Splitting Planes—The Good, The Bad And The Ugly
Table of Contents
Splitting planes or making plane cuts is another one of those technical issues wherein there is a lot of conflicting information. Some say it’s a good thing to split planes; others say you can split ground planes and power planes both, some say you make cuts only in power planes, and others say to avoid plane cuts altogether. This article will debunk the myths surrounding split planes, provide evidence as to when they are useful, and describe when they should not be made.
As noted above, splitting planes or making plane cuts is one of those topic areas that is plagued with a lot of misinformation and confusion. Following are some of the more frequently made comments, which serve to confuse the topic as a whole, and do a disservice to product developers. It should be noted that the “anti-split” warnings are somewhat randomized in terms of where they should be placed, why they should be done and what harm they can do. They include:
“Crossing a split plane with a trace is bad because it increases inductance and complicates the path for the return current.”
“You split ground planes to reduce common mode noise on its analog side “
“Position your board into separate analog and digital sections.”
“If you isolate your analog sections, you need split planes.”
“Crossing a split plane should never be done because of the increased risk of crosstalk and not meeting EMC requirements.”
To make things easier, we can readily debunk all of the foregoing and say they are not true. But, perhaps one of the most important takeaways is that you should NEVER, EVER split ground planes. If you do, you will destroy the integrity of your PDS.
Lee Ritchey, Founder and President of Speeding Edge notes, “There are self-proclaimed EMI gurus who advocate the cutting of the ground plane because there is a current circulating in the ground plane that will upset some analog signal somewhere. The idea here is that you turn a patch of the ground plane into a little island and attach it at one place. In almost every case I have seen, someone is assuming some sort of magic problem exists because the currents are circulating in the ground plane. In actuality, every time I have seen someone cut a ground plane they have created an EMI problem.”
So, once we have eliminated all the bad data which continues to circulate about ground splitting, the discussion moves to power planes, and there are legitimate reasons for splitting them. Those reasons and the ways to implement them are detailed below.
There is only one reason ever for splitting a plane, and that is done in a power plane when you have two or more Vdds in the same plane. In truth, modern electronics would not exist without this capability. First, you have to be sure that the impedance of the Vdds that are on opposite sides of the split is very low (milliohms), so that the power delivery integrity is good for all voltages. The low impedance of each of the Vdds, between each Vdd and the ground plane, is the AC path across the gap. Also, it should be noted that this gap never needs to be wider than 10 mils (0.254mm).
To illustrate the foregoing, Figure 1 is a test PCB with traces in the buried microstrip layer (layer 2) that cross the plane in layer 3.
Figure 1. Test PCB With Traces Crossing Plane Splits
Figure 2 is the cross section of the split plane underneath a trace. Both the outbound and return currents are shown with arrows.
Figure 2. Side View of Trace Crossing a Split Plane with Arrows to Show Current
Note: In the upper left-hand corner of this diagram is a table showing the capacitive reactance of three different size capacitors as a function of frequency. The 1 nF and 10 nF capacitors commonly used for discrete decoupling capacitors, even one at a time, produce a relatively low impedance. When power delivery systems are engineered correctly, a combination of the discrete capacitors and plane capacitance will be used, which results in the impedance at or below 10 milliohms between Vdd and ground from DC to a gigahertz or more. This effectively “shorts” the power planes to the underlying plane at all frequencies of interest. The return current has an AC path around the plane cut and is not visible to the signal.
Figure 3 is a TDR waveform showing that there is no significant degradation as a result of crossing the split. The blue waveform is the signal crossing the plane split. The very small inflection upward in the middle of the waveform is the location of the plane split. This eliminates the worry about signal quality as a result of split planes. In addition, EMI is not an issue of concern. The trace noted above was excited with an RF generator and probed with a near field probe attached to a spectrum analyzer. When the probe was moved back and forth across the split, there was no change in the level of energy that was detected.
Figure 3. TDR Waveform of Signal Crossing Plane Split in Figure 1
Common mode noise: One of the preceding warnings above talks about splitting a plane to reduce common mode noise. Common mode means that there are two items that have something in common. Almost always this is a differential pair. If you are going to have noise, you are going to hope it is common mode. This means the same size noise is in both sides and that the differential pair then ignores that. This is the definition of a ground offset—it is true common mode noise and it has nothing to do with split planes.
Analog and digital sections of a board: Another warning cited above links plane cuts to the analog sections of a board. Splits have to do with the distribution of two power supply voltages in the same plane and not the location of the analog or digital sections of a board.
Similar to other topics of PCB design that are shrouded in misconceptions and false assumptions, the use of plane splits is marked by lots of misinformation and misdirection. When it is understood that plane splits are limited to the distribution of two power supply voltages in the same plane, it becomes much easier to factor plane cuts into the overall system design process and ensure that PCBs will work as designed, the first time.
Discover more about advanced routing and verification of ground and power supply design planes in PCB layout traces with Altium Designer®. Have more questions? Call an expert at Altium.
Ritchey, Lee W. and Zasio, John J., “Right The First Time, A Practical Handbook on High-Speed PCB and System Design, Volume2.”