Can a different power supply plane be a Return path for a signal in trace?

[myatham]

Hello All,
Can we use different power plane as reference for a signal which uses different power supply?

I think using ground plane as reference is always best, if not possible, we need to use any reference power plane as reference but that power plane has to be tightly coupled to ground with decoupling capacitors. Please correct me if i misunderstood anything.

Can we consider either ground or power plane as refence for impedance calculations?

 

[albbg]

Yes, as you said the ground plane is the better choice but also power planes can be used as reference. That power plane has to be large enough to reduce as much as possible its impedance.
Be careful about the noise that could be carried by power planes mainly that connected to DC/DC converters or pulsed loads.

 

[marce]

If the power plane is bouncing or noisy so is the ground plane usually.
A signals return will couple to any adjacent plane, the thing to watch is crossing different planes, there could be problems.

 

[albbg]

If the power plane is bouncing or noisy so is the ground plane usually.

Usually the ground plane is larger than power planes so the noise density (per area) is less.

 

[marce]

!!!
The ground is bouncing merrily with all the switching of the logic and is related to ALL the different supplies.
And if you use a plane that is smaller than the signal travels the signal will have to cross from one voltage plane to another, not good for high speed signals, greatly increases the return loop...

 

[albbg]

!!!
And if you use a plane that is smaller than the signal...

Yes, but this means the PCB has not properly designed.

 

[marce]

What are you on about, I don't understand your comment. Often power planes have multiple voltages on them so have small copper pours, so if a track is next to the plane it will have to cross a gap. This is no problem for lower speed signals.

 

[albbg]

it could be I didn't clearly understand your sentence in #5; however I meant that tracks carrying signals that have to be treated with care (rf/high speed) should avoid to cross multiple power planes. I think, in that case is better to add in between a ground layer to the PCB.

 

[marce]

I agree, a contiguous ground plane is best, but not always possible...Then you have to sort the correct tracks to the correct layers to avoid crossing planes...

 

[praveenlb]

marce.can we use stitching capacitor where signals are crossing the split plane.....?

 

[marce]

Yes, that's the standard practice, it can soon take up a lot of room as the cap needs to be a near the signal crossing as possible. I think Henry Ott has a good paper on it.
Hers a couple of other links...
http://pcdandf.com/cms/magazine/192/3413-effects-of-plane-splits-on-high-speed-signals-parts-1-and-2
http://www.hottconsultants.com/techtips/pcb-stack-up-6.html