I took a class many years ago, where they talked about creating separate power and ground planes for the analog and digital circuitry on a board. Of course, the ground planes would be joined at one location, typically under the chip that had both analog and digital signals, like an ADC or DAC.
The high speed digital signals would be routed anywhere other than over the analog ground planes, of course. Some people are telling me this is a bad idea, as if I have totally separate ground planes.
Almost always best is one solid ground plane for everything, bolted to the metal case through every available spacer and bracket and connector shell. We standardize on layer 2 for the ground plane, and occasioanlly also layer 5 (of 6) mostly to keep the copper balanced when we don't need a bunch of power planes..
Handle any microvolt ground loops properly of course.
There's no reason for any two grounds to be at different potentials.
The IC people think *their* single chip is the center of the universe, and that the two system grounds should only meet under their single chip.
Hmmm... Why would two ground planes be at different potentials if they are connected? Perhaps you missed where I said, "joined at one location".
The idea is that some circuitry, such as a switching power converter or a power hungry IC, puts large currents in the ground plane, which do not limit themselves to the immediate area under that circuit.
Connecting the two ground planes at one spot, limits the impact of these currents to the digital plane.
Of course, there is always more to a design than one such detail. This still requires the elimination of ground loops from other ground connections, such as off board.
Just think currents. I do split planes when I have currents I don't want to see go into sensitive analog areas - e.g. DC-DC converters can be nicely contained within themselves and connect to the main GND plane where you want their output current to go through.
Basically the rule is do it with reason, if you don't know why you split a plane just don't, luck will likely be on your side if you don't. And of course make sure not to route fast signals across splits, the return current flows through the plane just underneath the trace; cut that and you have a discontinuity, potentially a killer one.
There is some irony that Lee Ritchey is quoted as saying splitting of planes is always bad. That's who said it should be considered, in the class he taught some years ago.
One of the things in Lee's class that impressed me, was that nearly everything he taught he analyzed the theory, simulated and finally built boards to test the idea. That's very powerful evidence.
Yeah, people warn me about the fast digital signals all the time. I don't have fast digital signals in the analog circuits, only the ADC which is where the planes are split.
One common connection location won't force two planes to be equipotential, AC or DC.
I work with one giant organization whose religion includes single-point grounding not only for multiple boards in a box, but for entire building-sized systems. That gets absurd. Sometimes their stuff works, typically after six iterations and three or four years.
A dipole voltage in a plane falls off fast with distance, 3rd power as I recall. And it's not hard to keep switcher currents from getting into a ground plane.
How do you pick the "one spot" ?
The planes are capacitively coupled anyhow. And some power pours would be bypassed to one plane, some to the other. Nightmare.
Handle low-level signals carefully, differentially if required.
Ground planes with differential AC voltage between them cause all sorts of problems.
The board I just posted the pic of has two reference planes, hard ground and N, the 3-phase floating neutral. They can't be connected but are mightily bypassed to one another. Some long, fast microstrip logic signals cross the "reference plane" boundary.
"But, perhaps one of the most important takeaways is that you should NEVER, EVER split ground planes."
That's all you need to read.
I have a few times cut a C shape into a ground plane to create a peninsula that is mostly free of ground loop potentials. I tucked some nanovolt opamp circuits there. But that's not a separate plane and the open side of the C only adds micro-ohms to the peninsula from the overall plane.
There are lots of reasons to have separate ground planes. The classic is to separate digital from analog circuitry, as digital can be pretty noisy, and analog can interpret ground bounce as a valid input.
Another reason to have multiple analog ground planes is a Dual Mixer Time Difference instrument, where the beatnote between ~ 10 MHz carriers is one to ten Hertz, so the "just underneath the trace" fills the entire ground plane uniformly. The usual dodge is to transformer-couple the two RF carriers, generating the sinewave beatnote with a double-balanced diode-ring mixer on the floating ground plane, and transmit the beatnote signal differentially over shielded twisted pair cable to where it will be used, or to square the beatnote sinewave and send that by shielded twisted pair cable.
The classic reference is "Noise Reduction Techniques in Electronic Systems", 2nd Edition, by Henry W. Ott, Wiley 1988, 448 pages.
.
formatting link
Also covered in "Electromagnetic Compatibility Engineering First Edition", also by Ott, Wiley 2009, 880 pages.
I've TDR tested microstrips that cross ground splits or cuts, or transition from running over a ground to over a power pour. At 30 pS resolution, the crossing is generally invisible.
In a multilayer board, plane-plane capacitance is high so a trace doesn't notice changing reference planes. AC-wise, the board is a monolithic equipotential brick.
Hard right angles are usually TDR invisible too, or so small a discontinuity that few signals would care.
How close to the discontinued plane was the next one the signal would have gone through?
Well unless the alternate plane is far enough (say 1mm). But I guess you are talking multiple layers, 0.1mm or so separation, which I can believe (have not done that sort of test).
Hard right angles sound more like folklore, I can understand how some signals could care (not experienced any of it though).
I am not an RF person, I mostly think time domain so I am not sure I understand all of what you say. That very low frequency thing must be quite juicy in order to make a difference, or (and?) you must have some very sensitive stuff to be affected.
I tried one case with a 50 ohm microstrip, about 50 mils wide, crossing a cut in the layer-2 ground plane about 20 mils wide. The trace, looking down, sees a slightly higher capacitance where there is a gap in the metal and epoxy is visible through that gap. As I recall, the discontinuity was questionally visible among the usual trace woopie-doos.
Of course both sides of the cut were equipotential, and that plane was parallel to another unbroken plane, so plane-plane capacitances glues everything together.
There could in theory be a slotline resonance at a slit in a ground plane, but I've never seen any evidence of that in a TDR.
We often have a trace swap its "reference" between different pour pour regions, and that seems to always work.
The "return current" concept usually makes no sense. Just keep all the planes parallel and reasonably bypassed, and traces will be happy riding over any of them.
Our most common board is 6 layers with roughly equal gaps between planes, of maybe a lottle closer between grounds and power planes.
We try to keep the stack symmetric and pours all over planes to minimize board warping.
The classic Motorola ECL Handbook cautioned about right angles, when ECL was still 1 ns stuff at best.
Few signals are fast enough to care about even 1"-scale abberations.
Our fastest signals are in the 40 ps range, and vias are the worst features. Best to have none in the critical signal paths.
The Dual Mixer Time Difference (DMTD) instruments are used to measure low frequency instability of clock oscillators, for Allan Deviation (ADEV) levels below 10^-14. So it does see all manner of stuff.
I don't expect to hear from you. You have often said I'm in your killfile list. Please return me there if you don't like what I post.
That's only an issue if there is significant current flowing through the connection. Why would there be significant current flowing from the sensitive analog circuits to the digital circuits. You have to do more than just connect the two areas at one point. You have to pay attention to the entire grounding plan. But there's nothing inherently bad about making such a connection to keep digital and switcher currents out of the analog circuits.
You mean like isolating the ground plane under the switcher circuit, connected at one point to the rest of the ground plane? I think that might just work. Thanks for recommending it.
For an ADC circuit, the ADC is typically a good point. The high speed digital signals get a digital ground plane, and the analog circuit gets an analog plane, with very little voltage between the two, not that this matters. What matters is keeping currents out of the analog plane, so there isn't digital noise in the analog plane, showing up in the analog signals.
LOL How would two separated areas on a ground layer, be capacitively coupled??? I don't know what you are talking about here.
Yes, all the power rails have their own power planes. They capacitively couple to the appropriate ground plane area.
Or... just don't inject noise from the digital circuits.
Yes, that would be terrible. That's why they need to be connected. But the voltage between the ground plane areas is not so important, as long as it is within the tolerance of the devices spanning the two plane areas. I can't think of a reason why, a connection with very little current flowing through it, would produce much of a voltage offset. Can you? I suppose you have some experience with this.
My designs are always pretty simple, because I try hard to not let them get difficult, like designing differential circuits to minimize the impact of noise that I didn't need to introduce in the first place.
I don't split ground planes. I keep them separate, tied at one point.
Ah, so you agree with the split, but connected plane concept! Thanks. I appreciate the support. Now, we just need to work out how much connectivity is required.
How much current flowed between the two ground plane areas?
The right angle trace effect is real, but people often use the wrong explanation, such as "the signal flying off the end of the wire, rather than making the turn" (I've actually had someone tell me that with a straight face). The simple fact is that the corner represents a lumped capacitance in the trace. Often, that is of no consequence. Sometimes it is of consequence. Depends on all the many details.
Rounding the corner makes the lumped capacitance a much, much lower value to the point of vanishing. Making it a pair of 45 degree bends does a pretty good job too.
In the case of complex RF circuits, the _ARRL Handbook_ advises against single point grounding. Instead it suggests breaking a unit into modules, each with its own full copper ground plane, connected by coax to other modules. Elecraft
formatting link
follows this approach. And also enjoys wildly successful products.
In industrial control systems you often use a 6 wire system, three phases (P1, P2, P3), Neutral (N) Protective Earth (PE) and Technical/Functional Earth (TE/FE) to carry different kinds of currents and avoid harmful voltage drops.
The N is polluted by unbalanced single phase loads, especially those with rectifiers. The N potential in different mains sockets on a site can be several volts from each other. It is mot a good idea having some kind of signal ground connection between equipment in two mains sockets (especially in TN-C systems).
Originally he PE connection was intended to only carry the ground fault current and reliably blow the fuse. Nowadays the mains EMC filter capacitors are connected to the PE network, polluting the PE network with all kinds of high frequency currents, causing interference voltages between different equipment (even in TN-S).
TE/FE network is supposed not to carry any current and thus no voltage differences between equipment and hence it can be as a reference for unbalanced measurement.
Of course this requires that the N, PE and TE/FE networks are kept separate within the whole industrial site and only connect together the main busbars together at a single point with heavy jumpers.The jumpers can be removed during commissioning to verify that N, PE and TE/FE networks are really separate on the whole site.
Most problems with this system is when local installers note that an equipment has separate N, PE and TE/FE connections that they are "at the sane" potential and wire then together at the equipment and connect all to N. :-( You really have to watch what these local installers are doing.
Fortunately most industrial analog measurements are still 4-20 mA current loop, which are more or less optoisolated and do not need a separate ground reference. Signals can be transferred for hundreds of meters. Serial connections are often optoisolated, Ethernet uses standard magnetics and optical fibers are used especially in high interference environments.
One should remember that there is NOT a universal ground potential but all kinds of (very) local reference potentials at ,ore or less different potentials..
ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here.
All logos and trade names are the property of their respective owners.