Currently I am creating a 6-layer PCB. I have multiple voltages as 3.3V, 5V, 12-14V and 48V. Now I am sitting on the stack up to get started with the tracing.
Should I put multiple power planes for the different voltages?
Would it be possible to make on power layer and multiple GND and signal layer, then tracing some of the power traces on one of the signal layers?
One power plane for each voltage would probably give good results without having to think much about what you do. But I doubt you can get 4 voltage planes + all the ground planes + signal planes into 6 layers. So if you don't care about money, then just increase the number of layers to give each voltage its own plane.
If the cost of the PCB matters to you (more that the extra time to design it), then you can probably reduce somewhat the number of planes required for power :
Think about where you need each voltage. I'm betting either you don't need all of them everywhere to begin with, or components can be arranged with little effect on other constraints, to make exclusive regions where each is necessary.
Consider the size (relative number of pins) of each net. The more numerous ones are probably more generalized (evenly distributed over the board), too. These are good candidates for board-wide planes, or indeed the reference plane (GND itself).
It's generally a good idea anyway, to separate higher voltage / power nets, as transients/noise will be worse around them, and heat generation. These can be kept separate from low level signal/control sections.
Considering these points, you might not even need 6 layers anymore. Generally, 6 layers are only needed for very dense components like BGAs, high currents particularly with high complexity (more layers = more copper overall; with enough component density, fine pitch, or number of connections, that a heavier 2 or 4-layer build isn't practical), or occasionally for dense builds otherwise (perhaps with blind/buried vias or even HDI to allow components/pads to overlap).
There isn't a hard and fast rule for when to use a power plane instead of a trace. Here are some instances where you might want to consider using a power planes:
The down side is that power planes eat up a lot of available copper for routing. A work around is to use split planes (planes side by side on the same layer with a gap in-between).
For high speed signals there are some power plane stack ups that are detrimental in terms of EMI. The following presentation is from Rick Hartley on "How to Achieve Proper Grounding", which also discusses issues with power planes:
https://www.youtube.com/watch?v=ySuUZEjARPY
See from 1:45:19 to 1:50:54 for a discussion of six layer boards.
I design moderate sized boards (10" x 8") with multiple rails on them. Usually 24, 12, 5, 3.3 and one other specialty rail. It is fairly straightforward to put all your power planes on one layer as long as you can control component placement. In my boards they're driving stepper motors, solenoids, sensors, etc. Around the very outside, about 0.1" wide is chassis ground. This is separated from everything else by 20mil or 40mil. Next in a big 'U' shape goes the 24V rail since all the 24V stuff is usually on the outside, driving external systems. Then inward is the 12V, and 5V. Finally, the middle section is all 3.3V since that's where the microcontroller and low voltage circuitry is located. A couple key points: a. Think about power routing when doing initial floorplanning b. Don't make any plane a complete ring - leave an opening on one side to minimize current loops c. Know that occasionally you will need to use traces to get a power signal out to the plane where it needs to go d. If the source and sink of a rail are far apart, be sure to use enough decoupling capacitance.
