When to use a ground plane - Page 1
Forum section: electronics / projects

author: mal-c
author_rank: Newbie
timestamp: November 09, 2015, 01:04:11 am
content: Just a general question. If you were designing a PCB, when is it deemed not to use a ground plane. For example, if the board was using gates or micros and 5v logic levels, then I'm guessing that would be fine. If say you were combining 5v logic and constant current LED drivers that used 48v DC would you still use a ground plane. And if you had AC mains at 240v being switched by SSRs that ran from 5v DC logic lines, then I'm assuming you would need to keep the ground plane well away from the AC side of the relays and output terminals.If you have a PIC running between 20mhz and 48Mhz or more, do you need a ground plane to reduce chance of interfearance ?

author: DanielS
author_rank: Frequent Contributor
timestamp: November 09, 2015, 08:37:49 am
content: You need a ground plane whenever you deal with fast rising/falling edges, otherwise all your traces become coupled inductors, crosstalk becomes unmanageable and EMI, both received and emitted, become a nightmare.

author: tggzzz
author_rank: Super Contributor
timestamp: November 09, 2015, 08:56:16 am
content: Quote from: mal-c on November 09, 2015, 01:04:11 amYou have to consider where the currents will flow. As a crude approximation, for low frequency circuits they will follow the path of least resistance, for high frequency circuits they will follow the signal conductor. Low frequency currents will create voltage drops according to V=IR. High frequency currents will create voltage drops according to V=Ldi/dt. For logic circuits the latter are often more significant because although the currents are "small", the time periods are "smaller" - often 10-9s, or less.If you are considering high voltages, e.g. mains, you must also consider physical isolation for safety, and that is a big topic in itself. For example sometimes you see slots milled in boards to increase the distance between different parts of a circuit.FFI, see the many many web pages, application notes, text books and safety standards. There's no way anyone here is going to try an reproduce those!

author: AndyC_772
author_rank: Super Contributor
timestamp: November 09, 2015, 09:11:22 am
content: Use a ground plane unless there's an absolutely compelling reason why the board cannot possibly have one. The same goes for a power plane too.Troubleshooting a board which doesn't work because of grounding problems is time consuming, painful, and more often than not, pointless.You mention "interference", but that's not really the correct word to use. "Interference" would imply some signal external to the board coupling into it somehow, and causing problems. That's not really the issue.If you have no proper power and ground planes, then all your devices' supply current has to flow through a power or ground trace, which is inherently inductive. As a very rough approximation, 1mm of trace has an inductance of about 1nH.Now suppose you have a microcontroller with pins that switch states in 10ns, which is pretty slow. That means pins can toggle at about 50 MHz, and the reactance of 1mm of trace @ 50 MHz is given by X = j2*pi*f*L = 0.3j Ohms. Add that up over, say, 10cm of power and ground traces, and you're up to 30j Ohms in series with your power supply.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 09, 2015, 10:25:19 am
content: Quote from: DanielS on November 09, 2015, 08:37:49 amFixed.The only time you DON'T want ground plane, is if:1. Large clearance (high voltage, isolation, safety?)2. Small capacitance required3. High impedance requiredAlmost all semiconductor circuits work great over ground plane, because the trace impedances are comparable to the circuit impedances (~ 100 ohms), for the most part. And thus there is a minimal excess of stray inductance or capacitance.A high impedance sensor might benefit from the increased clearance or reduced capacitance.Vacuum tube technology tends to benefit, because of the high impedances (>1 kohm) typical there. Indeed, most tube tech wasn't wired on PCB at all, but point-to-point over terminal strips, where the clearance is always high.Tim

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 09, 2015, 11:02:14 am
content: Quote from: AndyC_772 on November 09, 2015, 09:11:22 amBy the way, "planes" don't have to be 100% solid (as would be typical for a multilayer PCB). Fill the top and bottom layers of a 2-sided board, and stitch them liberally to get a solid ground. You can't effectively do both power and ground this way, so you'll have to route power conventionally, with bypasses, but that's perfectly fine.QuoteY'know, I should make an example of this:Years ago, I had built a class D amplifier, which was hand etched, so I made it single sided. It basically didn't work. Remade it with one side ground, no problems! This is the latter:http://seventransistorlabs.com/ClassD1/index.htmlJust imagine that without the top ground.Quote"Interference" isn't a terrible word. There are three factors acting in your circuit:1. Functional. Does it even work, on its own?2. Emissions. Do other things (e.g., sensitive radios) still work while your thing is running?3. Susceptibility. Does your thing still work when other things (e.g., licensed radio transmitters) are running?Lack of ground plane typically fails all three with flying colors!You can address #1 with some help from layout. Back in the dark old days of TTL and 2 layer boards, you'd find pairs of heavy traces, running in rows underneath the chips: power and ground. Their proximity to each other helps reduce supply inductance, but frequent bypass caps are really what does the job.Electromagnetic compatibility (EMC), #2 and #3, are a lot harder to deal with at layout time. If you have to route dense parallel buses (as was the case back then), you don't have room for ground pour. So the distance between a random signal trace and VCC/GND was large, variable, and random. Signal quality was terrible, but switching speed was relatively small too (a few ns), so it wasn't a big deal. And everything was good and settled by the time the next clock pulse arrived (say at a blazing 4.0 MHz!).Everything was built inside metal shielding boxes: necessary to keep all the nasty switching noise inside, and to keep outside radio signals away.For that kind of circuit, unshielded, you can expect a loud din of switching noise, at harmonics of the clock frequency, perhaps peaking in the 100MHz range, and extending noticeably into the 200-500MHz range, probably. Good luck watching TV or listening to the radio while that's going on!As for ground plane construction: if your circuit is low enough density that, say, >80% of board area can be ground pour, on one side or the other (or both), and you've minimized the areas where traces or footprints cross on top and bottom (where there cannot be any ground pour), then the shielding benefit should be quite good. Such a board performs about as well as a 4-layer board with inner VCC/GND layers, and rarely needs additional shielding to pass EMC.QuoteAnd only CD4000 is about that slow! The big concern is today's fast microcontrollers and other digital devices, which have pin drivers comparable to the 74LVC logic family. These switch in less than a nanosecond! At that rate, 10cm looks like a 1/4 wave stub, and will ring at the far end, introducing erroneous clock edges and banging into the input-protection diodes. (Also, the input pins are fast enough to respond to those erroneous edges, too.) Needless to say, supply bypasses need to be very close!Source termination works well for CMOS signals. This is simply placing a resistor in series with the output pin. The aim is to match the output driver impedance to the trace's transmission line impedance. Typical PCB traces are around 100 ohms, so you use a 100 ohm source. CMOS outputs are typically in the 20-100 ohm range, so not much external resistance is needed (22 to 220 ohms being common -- use larger values if you can tolerate it being extra slow).But this only works well when the trace is point-to-point (e.g., MCU to LCD display via long traces, or ribbon cable). If there are multiple input and/or output pins along the trace (a multidrop or star bus -- SPI perhaps?), a wonky waveform will be seen in the middle of the trace (and that's bad if you're sending something important, like an edge sensitive clock signal). For those cases, you should try for a strong source driver, and load termination. But load termination is very wasteful, because it draws DC current. You can compromise by using an R+C terminator, where R == characteristic impedance, and C >= 2.5 * (total trace and pin capacitances). The capacitor saves DC without introducing too much ringing (the effective trace inductance resonates with the capacitor, but is heavily damped by the resistor), but this is still wasteful for high frequencies (f > 1 / (2*pi*R*C)).For high frequencies AND long routes, consider moving to another signaling method, like LVDS, which is necessarily load terminated -- and differential, which will save you some trouble if your routing isn't stellar. (The common mode range is only a few volts, so LVDS is kind of marginal over cables, and impossible over external connections without heavy shielding. Which is why USB and HDMI require fully shielded cables!)(By the way, differential routing is something of a farce: the coupling between traces is weaker than the coupling of each trace to ground. The real goal is to expose each trace to more-or-less the same electromagnetic fields along the route -- it's not so much that they should be routed together for the signal's sake, but to control interference.)Tim

author: DanielS
author_rank: Frequent Contributor
timestamp: November 09, 2015, 04:31:55 pm
content: Quote from: AndyC_772 on November 09, 2015, 09:11:22 amAnd that's when you use local decoupling, as they did in old computers on two layer boards.On many modern BGA chips, CPUs and GPUs in particular, critical decoupling is done on-package, sometimes even on-die.

author: akis
author_rank: Frequent Contributor
timestamp: November 09, 2015, 04:59:33 pm
content: Ground plane is not a panakea for HF applications. For example two traces running in parallel for X mm length, or even one trace on top and the other at the bottom, and you get capacitive coupling and maybe positive feedback or other weird phenomena. The whole PCB has to be designed with that in mind. My work has been at 200KHz / 30W RMS and it takes a while to design a robust PCB that will work time and time again regardless of the variations of components. With Class-D amps (which was mentioned above) I assume things are much harder.

author: AndyC_772
author_rank: Super Contributor
timestamp: November 09, 2015, 05:51:34 pm
content: Quote from: DanielS on November 09, 2015, 04:31:55 pmI'm afraid I don't have time right now to go into why that's far, far from being a solution. No doubt someone will be along soon to fill in the gap.QuoteThis is to do with the inevitable inductance of the package lead frame, and the effect of its impedance at 100's of MHz upwards.

author: Howardlong
author_rank: Super Contributor
timestamp: November 09, 2015, 05:59:59 pm
content: As a general rule, the first thing I do is flood fill ground plane(s) before routing any tracks. When I make my own boards for unit tests, I flood fill both top and bottom layers, but as well as for signal integrity reasons, it's because you use up far less ferric chloride!

author: georges80
author_rank: Frequent Contributor
timestamp: November 09, 2015, 06:43:46 pm
content: On two layer boards, blindly flooding copper everywhere it can flood (as a ground) can cause problems with high current/power/speed switching supply circuits.You can create ground paths that carry high currents that cause the ground voltage to be far from 0V. Those high currents if underneath sense traces can couple noise into the sense circuitry and cause all sorts of operational problems. These problems also exist where there are mixed signal circuits (e.g. in the OP case, microcontroller/digital circuitry on the same PCB as a high power LED driver).Before you try to flood ground, consider how the current will flow and also consider the circuitry/traces above it. Cutting planes to allow high current to flow through the paths you want and not flow in other areas is on possibility. Of course you don't want high speed signals to cross over those cut planes due to impedance mismatches.As with many cases in electronics, the devil is in the details and there isn't "one rule fits all".cheers,george.

author: DanielS
author_rank: Frequent Contributor
timestamp: November 10, 2015, 04:23:28 am
content: Quote from: AndyC_772 on November 09, 2015, 05:51:34 pmI don't need help filling the gaps, I've done some ASIC engineering.But local decoupling of power distributed through H/V-routed power lines is how they used to do it in the early days and it worked fine for computers up to about 15MHz. It may not do anything for signal integrity in/out of the chip but it gets the job done as far as the chip's internal processes are concerned, which is often good enough in many microcontroller or simple logic applications.OP is mentioning a bunch of random things that are more in line with programmable logic controllers and driving LEDs than high speed electronics, not much high speed signal integrity involved there.

author: nfmax
author_rank: Super Contributor
timestamp: November 10, 2015, 08:14:54 am
content: There are two (or maybe two and a half)differentreasons to use a ground plane. A plane may work for one, but not the other, it may even make things worse!Providing a return path for high frequency currents. In this case the current will flow only in that part of the ground plane adjacent to/beneath the signal conductor. This minimises the area of the current loop, thereby also minimising the energy stored in the magnetic field, or equivalently the circuit inductance. If you know exactly where the signal conductor is,the rest of the ground plane could be removed, without changing the inductance, as it is not carrying any current.of course, it is rare that you actually know with certainty where the signal currents flow. Least area/inductance also means least magnetic coupling into victim circuits, also least susceptibility to magnetic coupling.providing electrostatic shielding between circuits. The idea is to minimise the capacitance between circuit nodes by placing grounded copper between them (or as between as can be got). This also increases the capacitance to ground, and if the circuit node carries fast signals this will cause current to flow. These currents need return paths as described in point 1, but this is a secondary issue. For some circuit nodes, increased capacitance to ground can be a disaster. The input of a transimpedance amplifier is an example. You need to keep the ground plane away from these points: if shielding is needed (and it usually is) you generally end up with some kind of metal box, of dimensions large compared to the physical circuit, of which a ground plane may form partThe 'half' case is where the ground plane forms part of a controlled impedance transmission line, in which case just follow the design rules. But remember that it may end up acting as a current return path for some unrelated signal current, or adding possibly unwanted capacitance elsewhere.To sum up, think circuits, think signals!

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 10, 2015, 12:46:18 pm
content: Both can be rolled up succinctly into one rule: use the characteristic impedance that matters.Mind that, every single possible time someone refers to stray inductance or capacitance, whether they think about it this way or not: what they actually mean is, the inductive or capacitive low frequency equivalent, of the transmission line impedance and length, which are characteristic of that route.So when you suggest a shield box instead of direct (on-PCB) grounding, you're really just increasing the height distance to the ground plane. Which increases the impedance, reducing the capacitance equivalent, and increasing the inductance equivalent.Characteristic impedances of perhaps 200-300 ohms are about the most to expect on a PCB (say for CPW traces with 12mm clearance), and impedances up to maybe 1kohm for free wiring in a chassis, or lines in space. (Of course, lines in space are limited by radiation resistance, i.e., your transmission line acts like an antenna instead, at suitable frequencies.)BTW, very wide parallel traces on a PCB can get pretty low impedances (~10 ohms), which can be of great use around switching power supplies (say, where the inverter is switching a load of about Vsupply / Ipeak ~= 10 ohms).Tim