I seem to have confused the terminology between signal and power planes! There is a ground plane, plus potentially four power planes -- +/- 15V, +HV (200V), and i'm not sure if a -VREF (~ -7V) reference voltage should be considered a "power" or a "signal".

I guess what I'm really wondering is whether it's considered kosher to turn the +/-15V, +HV, and -VREF into solid copper layers analogous to the ground plane, as opposed to trying to draw out all those traces.


I'm laying out a schematic for a piezo driver on a multi-layer PCB. The schematic has potentially five signal layers -- a ground, +15V, -15V, -VREF (-6.95V), and a +HV (+200V). Is there any advantage/disadvantage to having 5 signal planes? Is there a "best practice" on how to order them? The output is a ~0-150V signal, which might be a low-frequency sweep of ~ 10 to 100Hz, or a high(er) frequency dither of ~ 1-100kHz.

  • 3
    \$\begingroup\$ ... may as well make it a six layer board, the cost is probably the same either way \$\endgroup\$
    – vicatcu
    Oct 3, 2012 at 20:11
  • 2
    \$\begingroup\$ You seem to be confusing the number of layers in your PCB with the number of power supplies you have in your design. The two are actually quite unrelated. \$\endgroup\$
    – Dave Tweed
    Oct 3, 2012 at 20:22
  • \$\begingroup\$ @DaveTweed -- yeah, i just figured that out! Completely new to this... I'm amending my question. \$\endgroup\$ Oct 3, 2012 at 20:35

3 Answers 3


This set of articles has been referenced a number of times on this site and it's quite a good primer. Read through it and decide which goals you are content to optimize for.

http://www.hottconsultants.com/techtips/pcb-stack-up-1.html http://www.hottconsultants.com/techtips/pcb-stack-up-2.html http://www.hottconsultants.com/techtips/pcb-stack-up-3.html

... read on for more layers.

Here is an excerpt of the objectives of stackup design:

When using multi-layer boards there are five objectives that you should try to achieve. They are:

  1. A signal layer should always be adjacent to a plane.
  2. Signal layers should be tightly coupled (close) to their adjacent planes.
  3. Power and Ground planes should be closely coupled together.
  4. High-speed signals should be routed on buried layers located between planes. In this way the planes can act as shields and contain the radiation from the high-speed traces.
  5. Multiple ground planes are very advantageous, since they will lower the ground (reference plane) impedance of the board and reduce the common-mode radiation..

If you read through the articles, you'll find that there is no one "best" way to stack up your design. There are just a number of possibilities with different characteristics and tradeoffs.


You don't need to put your high voltage tracks or plane on its own layer. But you should make sure that it keeps its distance from tracks on the same layer. Some PCBs have slots cut in them to separate areas with a large voltage difference.

Inside induction hob

Notice the black slots around some of the resistors, and near the heatsink.

Also, you don't have to dedicate an entire plane to each power supply voltage. In fact, you don't have to dedicate any plane to any power supply voltage or ground. You could probably do this in two layers. Someone designing a piezo driver for a commercial product may even be able to do it in one. It's amazing how many products you can open up to reveal a single sided PCB. For example the PCB in this answer! It's from an induction hob. It's got a bunch of high and low voltages on it, and very high currents too, but doesn't worry about having 5 or 6 layers.

  • \$\begingroup\$ "In fact, you don't have to dedicate any plane to any power supply voltage or ground" Good advice, IMHO. I've never understood some designers' obsession with power planes. Power comes from bypass capacitors near the devices being supplied, not planes or traces. \$\endgroup\$
    – user572
    Oct 4, 2012 at 2:47

In general you want to have a a symmetrical stack, so 4 or 6 layers in your case. I realize you only said five signal layers and not what you'll be doing for power, but I'll ramble on anyway. Uneven stacking can lead to warping problems. Like if you have the top layer as a plane and then five layers of signals. When that's heated in the oven it's going to warp like a potato chip. Some people like to keep their signal layers routed orthogonally to reduce cross talk so you can'd do that as easy with 3 sig layers on top of one another.

Also I don't think it's going to save you any money, the board houses like to do things it twos also.

Looking at your signals (damn +200V hah), I'm thinking you'll want to isolate that high voltage signaling from your low voltage work. So maybe an extra plane for that is not really the way to go? You might want to put him on one edge or something. Tough to say without knowing your design. I feel like if I brought that to UL for a safety cert that's what I'd have to do. Unless of course your whole system can never be touched by a person.

  • \$\begingroup\$ Ah, i think i confused terminology... the +/-15V powers several op-amps and a few other ICs; the +HV (200V) powers two PA84 power amps. \$\endgroup\$ Oct 3, 2012 at 20:31
  • \$\begingroup\$ FWIW, the board will ultimately be packaged in a euro-card rack, with input/output signals being routed through BNC connectors on the front panel. \$\endgroup\$ Oct 3, 2012 at 20:33

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.