I have a board with a mix of voltages. It wound up being one voltage to one side of the board, and one to the other. I'd like to make this board 4 layers instead of the original 2. Is there any reason I shouldn't split the internal +ve voltage plane into two? A 3.3 VDC on the left and a 12 VDC on the right on a single internal layer? I'd keep a single ground layer for all.

I don't immediately see an issue with this and it would save cost from needing 5+ layers.

  • \$\begingroup\$ Do either of the voltages ever need to cross over onto the other "side"? \$\endgroup\$ – Ignacio Vazquez-Abrams Oct 3 '16 at 13:54
  • \$\begingroup\$ No, they do not. \$\endgroup\$ – EscapingBlueSmoke Oct 3 '16 at 13:57

I had some experience with multi-voltage boards (design that for whatever reason need different voltages for different parts of the circuit).

I learned the hardway that multiple voltages can be treated the same way you treat different ground signals (for example analog and digital ground). That is, you dedicate different parts of your board to different "functionalities".

Therefore, if your design permits it, put all 5V components on one part of the board, an all 12V components on another part. That way you can have both voltage planes coexist in the same layer of your PCB, as they would not overlap.

  • \$\begingroup\$ Depending on the frequencies the split does not really matter which is the case for majority of signals except for data buses and clock. With regards to power distribution, I favor routing power planes along edges of the PCB which allows you to reach various places on the board while letting majority of the PCB to use an unified voltage plane and/or gnd. YMMV and the application matters. On real high speed signals using power plane as reference requires providing bypass caps whenever you change reference plane as well as start and stop. Gigahertz is funky. \$\endgroup\$ – Barleyman Oct 3 '16 at 14:11

There is one reason why not to do this - If you route high speed signals over the gap between +12V and +3.3V planes, you're getting a double dose of signal integrity issues and EMI transmissions.

As long as you're aware of that, there's indeed no reason not to split power planes. There are ways around that problem such as using a capacitor next to the lines to "stitch" the power planes together at RF or perhaps by adding GND copper to the power plane where possible.

Note that "high speed" is highly fuzzy term. In today's gigabit clock speed environment 10MHz may appear to be more or less DC. However the clock edges contain far higher frequencies that won't be happy about discontinuity in reference plane.

  • 1
    \$\begingroup\$ Good point to keep in mind, but I wouldn't say it's a reason not to have a split power plane. Just ensure you route all the high-speed signals on the layer adjacent to the ground plane. \$\endgroup\$ – Armandas Oct 3 '16 at 14:08
  • \$\begingroup\$ @Armandas Yeah, which gets into the territory of careful handholding of the signals. Unfortunately you need separate planes for horizontal and vertical routings with any kind of complexity and on a four-layer board one of these is usually not going to have the luxury of a nice uniform GND plane. I often spend some time at the end of a layout project going over digital signal traces to ensure they're not crossing reference planes where possible. You will still have the issue where your reference plane jumps from VCC to GND when changing layers. Unhappy customer if closest bypass caps is "far". \$\endgroup\$ – Barleyman Oct 3 '16 at 14:16
  • \$\begingroup\$ @Barleyman, A 4-layer board is not likely to have the benefit of distinct horizontal and vertical routing layers. \$\endgroup\$ – The Photon Oct 3 '16 at 15:43
  • \$\begingroup\$ @ThePhoton Sure it does. Top and bottom! The less space you have to play with the more religious I get with routing direction as it almost always backfires on you if you play fast and loose with it before you have to squeeze the last few traces in. \$\endgroup\$ – Barleyman Oct 3 '16 at 16:38
  • \$\begingroup\$ @Barleyman, in my designs, at least one of those is usually too full of parts to be dedicated to routing in just one direction. Of course then trying to do 4 layers with 2 dedicated plane layers might not be such a great idea. \$\endgroup\$ – The Photon Oct 3 '16 at 16:51

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.