will be best for you. But, if it were my design, I would go ahead and just leave the extra copper on the board, but leave it disconnected from everything.

Answer 2

Air-core inductors should not be used with their flux passing through a ground plane; otherwise the ground plane acts like a parasitic transformer with a shorted turn.

I've had to deal with this in a poor design made by a contractor and it was not fun.

Answer 3

As Kellenjb said, ground planes and ground pours are almost always a good thing.

So far, I've only encountered two situations to avoid putting a ground pour or a ground plane on a PCB (neither one of which apply to D/A converters):

• RF transmitters, in particular: no ground plane near the "PCB antennas" often used for RFID. a b c
• CCFL lamps: "the ground plane should not be placed under or near the high voltage floating side" (IRS2552D); "ground ... planes should be relieved by at least 1/4" in the high voltage area" -- Jim Williams, LTS AN65 (I imagine this is true for other high-frequency, high-voltage systems such as other kinds of fluorescent lamps and Tesla coils)

A possible third case is capacitive touch sensors (CapTouch, CapSense, etc). Some people put ground planes under the sensors, others cut out the ground plane under the sensors. It's not clear to me which way is better overall.

Answer 4

Ground plane needs to be cleared out for high voltages eg. mains to meet the creepage and clearance rules for safety.

Continuous plane on one side which is not matched by a similar size area on the other side leads to the board warping because of the tension provided by the copper.

Unconnected bits of copper act as antennas and can increase noise in your circuit. You are usually better off eliminating them if you can't connect them to ground.