5v traces on 3.3v power plane

I’m doing a simple pcb, I’m using 3.3v for pull ups on switches, so most traces are 3.3v (power and signal), but there’s some leds on the same layer that need 5v for power, I already did a 3.3v power plane on the layer, so I was wondering if it’s ok to route 5v traces for these leds on the 3.3v power plane, would it interfere with other 3.3v traces or cause problem on the plane?

I use layer 3 for lots of power distribution in many projects, with layer 2 being solid ground – then signals mostly on top, and bottom as needed. Layer 3 is also handy for those last needed signal jumpers. L3 also a good place to route noisy signals (buried with ground plane below it on bottom layer as well as L2 above). This board has many different power voltages and references distributed to different areas, with infill of digital and analog ground:

If you have a 3.3V plane you can easily add a fat 5V trace to it. You need to cut through 3.3 distribution as little as possible (eg: not down the middle as much as practical). I like to route the secondary voltage around the outer perimeter, and shoot branches inwards from there, sometimes finishing some of the run on a different layer.

1 Like

Very few boards are single supply these days. I rarely put in power planes, my priority is an unbroken ground plane. I often end up with a few power “trees” on the same layer


It looks that you use 3V3 mainly (or only) for pull ups. Pull ups rather don’t need high current.
Plane has 2 advantages:

  • can lead higher current than track,
  • ensures good return path for fast switching signals (mainly GND plane, but sometimes also VCC plane is used for it as high frequency ignores DC voltage at plane).

If none of these is needed from your 3V3 plane then may be it is not needed at all.

At 2 layer PCB I use GND plane at both sides with one (typically bottom) being continuous, and I route VCC as other signals.
My example:

All vias you see there are GND.

This is the way. Power planes aren’t mandatory in most cases and the routing benefits are relatively small, while good GND is always important. A nice star-shaped supply is the default.

If none of these is needed from your 3V3 plane then may be it is not needed at all.

That’s really interesting, my rationale for adding a 3.3v power plane to the top layer instead of a ground one was based on how getting a ground wire closer to a “pulled up” signal wire triggered a false low digital noise in my physical circuit. So if I switched it for a ground plane on the top layer, are you telling me the ground copper around the signal traces wouldn’t disturb my signal?? I’m very new to working with PCB design so all this is new to me hh

I already have a continuous ground plane on the bottom just for ground connections to through holes and smd pads, so I’m fine there.

The best proven concept in PCB design is to have a good GND plane. Rick Hartley (from altium) has made an excellent 2 hour video about the importance of GND planes, and it is really worth watching (on youtube). That is how important the GND plane is. It is the reference for “everything”, and the return path for all currents. (How currents flow though the GND plane is a big part of that video).

Next thing is decoupling capacitors. Local decoupling capacitors near each IC buffer power supply voltages, filter noise and stabilize them with also the GND plane as a reference. As a result, power distribution over the PCB is mostly DC, and the frequency content of ripple currents (except from the short distances between the decoupling capacitors and the IC’s) should be below approximately 1kHz. That is about the limit where DC resistance dominates the impedance. Already at a few kHz, loop inductance starts to dominate the impedance of PCB tracks.

As a result, as long as the DC resistance is small enough in your power delivery system, there is no advantage to use power planes. And even if there are ripple currents with higher frequency content in the power delivery, they are still referenced to the GND plane, an loop inductance is still minimized.

This sounds like board contamination causing leakage from the signal track to nearby tracks

A copper pour of GND under all signals improves signal integrity because it lowers loop inductance.

All wires have inductance, and if you connect your GND with a wire, the inductance of this wire disturbs the local GND during signal transitions.

Maybe it’s a silly analogy, but I just got a vision. Suppose a bucket of water as an analogy for a signal transition. If GND is a wire, this bucket gets thrown into your face. If you have a GND plane, then the bucket of water is pushed over the table towards you. It may still slosh a bit (generate noise) but the level surface used as a reference keeps everything in check.

Oh I see now, thank god I didn’t send the gerber files yet, I’m gonna remove that power plane then, would you in my case (considering I only carry 3.3v traces and some 5v traces on the top layer) recommend either way a ground plane on the top layer because as you say “improves signal integrity”, or it’s enough with the one I already have on the bottom layer?

In that case I would end up with a GND plane on the top and bottom layer, so I guess that would be better for the signals

I don’t know about the specifics of your design. But I generally pour GND on all planes unless specific components like power inductors require empty areas below. Just make sure to stitch them together properly and put vias near the outlines and where tracks merge to prevent stubs and reflections.


I’m not sure what “false low digital noise” exactly is.

Your top layer track and bottom GND plane looks like capacitor. Your track and top GND plane have very little surfaces seeing at each other. You can set top GND zone clearance intentionally bigger (like 0.5mm).
In my PCB I have linked in my previous post you can find something (see top left from main IC) looking like a wire ended with vias (it is not the only one there). And I said all vias you see are GND. So it is not the signal line traveling here. My intention was to shield fast output signals from slow input signals.

If you read and understand all articles I have mentioned here:

and here:

you will have knowledge enough for most PCB designers.

Having continuous GND plane is mainly important for return paths and not connections. Connections could be done with tracks.

If you will solder your PCB yourself GND at top is not needed (bottom should be enough). If it be automatic assembled than having comparable amount of copper at top and bottom is important to avoid bending the board during reflow soldering.
In my opinion GND plane is always good from EMC point of view, but sometimes not good from other points of view (may be even signal integrity).
Around 2000 I have redesigned PCB that originally had no plane at all and suddenly OpAmp begin to oscillate because being loaded with too high capacity.

Switch to 4 layer and have 2 GND planes on the inner 2 layers, due to the layer stack up it gets your GND planes closer to your signals . . . and watch the Rick Hartley video a few times.

1 Like