I'm routing a PCB and, due to its small size, I'm thinking to use 4 layers. I'm planning to use top, bottom and two internal layers.


  • TopLayer : GND plane
  • Midlayer1: 5Vcc plane
  • MidLayer2: 3.3Vcc plane
  • Bottom layer: GND plane

It will have 3 ICs only (one 8 bit level shifter, one 8 bit bus switch and a 5 to 3.3 V regulator) and smaller components like TVS diodes, clamping diodes, resistors and capacitors. The current is not high, the purpose is to digital communications only. Frequency is not defined, but it will be no greater than 1 MHz.

I don't know if there is a generical rule for it, but someone know if Is there a preferable distributions of layers? A rule of thumb or something?


Due to some doubts and discussion I will refine the informationhere. The PCB will need to be very small, so I choose this distribution:

  • TopLayer : GND plane + components + signals
  • Midlayer1: 5Vcc plane
  • MidLayer2: 3.3Vcc plane
  • Bottom layer: GND plane + components + signals
  • \$\begingroup\$ To me it sounds like there is no reason to go with 4 layers, but please explain more to justify more than two layers. What chips, what packages the chips use, what frequencies are used, is impedance control needed? Preferably post schematics to assess the design further. \$\endgroup\$
    – Justme
    Commented Jun 22, 2021 at 17:57
  • 3
    \$\begingroup\$ I personally would use GND as one of the mid layers, then either 3.3V or/and 5V as the other mid layer, depending on the actual requirements of the circuit. Pouring on the external layers (of GND) would depend on the design as well. \$\endgroup\$
    – Wesley Lee
    Commented Jun 22, 2021 at 18:00
  • 2
    \$\begingroup\$ Don't waste a layer on power plane, give yourself 3 signal+power layers. Put ground as one of the middle layers. \$\endgroup\$
    – Neil_UK
    Commented Jun 22, 2021 at 18:37
  • \$\begingroup\$ I see no reason to go beyond 1 layer here unless you want it to look pretty. \$\endgroup\$ Commented Jun 22, 2021 at 19:24

1 Answer 1


There are two main conventions, but no rule of thumb as PCB layer stackups are design dependent. These are two general conventions:

[![enter image description here][1]][1]
Source: Electromagnetic Compatibility Engineering by Henry W. Ott

Using grounds on the outside to help with EMC, the grounds function as a shield that signals on the inside might use. Both schemes in figure 16-14 are good for shielding signals with either two grounds on the outside or a power plane and ground.

The problem with the scheme in figure 16-14 is the components are on the top layer, so you would need to use a lot of vias to route the signals to an inside mid-layer.

The scheme in figure 16-15 uses signals on the top and bottom and grounds in the middle, and in my opinon much easier to route, and is the scheme that I see used the most often.

I would use grounds in the middle and signals on the outside, it works for most designs. I use this scheme:

  1. Signal+Power+Components
  2. Ground
  3. Power
  4. Signals

Or this one:

  1. Signal+Power+Components
  2. Ground
  3. Power+few signals
  4. Power+Signals

As far as frequency goes, any traces over (generally) 50MHz will need to use transmission lines. In that case you do need to worry about many more things like the width of the traces and height between layers. At 1MHz losses are much less, you may have to worry about signals radiating off the board and causing interference (mainly with DC DC converters or clocks).

One Nice thing about having a ground layer in a middle layer is it creates a small amount of capacitance between planes and it keeps a continuous ground plane both of which work to reduce EMI and EMC problems in a design. If you don't have a continuous ground plane currents must go around components and it can add inductance and resistance to a ground plane.

With components on top layer becomes difficult to keep it continuous ground plane, this can also be a problem with ground loops or common mode voltage noise as a non continuous ground plane will have more resistance and inductance between the load and the source, especially on the low side of the load. If you do decide to go with grounds on the outer layer make sure they are continuous as possible.

Components on both sides does not really create issues for either stack up as it's only a matter of routing, however signal layers on the outside is much easier to route especially if you're going for more compact design

  • 1
    \$\begingroup\$ Using ground planes in top/bottom also helps to make reverse engineering more difficult (but not impossible). \$\endgroup\$
    – Damien
    Commented Jun 23, 2021 at 2:50
  • 1
    \$\begingroup\$ A plane has never stopped my exacto knife or screwdriver... you can also pay for x-ray services. If someone wants to find out what it is they will. Even conformal coats or epoxy can be loosend and pried off by acetone or other solvents. But yes, doors stop most thieves from breaking in. \$\endgroup\$
    – Voltage Spike
    Commented Jun 23, 2021 at 3:35
  • \$\begingroup\$ +1 for being an Ott fan! \$\endgroup\$ Commented Jun 23, 2021 at 7:20
  • \$\begingroup\$ @VoltageSpike . Very good you explanation and reference. In my design, due to its small size, I'm using components in both sides, Top and Bottom. So add an "edited" explanation in question \$\endgroup\$
    – Daniel
    Commented Jun 23, 2021 at 12:02
  • 1
    \$\begingroup\$ The answer is still the same even with components on the bottom layer the difference is that the bottom layer would be signal plus components or ground plus components \$\endgroup\$
    – Voltage Spike
    Commented Jun 23, 2021 at 12:54

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.