I have a 4 layer PCB which has Analog ground, digital ground , AVDD as well as 2.8V and 1.8V. I think a 4 layer PCB is what I will use but I need to understand how to partition the power plane. For the ground plane I have it on Layer 2 and it is combined with AGND and DGND and I will minimize cross over on the top layer while routing.

But I am confused about the power plane. Does anyone have any suggestions? How do you handle multiple voltage levels on a power plane? Is there an alternative stackup?

  • 2
    \$\begingroup\$ A schematic or partial schematic showing the different powers would be helpful. My recommendation regarding power and analog ground is to simply combine them into one ground plane. It is very difficult to get good results from splitting ground planes. If you don't do everything just right, it will actually make noise and EMI worse instead of better. You should DEFINITELY consider all the return currents and which way they will flow and how they will effect each other. I just don't think you should actually split the plane. \$\endgroup\$
    – user57037
    Commented May 17, 2017 at 2:34
  • \$\begingroup\$ What about the power plane for multiple voltages? Usually layer 3 is power plane on a 4 layer stackup \$\endgroup\$
    – Sab VS
    Commented May 17, 2017 at 2:38
  • 1
    \$\begingroup\$ related thread: Can I lay traces on internal layers of 4 layer PCB? \$\endgroup\$ Commented May 17, 2017 at 2:40
  • \$\begingroup\$ It is hard to comment on the power plane until you give us some idea of how many power rails there are and what they are used for. But I never said you shouldn't split the positive power plane, or that you shouldn't have a power plane. I just said you should not split the ground plane. \$\endgroup\$
    – user57037
    Commented May 17, 2017 at 2:47
  • 1
    \$\begingroup\$ Is the "analog" designated for 12bit or 16 bit or 20bit or 24bit measurements? Or is the "analog" for power-drivers to solenoids? Or? \$\endgroup\$ Commented May 17, 2017 at 3:40

2 Answers 2


I second the advice to use a single ground plane. It is very difficult to get a split ground plane correct. In most situations a continuous ground plane will perform just as well -- if designed properly. Properly mostly means that digital signals and their return paths are kept separate from analog signals and their return paths. One way to think about it is to design as if you were going to use a split ground plane: designate analog and digital regions, and traces are not allows to cross the boundary without heavy filtering, but then simply neglect to do the split.

Splitting power planes is a good idea, especially on a 4 layer board. Try to arrange your PCB so that the various power rails can be nice contiguous regions. Concentrate first on the highest frequency, highest current, lowest voltage rails -- for instance, CPU and FPGA core logic voltages. Next, any power rail that supplies a large number of non-differential IOs. These are the power supplies that need especially low inductance. For less critical rails like opamp power supplies or low speed digital logic, you can just run traces for the power supply.

The other thing to keep in mind is that in a 4 layer stack like this signals on one side will be referenced to the power plane, not the ground plane. This means a few things. First, if you have noise on your power plane, signals referenced to it will see that noise. Second, if you have a split your power plane as suggested any traces that cross the gap won't have a suitable return path. If possible, avoid crossing breaks in the plane, but if you have to, use bypass capacitors. A special case of this issue is that if you use a via to go from the top to the bottom layer your reference plane changes from ground to power. Any signal vias like this need a bypass capacitor as close as possible.

In some cases, I have used a 4 layer PCB with both inner planes dedicated to ground, and run the power as traces. This won't work for a lot of applications, but this was a low density analog board and it worked great. I have also used a continuous ground + split power plane, but in one area placed a second ground on the power layer to accommodate ground referenced analog signals.

The advantage of having two ground planes is that when your signal goes through a via, the reference is ground on both sides. You still need to provide a path for the return current, but it can be a via rather than a bypass capacitor.

  • \$\begingroup\$ Good answer. When you have a signal going from top to bottom, do you bypass the signal or the power and ground planes? In other words, do you place the cap on the component side with via to power and ground, or something else? \$\endgroup\$
    – bitsmack
    Commented May 17, 2017 at 6:21
  • \$\begingroup\$ You connect the bypass capacitor to the power and ground planes in order to provide a path for the return current. \$\endgroup\$
    – Evan
    Commented May 17, 2017 at 18:18
  • \$\begingroup\$ What are the disadvantages of using both inner layers as a ground plane? \$\endgroup\$
    – Sab VS
    Commented May 17, 2017 at 19:19
  • \$\begingroup\$ You then have to route power through tracks on the top and bottom. This means using narrower power conductors which increases supply inductance, and also reduces flexibility in signal wiring. By using a power plane, you have two layers completely open for signal routing. \$\endgroup\$
    – Evan
    Commented May 17, 2017 at 20:01

Hopefully when you place your components they will be arranged in logical groupings based on voltage levels, e.g. a MCU with some surrounding decoupling caps and peripherals will be grouped together, and another circuit running at a different voltage level will be grouped together in another area, and so on. When that's done it should be simpler to define regions where a certain voltage rail dominates, and you would section that area on the power plane.

How you do it depends on your tool, but for example in Altium you would start with a solid plane (not a layer which starts empty and you add copper traces and other features, but a plane which starts as solid copper and when elements are added the copper is removed), and you would add lines to isolate various sections. Then you need to feed those split planes using vias from the voltage sources somehow. Perhaps the split plane passes under the regulator that supplies that rail, or you might bring a trace to the area.

Here's an example of what it might look like: split plane example

Be careful when you do this that you don't choke off plane areas with a lot of vias.


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.