[LIVE] How to Achieve Proper Grounding - Rick Hartley - Expert Live Training (US)

hi everybody welcome to the session on proper grounding in pc boards just a couple of things before we get started first I want to apologize for the way I sound I have a cold I'm gonna try really hard not to cough but if I do please understand secondly if you have questions you can administer them or send them through the YouTube chat and we will try to address as many of them as we can at the end of the session and lastly those of you who are interested in more educational material can find things on al tiems youtube channel so please go there there's stuff building up daily they're constantly providing new material like this class we're gonna do today and so on and with all that in mind let's get started where's no here we go okay talking about grounding the term ground of course refers to the earth what happened the term ground sorry we had a little technical difficulty there the term ground refers to the earth we first used the earth about 300 years ago to divert lightning away from buildings lightning naturally couples between the clouds and the earth anyway because that's the earth is where it wants to couple to and it went away again what were naturally once - couple - so by putting a nice long rod on top of buildings and a big hefty wire going down the building to a stake in the earth it allowed us to divert lightning to keep buildings from catching on fire and burning down so this was one of the first uses and is a perfect use of the earth as a return path for energy it was quickly learned from that that we could use the earth for other things as a return path for example in the early days of telegraphy back in the 1830s and 1840s when they strung telegraph lines they put up two wires because generally you need a forward and a return path in a transmission line to get energy to move while they soon realize that if they connected transceivers which were sending and receiving energy between points along the telegraph lines if they connected the internal circuitry of the transceivers to the chassis that was containing it and then it secured that's very properly to the earth through a nice concrete pad to keep it from blowing away or or heaving from frost they had such a strong attachment to the earth itself that they could eliminate one of the wires they didn't need the quote-unquote ground wire as it was called they could literally use the ground as a return path now I'm sure everyone listening to this is well aware that the earth is not a great return path it is an adequate return path under the right circumstances in a situation like telegraphy where you have a very strong signal at a relatively low frequency earth can be a nice return path to allow things to function for example one of the things we use earth for today with most electronic circuitry is to attach the third wire of the AC line coming in in the United States Europe and various other parts of the world it's either green or yellow or yellow green and that third wire is supposed to be attached from the chassis of the system to the earth for what purpose safety it's all about safety if the phase line of the AC coming in were too short to the case you want to be able for that that ground that line going to ground to cause a high enough current so that you'll blow a breaker or a fuse because if you didn't have that third wire going to ground and that phase line attached or connected if you will to the chassis and someone walked up and touched the chassis because it would send a current through their heart and could treat major problems so these are the kinds of things that we do today the reason today that we attach things to the earth is safety its safety is its only value and it's only role it has nothing what so ever to ooh was passing EMI testing and that third wire carries no value with respect to EMI the reality is the third wire doesn't help with the mi in fact if we don't attach the third wire correctly the third wire will become the EMI problem when we hook up that third wire you generally have to put some inductance in the wire so that you have to put some inductance in the wire so that it won't transmit high frequency energy back down the wire toward the earth because it's such a high impedance from the box to the earth at high frequencies along that wire that it would behave as an antenna in would cause EMI problems and a lot of people I've met over the years think oh we have to attach this or that to the earth to pass EMI testing no you don't your cellphone isn't attached to the earth the aircraft avionics that I worked on years ago there was no wire coming off the electronics and going down to the earth somewhere to allow this stuff to pass EMI testing it all past EMI testing without ever attaching in any form to the earth we attach to the earth for safety and for safety only speaking of that many people I've talked to refer to the chassis of a system the metal chassis as earth ground or chassis ground frankly it is neither even when that chassis is attached to the earth for safety purposes it is nothing more than a metal chassis its function is to behave as a Faraday cage the Faraday cage is intended to keep the fields that are in the unit inside and keep outside fields from coming into the unit the whole concept of the Faraday cage is to shield everything so that our intended fields stay in an unintended fields stay out someone asked a question before we even started that I'm going to just answer right now the question was how how should you attach the shield on a wire on a cable should it be attached to the internal ground it should it should it be attached to the earth and I'm pretty sure what the person meant by the term earth was should it be attached to the chassis and the answer is it should always be attached to the chassis in fact you want a connector that gives as much as possible a 360 degree attachment of the shape of the shield to the chassis reason being that the shield is simply a continuation of the Faraday cage when you send energy down a pair of lines from the board into the cable the shield simply acts as a continuation of the Faraday cage to continue to shield to keep intended fields in an unintended fields out that's the whole concept of shielding you're not grounding the shield you're attaching it to the chassis to continue the Faraday cage food-for-thought ground when PC boards is often considered a region of zero volt potential with zero resistance and zero impedance and that is simply not true and I hope everybody watching this understands that ground is not zero volts it's close to zero volts but it isn't a perfect zero volts when you send energy down transmission lines and you get current in ground that current causes a voltage drop and that voltage drop means that from one point to another the ground potential difference is never exactly zero volts close but not zero volts that statement is only true is only close to true at DC where it's zero resistance and zero impedance as you go up in frequency ground is anything but zero volts and zero impedance ground is often thought of and I've heard many engineers say this and this is a statement that just drives me nuts ground is often thought of as a place to attach components to bleed off or filter noise as if ground is a sinkhole that's used to eliminate noise masseur ckets that concept comes from the belief that it's like the water analogy we've all heard of the water analogy send water through pipes and lava blonde that's similar to electrical energy and it is and we'll talk about why in a short while but the way that the analogies taught we bring water through pipes to a sink we use it for stuff we put it in the drain and goes back to where it came from and that's they say is analogous to ground that's not at all what ground is ground in a circuit board has nothing to do or has any similarity at all to the drain of a sink carrying water away from its usage point it has nothing to do with it and we're gonna discuss this further as we go oh it didn't advance for a second sorry sorry another technical difficulties the idiot behind the wheel that would be me of course the concept and belief that many people have about ground simply doesn't exist and frankly until about 20 years ago I was one of those idiots that had a ridiculous belief about what ground was and we're gonna talk about that in just a moment sixteen years ago I met a gentleman by the name of Ralph Morrison and the man changed my life he came to one of my classes once and attended a full-day class and at the end of the session he came up to me and he said Rick I liked a lot of what you presented today can we have dinner and I thought sure this is a great plan I'd love to have dinner with Ralph Morrison so we went to dinner and over dinner he said I truly did like much of what you taught you have some great ideas some good concepts that you're teaching and they're gonna be helpful to people however you're thinking about things incorrectly and I said oh and he said to ask me the question what is energy and I said well I remembered back to my days in college physics and I gave him some answer that was similar to what you see on the screen that it's the property of matter that manifests itself in the capacity to perform work motion interaction of molecules and I don't know that I gave him that answer but something similar to that and he said yeah and he nodded and he said yeah and as you know energy exists in many forms it exists as mechanical energy light heat sound electrical etc energy is never destroyed it's never created it's converted from one form to another we move energy from a quiescent state to a state in motion we take it back to a stable state but we but we don't create or destroy energy speaking of different types of energy something I hope all of you know is that light energy and electrical energy are exactly the same thing they are absolutely precisely the same form of energy and a lot of people are listening to this thinking wait a minute light that lights the room an electrical energy that conducts down wires are the same thing the answer is yes the only difference between them is frequency light is about about a million times higher frequency than electrical energy at 500 megahertz there other than that they are identical and you'll see what I mean in just a moment so then Ralph asked me where's the energy in the circuit is it in the voltage or is it in the current and I thought about this for a minute and I thought you know when you when you do power delivery to an IC to generate energy in the IC to drive transmission lines the voltage is relatively stable it's relatively fixed and the currents the current coming in and out changed rapidly in frequency and amplitude so I thought well it must be the current clearly the energy is in the current so I said that to Ralph and Ralph smiled at me and he said actually Rick it's neither he said I'm just messing with you and I said oh neither and he said that's correct there is no energy in voltage or current well that's not what I was taught in college and he went on to say the energy is not in the voltage or current it's in the fields it's in the field better known as the electric and the magnetic field and he then asked me where do the fields travel where are they located in a circuit board is it in the traces or is it in the planes of the board and I thought about this for a minute and really was really scratching my head at this point in time because frankly I didn't have a clue and Ralph looked at me and smiled and he said sorry Rick I'm messing with you again it's neither the energy doesn't travel in in the copper at all the energy travels in the space between the traces and the planes the energy travels in the dielectric in an fr4 circuit board the energy travels in the plastic and fiberglass of the board and no energy travels in the copper now I was really scratching my head at this point but as it started to sink into my head I suddenly began to realize why all the problems I had ever seen why circuit a interfered with sir could be or why energy coupled from one place to another it all came down to the fact that we didn't take good care of the space between the traces and the return path a perfect example my friend Dan beaker has created a song to the tune of Meghan Trainor's it's all about the bass and he sings it's all about the space it's all about the space between the copper features the energy travels in the plastic the energy and the transmission of and is called a wave an electromagnetic wave the traces or trace and plane that make up the transmission line steer the energy from point A to point B these copper elements act as a waveguide so as the trace travels through the circuit board above a plane the energy travels in the space between the trace and plane as the trace travels across the board why does the energy follow a trace because it's the path of lowest impedance could you launch the energy into the dielectric without traces yes you could we do it in air all the time we launch signals into air for radio broadcast and television broadcast and for Wi-Fi and Bluetooth and all sorts of other things that are wireless communication this is simply launching the energy into the dielectric the advantage of having traces on boards is if we launch the energy into the dielectric between a trace and a plane that offers a low impedance path so we can guide the energy the the copper features act as a waveguide waveguide yeah the RF people I work with they have wave guides yes and so there's every person designing digital circuit boards I don't care if you're designing power supplies or what you are doing every forward path and turn path that constitutes a transmission line forms a waveguide and it guides that energy from point A to point B what is this it's a wave guide this is a tubular wave guide made out of metal if you apply and this isn't how you would do it but if you applied energy to that tube and that energy had a wavelength whose half wave length was equal to the distance X you would get a standing wave inside that tube at one and only one frequency the frequency whose wavelength was two times X that's the frequency that would transmit down that tube it would flow through the air of the tube creating current flow in the side walls and top and bottom of the tube and creating a voltage across the structures of that tube the fields do create voltage and current but they do not carry the energy the I mean the the fields do carry the energy the voltage and current do not anyway this is a waveguide it's designed to conduct one frequency of energy and block or shunt all other frequencies what is this it's also a waveguide it's a substrate integrated waveguide designed into circuit board material so that the circuit board material will behave precisely as this metal waveguide behaves it's with one exception because the dielectric constant of the board is higher than the decay of air it will travel at a slower speed energy for example in fr4 travels at approximately half the speed of light whereas energy and air travels at close to the speed of light so this is the same thing as the tubular waveguide on the previous page notice that this waveguide is fed by a microstrip trace a trace on layer one routed above a plane on layer two the energy in the waveguide is shown on the right-hand side here the energy and the microstrip is shown on the left-hand side of this blue strip and you can see that they look remarkably the same the the microstrip traces energy spreads out more it sits cysts of more than one frequency it's it's different in that sense but other than that they're just bursts of energy that travel in waves through the Micra through the micro stripped trace and then are simply fed into the waveguide the way you feed a substrate integrated waveguide is exactly what they've shown here with a micro strip the bottom line is both the micro strip and the siw are wave guides both guide the wave through the dielectric from point A to point B a transmission line is any pair of it's it's a transmission line or waveguide they're both the same as any pair of conductors used to move energy from point A to point B there's a voltage across the copper of the transmission line and there's current in the copper the energy remember is in the fields traveling in the dielectric a lot of Engineers I've met will say to me yeah Rick I know house circuits when you launch energy into a circuit the current travels down the trace to the load and then comes back up the ground trace back to the driver no that's not how it works the energy is launched into the circuit in the form of a wave consisting of fields the fields create a voltage across both copper features at the same time and they create a forward and a return current in both copper features simultaneously so the return current is formed at the exact same time the forward current is formed in a transmission line it's not a down and back kind of thing it's a simultaneous event if we look at this transmission line that you see here if we lost energy into it and it was halfway down the line that field at some point if we look at it at the halfway point there will be voltage across the copper halfway down the line there will be current in both sides of the line halfway down the line and at the end that the other half nearest the load there will be no voltage there'll be no current there'll be no energy because it hasn't gotten there yet that's how transmission lines actually work how we take care of the return side the ground as we want to call it side of this line and makes a big difference as to how things will perform this is a strip line transmission line centered strip line with a trace centered between a pair of planes they can be to ground planes power in the ground plane we'll talk about that in this short while but this simply centered between a pair of planes as we launch energy into this transmission line the first thing that appears is the electric field it's coupled from the trace to the planes and the energy in that field excites the electrons in the copper the electrons in the atoms of copper and those electrons start to move causing current flow in the copper of the planes and in the copper of the trace the reaction to that is to form a magnetic field which surrounds the trace and is sandwiched between the trace and the planes notice that all of the energy is in that space between the trace and the planes also notice that it spreads out a little bit it isn't contained directly under the trace to the plane there is a spreading of energy and that spreading of energy is what causes crosstalk and other forms of interference if we get things too close to one another so that's the reality of that the fields do spread a little but for the most part they stay contained in that space these are the fields of an outer layer transmission line a trace routed above a ground plane and layer two of a board the fields as you can see expand more than the fields do on an inner layer and this expansion of fields does cause some radiation from the surface the outer surface of the board and this is a problem in some cases this by itself will never cause you to fail the mi but it will exacerbate an existing problem when it when when you have one but the fields do expand more in outer layers crosstalk is worse on outer layers all of the things that cause interference are greater on outer layers because the outer layer fields expand more imagine that we have a circuit board looking at it from the side that is a two layer board with a ground plane on layer two signals and power routed on layer one and poured copper in between all the signals and power to poured copper that's attached with lots of vias to the ground plate this is how the microwave world the RF world designs what are called microstrip boards and notice I said routed power there is no reason in an analog circuit to ever use a power plane you do not need power planes in analog circuits this can be the fodder for another talk sometime maybe we can discuss that in a future discussion but the reality is in this board you have routed signals routed power poured ground copper on top and a ground plane on the bottom let's rotate this 90 degrees look down on it from the top when I work with an engineer for the first time I will often draw a picture of this on their whiteboard and ask the question of them where's the return current from this signal that's routed around the outer perimeter of the board notice that these two ICS are attached to the ground plane in to one location each they each have a ground pin next to the signal pin at the ground plane layer and very often engineer 75 to 80% of them will say to me oh the return current is directly across the plane the short path between the two ground attachment points now if this were DC energy if this were purely a power supply output supplying DC energy that wasn't changing State at all yes that's where the return current would be it would take the short quick path directly across the plane but it wouldn't just take the short path it would spread out DC currents spread out to a very wide swath as well and the swath would be about as wide as it is long so it would effectively form a square why because it would take the path of least resistance at DC and resistance is a per square measurement therefore the currents path would be a basically square structure if you could change the frequency of the output of this and started raising it from DC to a few hundred cycle can you hear me now yes okay so it was that oh go ahead and just stick it on my belt somewhere it doesn't matter long as the logo wart hanging off my ass I don't care oh sorry sorry okay a little technical difficulty there sorry we lost power to the to the audio source anyway going back to where I was at low frequencies the current would flow in a shorter path between the two ground pens of the I see as you go up in frequency and and certainly by the time you're out of the audio range by the time you're above 20 kilohertz all of the return current and this signal will travel directly below the trace all the way back from the driver all the way to the receiver remember the forward return current are being created simultaneously and these arrows indicate that one of the current flow is the far recurrent and the trace the other current flow is in the ground plane directly below that and that's what happens at higher frequencies is you get the current flow directly below the trace why does the current flow directly below the trace because energy takes the path always this isn't 100% of the time true statement energy always takes the path of lowest impedance impedance is essentially the path of lowest inductance and greatest capacitive coupling meaning that what let's examine Tewa let's examine for just a moment what inductance and capacitance our inductance is an impedance to change in current flow caused by the mass or the inertia of the magnetic field meaning what if I have two traces that are side-by-side on a circuit board and one of them is the forward trace of a circuit and the other is the ground trace and they're separated by two three four inches which would be fifty to a hundred millimeters at that kind of spacing the fields are going to exist in this large space between them and the magnetic field is going to be huge and as a result of its large size it will have high inertia which means it will create a high impedance to current change in the circuit and that is the definition of what drives up inductance large volume of fields large volume of magnetic field large high high inductance so how can we reduce the inductance while I was taught in college you can make bigger wires and the inductance will go down and to a degree that is true but only to a degree there's a point where it really isn't beneficial for example if I wanted to have the inductance of those wires I would have to increase their width assuming I kept them separated by three or four inches I would have to increase their width from let's say a 10 mil trace out to a half inch wide trace just to have the inductance that's not exactly productive what else can we do to lower the inductance well instead of having the trace as far apart bring them close together on the same layer now you have a small volume of space for the magnetic fields and the end result is you'll have small field small inertia low inductance the best of all put one directly above the other in other words have the forward trace and the return trace directly over one another in the board stack route everything above for example a ground plane and keep the dielectric space small and you will minimize inductance in structures capacitance is the same way remember we said impedance is L over C so we want low inductance high capacitance you keep capacitance high by keeping traces routed over a return path or extremely close to their return path it's all about proximity I have people say to me all the time I want low inductance in power vias connecting decoupling capacitors to the planes do I do that by creating large vias the answer is no you don't do that by creating large vias you do that by bringing the vias very close together you put them at the side of the capacitor with short attachments to the pad of the capacitor or maybe even have them in the pad of the capacitor if it's a small cap so the vias can be very close together size counts but proximity matters much much more and that's the key to controlling and lowering impedance but by lowering capacitance or inductance in raising capacitance in circuits okay then why did the low frequency current spread out well the answer is actually quite complex and it gets into a thing called skin effect which I if I had two more hours than I have I'm not sure I could explain the thing in that amount of time so let's take the easy way out let's look at the formula for impedance I said that it's the square root of L over C it's actually a little more complex than that impedance is the square root of resistance plus a frequency factor time in depth times inductance that's the numerator of the equation and in that numerator you have both resistance and inductance impacting the the for the impedance if you will of the transmission line at DC what is the impedance due to inductance well at DC frequency goes to zero so J Omega goes to 0 which means J Omega times L goes to zero so the only thing in the numerator at DC is the resistance of copper and that's why a DC current or energy follows the path of lowest resistance as you start to go up in frequency and you have some frequency factor times inductance inductance becomes more and more of a factor in determining the behavior of the fields so at DC and really low frequencies energy for the most part follows the path of least resistance at higher frequencies it will travel under the trace back to the driver here's a simple experiment you can run to prove that in your labs just hook up a 2 meter piece of coax which is about six and a half feet of coax and loop it back around so the ends of the coax are near one another separated by two three four inches and couple the shield's together with a two three four inch piece of wire and attach a signal generator at one end of the coax and a load resistor at the other do a very basic quick calculation how much current are we gonna get based on say five volts and a 10k resistor we're going to get X amount of current put a current loop around that short piece of wire turn this signal generator on to a DC level and push energy through the coax and what you're gonna find at DC all of the return current are 99.99% of the return current will be in that short wire that spans across the opening between the coax if you start to turn up frequency by a couple hundred cycles you're gonna have less current in the short wire and by a few hundred cycles more you're going to have much less and by the time you get into the kilohertz region you're gonna have a lot less current in the short wire and much more of it will be in the jacket surrounding the coax in other words the energy will be taking the six and a half foot path and not the three inch path even though the six and a half foot path is thirty or forty times longer it will be the path of lowest inductance and greatest capacitive coupling and for that reason the energy will take that path at higher frequencies by the time you get to one megahertz there will be zero current in the short wire do you operate above a megahertz are you doing digital designs everything you design is above a megahertz even if your clock frequency is one cycle a day because frequency is related not to clock frequency it's related to rise time rise time determines the frequency of digital circuits rise times today in most ICS are anywhere from 300 to 700 picoseconds which means the digital energy that exists in a rising or falling edge is pushing a gigahertz in all digital circuits the only exception to that would be low-end microcontrollers which are operating down in the 100 to 300 megahertz region but beyond microcontrollers everything is in the hundreds of men Hertz and are you above a megahertz yes you are absolutely this is a graph created by dr. Todd huming of Clemson University that plots the current flow in that short piece of wire based on frequency and you can see that beyond a hundred kilohertz there's virtually no current in that wire beyond a megahertz there is ZERO current in that wire energy takes the path of lowest impedance and at high frequencies that's the path directly under the trace this is a circuit board from 1984 it was part of a robot and it was a 2 layer board we routed the traces on the top and the x-direction as well as power and ground on the top of the board was routed in the x-direction and traces and power and ground on the bottom were routed in the y-direction every place where power crossed power we attached him together with a via every place were ground crossed over ground we attached him with a via and we created a grid work of power and ground to help drive these ICS because even by 1984 we had reached the point where just having a power and ground route wandering around the board wasn't good enough we couldn't make boards work if we didn't distribute power well even by 1984 there's a trace on here that there's an arrow pointing to the trace in 1984 the energy in that trace in fields would have spread out across this entire dielectric space that you see in this picture and the fields would have coupled from that trace to the power rail which is the rail routed above the eye sees and to the ground rail which is the rail routed below the eye sees and most of the return current from that line would have been in the power and ground rail because their size and the frequency of 1984 would have mandated that's how it would have behaved we could get away with this kind of board design in 1984 we can't get away with this type of board design today if we look at frequencies of today's speeds if we design the same board today and put a 500 picosecond rising signal into this line where would the return current be and the answer is none of it would be in the power or ground rails all of it would be in the traces next to the signal that that are routed near it so as you watch that signal route between ICS all of the fields all of the return energy would be in the traces on either side of it which means they would all use each other as a return path and in today's speeds this probably wouldn't work so be aware there are people today still trying to do this if I have a pair of wires a twisted wire pair and I launched energy into this regardless of frequency we know where the forward path is and we know where the return path is what if I add a second ground wire then what happens the audio range I'm gonna get well let's let's go all the way back to DC if this was a DC circuit I would get roughly equal current in all three of the ground lines the one the negative wire that's twisted with the positive wire and the other two ground wires would all have about the same current flow in them assuming they're the same gauge wire and roughly the same length as we go up in frequency we would get less energy flowing in the bottom ground wire and there's a point where energy would stop flowing in that ground wire and then we would eventually get no current flowing in the second ground wire the first one we showed and at some point in the audio range all of the return current would end up in the twisted wire pair we would have two ground loops attached to this but it wouldn't do anything because frequency is high enough that it would ignore the additional return path energy takes the path of lowest impedance and above the audio range that path is the path of the twisted wire pair or the path directly under the trace on the board back in my early design days we used to have to route sometimes ground under low frequency analog signals as we routed them under the board not using a ground plane using a wide ground route directly below traces in order to contain fields because low frequency energy fields tend to spread if you put a ground plane at really low frequencies in the board so be cognizant of that and think about that when you're designing but if you're doing high frequency stuff the energy will self channel you don't need to channel it if that weren't true ground planes wouldn't work a ground plane is potentially a million path for current to flow but it takes one path in one path only because at high frequencies that's how circuits behave here's an example of circuits let's talk about EMI for a moment there's a gentleman by the name of Professor Wu he's a doctor from the National Taiwan University who presented this material at an I Triple E EMC symposium many years ago in the United States and he brought this slide up on the screen and asked the question of the group we have four circuit boards here they're note the large grey area underneath figure a for example is a ground plane on layer 2 of a board the the the crosshatch line that's sitting above to display here he has four of them one has a solid ground plane figure two has a ground plane with a notch in it figures three and four are cross-hatched copper planes think about what we just said a moment ago at higher frequencies above audio returned current takes the path directly under the trace so if that's the case figure three even though it is a cross-hatched plane has a nice wide patch of copper directly below the trace exactly the way figure one does so if you looked at the EMI signatures of these four circuits you would pretty much expect figure one and figure three to have about the same overall EMI signature what about figures two and four well obviously they're both routed above openings in the return plane figure four is routed above a bunch of holes in the plane and figure two is routed above a notch in the plane a split in the ground plain if you will so the question is which of these is has the least EMI in which has the most well I think from what I just said it's pretty obvious that one in three will have the lowest EMI signatures and they'll be relatively similar in fact here's an here's what one and three look like this is the EMI output measured coming off the board of those two lines as they are seen by an antenna in both the horizontal and vertical direction figure two and figure four are another matter when dr. Wu asked the room full of Engineers which is going to be worse a lot of them said figure two and a very large number of them also said figure four because they weren't sure this is the gray line is figure four the one with the crosshatch plane and the trace routing across the openings in the plane look at figure two the one routed above the slot in the ground plane depending on frequency it's 20 to 30 DB worse than one and three twenty to thirty DB greater EMI signature then the traces on layer are on no figures one and three these are the current patterns developed in the planes of the the circuit this is one and three and they're pretty much what you would expect because both of them route across a nice solid area of ground with no disruptions they are precisely what you would expect to see this is figure four it is routed above openings in the plane the fields will spread and in doing so they will create a wider swath of current flow and the spreading fields create more energy radiating off the board hence what you saw in this you would expect the gray line from figure four to look something like that look at figure two case two is that ridiculous or what I mean there's energy going everywhere on that board because the energy remember is in the fields traveling through the dielectric space coupling to the the line and the plane below and when it got to this slot in the ground plane if it suddenly went oh oh where do I go it had no path to go so it's spread out along that slot along its entire length coupled around the end coupled through the air above the board to create a displacement current to get across the slot and coupled through the capacitance of the slot to get to the other side and that's what it took for this thing but in doing so the fields spread out immensely and caused a 20 to 30 DB worse EMI signature than any of the other three rule number one never route across splits in ground planes this is a rule that you really really have to think about dr. eric boe Girton said in a keynote that he did it out to him live in San Diego a few weeks back he said there are two kinds of Engineers there are those designing antennas intentionally designing antennas and circuit boards and there are those inadvertently designing antennas and circuit boards and there's a great deal of truth to that a lot of designers don't understand the complications created this is one of the complications you have to be aware of so if writing across splits is a bad idea what about this you've got what looks like ten traces routed across ten other traces on the bottom side of the board and they're routed over one another this is a two layer board with no planes in the board other than the poured copper that you see the blue is the top of the board the red is the bottom of the board and think about what's happening here we're not just routing across one split in a plane we have ten lines routing across ten splits on the other side of the board you this is going to be way worse than the trace routed across the split ground plane my friend Dan beaker received this from one of his automotive customers who said Dan we've got a serious problem in this circuit board and we're not sure what's going on dan had his group of designers at NXP semiconductor redesigned this board and what they did I'm gonna next slide shows just the top layer of the board what they did was rerouted these so that there are ground lines routed between every pair of signal lines that are on the board and by doing so by doing so he created a small space between the forward path and the return path by putting coplanar ground between each pair of signals now is this an ideal guard trace not even close to ideal but it's so much better than what they did it's night and day better they improved their EMI signature by 15 or 20 DB or more I don't remember the numbers but it was massive how much of an improvement they got you have to route every signal with respect to ground like you actually mean it you can't just route them randomly and go oh it'll find ground somewhere no it doesn't work that way that's not how circuits work they have to have an intentional low impedance ground nearby and that's what was done here notice that they also put a copper pour of ground underneath the IC why because this was a microcontroller that was less than ideal it's not a terribly well designed micro and the result is it was giving off a lot of energy and Dan wanted to help contain and collapse those fields so he put ground under it so the fields could couple to that space creating a low impedance attachment point to help reduce field size it's kind of like shielding if you will if you think of it in that way and in one sense it's shielding this is the back side of the same board with the traces on the back of the board routed with their ground with a and by the way these grounds are attached at both ends if you don't attach them at both ends you'll have an electric field shield only and you don't want to do that you want these to be attached at both ends so that you have the ability to move the electric and the magnetic field down the transmission lines from point A to point B we've got to do both ends that's how it works notice also that the decoupling caps are on the bottom of the board here and power is routed is it okay to route power in circuit boards if the frequency of the device is low enough absolutely I mentioned that we've always routed power in analog circuits I've done analog circuits now I've only designed to 16 gigahertz I haven't gone beyond that but in 16 gigahertz analog designs we routed power there's no reason to have a power plane in the board for 4 RF circuits or analog circuits and if you have digital circuits that are low enough in frequency you can route power unfortunately these guys didn't do a very good job of routing power on this board and again I've mentioned a couple of power delivery issues perhaps in the future someday we can do a session on proper power delivery because this was not done very well here's a four layer board stack up that has two signal layers on one and two and then a ground on three and a signal layer on four all of these signal layers reference the ground plane on layer three notice how thick the dielectric is between layers three and four why why did I draw that that way because that's how four layer boards actually are built if you go to the fabricators that you work with and ask the question what will the dielectric thicknesses be in a four layer board they're gonna tell you layer 1 to 2 and 3 to 4 is going to be on the order of eight ten twelve mills maybe fourteen mills tops and the dielectric between layers two and three will be on the order of 30 to 40 mils about three-quarters of a millimeter to a millimeter thick why because that's how they make four layer boards and unfortunately I don't have the time today to get into the specifics but four layer boards have a thick dielectric between two and three when we put ground and power on layers two and three of a four layer board it's a compromised approach and again that's something another piece of fodder for a future conversation but in this case we've got three signal layers to signal layers referencing the and one and two referencing the plane on three what's wrong with this well the people that did this the contacted Dan said here's our board and we have an EMI problem in our automotive product why well the answer is simple because the fields that couple from the signals on layer 2 through couple through the dielectric space to layer three and the signals on layer 1 have their fields in the dielectric space from 1 to 3 because those lines cross over each other now these were not routed above each other they were routed one in the X direction and one in the Y but because they cross over each other the fields coupled together every place where traces cross over one another is this gonna create a signal integrity problem absolutely not this will absolutely not create a signal integrity problem we did this for years and years before we were concerned about EMI and got away with it it's not an SI problem unless you're dealing with extremely high speed you know well up into the gigabit reads and designs stuff even in the hundreds of megahertz not a problem from an EMI standpoint this is a major problem this will only cause a couple millivolts of coupling from one of these lines to the other but a couple of millivolts is enough to create 10 20 30 micro amps of common mode current in line to line and that's enough to cause an EMI problem common mode currents coupled into lines are the major source of EMI and this is one of the ways that common mode currents are developed don't do this so how do what's the solution what did Dan tell his customer route the top layer in triplets think about the previous slide route the top layer in triplets and the problem goes away or for the most part goes away now what if you have an analog board in a similar structure I was contacted one day by a gentleman who said we've got an analog circuit an amplifier circuit and the output of the amplifier looks like the picture you see here when everything is functioning well unfortunately there's an accelerometer sampling circuit on the same board and when that thing's fired up and and sampling the accelerometer output the the energy from that feeds into this amplifier and the output of the amplifier looks more like the picture on the right here just a little bit of noise I mean a little more than is probably tolerable in fact a lot more obviously the circuit didn't work and they were worried about what can we do about this and my first question to the guy was what's the board stack up and his answer was the board on the previous slide we had signal signal we had signal signal ground signal exactly what you see here just the same four layer board that was on the previous slide because the fields couple through the same dielectric space there's no chance of stopping interference between the signals on one and the signals on two because they occupy the same dielectric space and there's just very little chance to get this thing to work and he said actually his initial question was what four layer board can we use to solve this and I said do you need three signal layers and he said yes and I said then there is no four layer board you can use to solve this you've got to go to six layers and they went to a six layer board which I will illustrate later which six layer board they used and you'll understand why it worked and why this four layer board did not years ago before I understood it and the people I worked with understood these problems we were faced with an EMI issue in the avionics world it was in my early years of avionics when I was with Goodrich aerospace and we had a six layer board that looked something like this signal signal power ground signal signal and we had an EMI problem what we realized years later was it was the same problem that Dan beakers customers had with the four layer board that was signal signal plane it's the exact same problem you've got signals occupying the same dielectric space they're coupling into one another and it's going to create a problem you simply can't do that we didn't understand that at the time we had no idea that that was a reality and so we thought well what's really happening here is those outer layer signals are too far away from a plane and they're radiated energy because we can't couple them tight enough to the plane that must be the problem so let's make this an eight layer board and we'll move the six layers that you have 2 layers 2 through 7 and we'll add a plane to the top and bottom of the board and Oh idea of ideas let's make that chassis because what better way to shield those signals than to put a chassis plane above them Oh fabulous idea wrong terrible idea the EMI signature of the board got worse when we put a chassis layer on layers 1 & 8 above the signal layers why did the EMI problem get worse because we were now coupling the fields on what head on lawn now layers 2 & 7 we were coupling their fields mostly to a plane that was connected to the chassis and there was no connection anywhere between the chassis and our internal ground because in the avionics world we figured out a long time ago we couldn't attach internal signal ground to the chassis ground and make that and pass all the levels of testing we had to long story why don't have time to get into that either but we couldn't so we were now forcing a return currents to exist in a plane that had no attachment to any of the ICS on the board and there was no way for these fields to couple through a low impedance path back to the driver versus where they needed to go and the EMI problem got worse we did not understand why this happened but we were guessing and we were good guessers in those days we decided to get rid of the chassis connection of those top planes and connect them to the ground plane of the board and as soon as we did that all of our problems went away because now we had provided a good quality return path in the board for the signals on 2 & 3 to couple to 1 & 4 and the signals on 6 & 7 to couple to 5 & 8 and everything worked wonderfully from that point on and frankly in 1993 when this happened we didn't have clue why it happened now I understand it perfectly I got called from a company near where I live some years ago and they said we've got a problem in a highly account board a twelve layer board and we have a signal this a very high-speed signal an analog signal and it's routed on layer one and it's one of the only analog signals on the board and when the it's at zero to nine volt signal and when the level of energy in the in the signal sinks low enough that the voltage of the signal drops below a half volt we are seeing an interference problem and the circuits not functioning correctly the circuit was operating at about the gigahertz or so in discussion we also found out that they had devices digital devices on the board that were generating high frequency harmonics because of their rising and falling edge that was at about a gigahertz so there was digital energy on the board at roughly the same frequency as the analog signal I went in and talked to him we discussed all sorts of things we looked at the schematic we talked about you know why I was on an outer layer I mean this and that just went through everything and then we brought up a picture of the board stack and basically the first four layers of the board looked like this and there were a lot of other signals on layer one mostly digital signals away from this high frequency analog signal and I said what is driving that you said it was a zero to nine volt signal what's driving it and the guy said it's 12 volts in ground that happened to exist on layers 3 & 4 of the board stack up and I said well then layer 2 must be a ground plane right and he queried it and said no layer 2 is a 5 volt plane and he sounded very puzzled he said you know this thing actually worked right until our most recent revision and he said I'm not sure how but I have a feeling during that revision this plane was changed from a ground plane to a 5 volt Lea and he got really mad he called up another engineer on the phone and he said Bob how did the plane in layer 2 of Yatta Yatta board become a 5 plane and Bob said well you remember back when we added the buffers to the i/o because we needed to have a 5-volt driver to get more signal energy into the lines because we were losing too much signal across these long transmission lines and we needed a spot to have 5 volts to drive these than the layout guy said heady Bob where should i how should i where should I find a plane to put 5 volts in and he said I told him I'll just turn one of the ground planes into five volts we don't need all the ground planes we have in the board anyway so he said I guess he turned layer 2 into 5 volts and I said to this guy after we hung up I said you do see why this is a problem don't you and he said yeah I think I do but I'm not sure so I explained to him things that we've just talked about and I said after I explained it to him I said where is the energy traveling in this from this circuit and he said in the dielectric space between 1 and 2 and I said that's right and all the return current from this high frequency analog signal is not in layer 3 or 4 where you'd want it to be it's in layer 2 because that's where the fields are and he said yeah I see that now and that's why it didn't work because the energy as the fields coupled out into the dielectric space they had to come from the IC into the dielectric spaces between 2 & 3 & 3 & 4 and they had to then find their way to that dielectric space between 1 & 2 so they could transmit down the transmission line well there was no way this was going to happen because there was no direct connection between that amplifier that sits at the drive into this and the plane on layer 2 and so the fields spread out across the dielectrics between 2 & 3 & 3 & 4 to find holes in the planes so they could couple up through and find their way into this dielectric space that exists between the signal on one and the plane on 2 and that's what it took it as the field spread because they were in the gigahertz region they coupled into digital signals in the same area that had gigahertz Harmon and voila they had an interference problem as soon as they dedicated an area of the board to five volts for the circuitry they'd added and changed this back to a ground plane all their problems went away and this brings up another question is it okay to reference power planes in a circuit board and some of you are going yes and some of you are going though the answer is yes if if and only if you reference a power plane that generated the signal in other words in this case they could have referenced the 12 volt plane because that 12 volts was used to reference the signal by simply coming out of the driver routing across the 12 volt plane to the receiver because both of them were attached to 12 volts and the fields would have coupled across that dielectric space coupled between the two devices and wouldn't have been a problem when you reference a power plane it's a bad idea to change layers and we're going to talk later about why that is true but it's generally not a good idea to change layers when you do reference a power plane so keep that in mind but most of all you must reference the plane if it's a 3.3 volt signal it can't reference a 5 volt plane or a 12 volt plane or any other plane other than a 3.3 volt plane period that's the way it works having low inductance on all pins of ICS is also extremely important are these low inductance IC pins what did we say defines low inductance spacing spacing defines low inductance these pins all of these signal pins are a long way most of them I should say in both of these ICS are very very far away from power and ground and both which means they don't have low inductance look at the IC on the Left look at one of the signal pins right in the middle of the left-hand row where do you think it's return current is going to be is it going to be in power or ground and I hope you know the answer is either it's going to be in a signal pin next to it or the two signal pins on either side of it if you look at this BGA I see on the right and pick one of the signal pins down on the lower quadrant of this I see where will its return path be the answer is in the six signal pins surrounding it these are great examples of extremely poorly designed I sees dr. Howard Johnson did a study years ago where he examined two FPGAs one from El Terra and one from Xilinx this is the Altair apart and as you can see if you compare this part to these two parts on the previous slide clearly this is a far better IC than the other two why because it has a lot more power and ground pins and those power and ground pins are closer to signal pins so you have a better chance of energy returning in a power ground pin which is what you want it to do however even this IC has areas where there are no powers and grounds present and the end result is you're going to have all of the signals for example inside these circular areas that are shown here all of them are going to return in one another they're not going to returning ground they're not going to return in power they're gonna return in each other this is the Xilinx part that is roughly the same part except it has a different pin out configuration than the Altair apart and it performed much better why look at all the powers and grounds the dark and light colored red or whatever color you want to call that balls that are in the Xilinx part much better power and ground configuration this IC gave better power delivery and it had better return paths for signals dr. Howard Johnson in his study found that the IC on the right caused five times greater interference between signals than the IC on the left 5x worse interference than the IC on the right all because of the pin out of the IC this is a and you need to be aware of it his paper is entitled BGA crosstalk it's still on the internet even though he's retired and it's still downloadable and I would strongly encourage you to get a copy of it and read it it is a magnificent paper that will teach you a lot about what I sees need to look like to function in today's world too many ICS that are being sold today by virtually every IC company on the planet don't look like they should look these are much better and they're getting better all the time this is a and IC from my friend Dan beaker again this IC was a microprocessor from nxp slash freescale back when they were free scale and it was a 324 pin BGA package and they went through a die shrink what does die shrink do die shrink makes the die smaller Oh wonderful that means they can get more diaper way for absolutely which means they can charge less and still make more profit yay I get a better price and they get more profit unfortunately you also get a faster I see the edge race when you shrink a die the edge rates go from whatever they are to something faster and as edge rates get faster what happens harmonic frequencies go up and as harmonic frequencies go up EMI gets worse signal integrity gets worse crosstalk gets worse everything gets worse they redesigned the dye and Shrunk it and afterwards they could not get it to work in the original package fortunately somebody in the office where they did this knew of Dan beaker and contacted my friend Dan and said Dan what do we need to do and he said you need to increase the number of pins in the IC and in doing so you need to add boatloads of power and ground pins they increase the pin count from 324 to 416 pins every pin added was power or ground so that it looked like what you see in this package on the screen all of the dark green is ground and so all you can see there are grounds distributed very heartily around the part the darker colored colors the purple and all the other dark colors dark blue those are all voltages coming into the device notice every one of them has a ground reference right next to it one pin away how do you minimize inductance spacing spacing it's all about proximity so all the power and ground pins are in pairs and they come into the part together also notice every signal pin which are the lighter more pastel colors all of them are surrounding power and ground so every signal pin is one pins distance away from power or ground or both how do you focus return currents and power and ground by putting the pins next to them this is what future ICS must look like if we're gonna continue to increase speeds and and actually expect them to work the good news a lot of IC companies are getting this I've seen a big improvement lately from micron AMD and XP obviously Intel and a lot of other IC companies that are doing a much better job than they used to if you go to an IC company and ask for an IC because you decide this is the one that has the the processes you need and it doesn't look something like this you really should think about moving on to somewhere else think about that group components let's move to a slightly different discussion group components by function and by family analog in its own area digital in its own area not in the same area not intermingled in different areas that are well-defined analog and digital and I realize they're not going to have straight line walls between them that they're gonna be jagged walls between analog and digital I laid out thousands of circuit boards in my 55 years I get how this works analog in one area digital in another area device is operating at different voltages in there area why if you put all the five old stuff here the three volt stuff here the two and a half old stuff here two things will happen one you won't have two and a half volts signals routed through the five old area with crosstalk problems because it's twice the voltage twice the energy level in those signals and two you'll be able to divide up one ground plane or one power plane sorry into multiple segments so that you can have five volt power three volt power two and a half volt power and so on around the board I've put as many as 18 different voltages and of all these plane before just by properly placing the parts to allow me to do that you can get by with fewer power planes and a board when you set up the board correctly device is operating at different frequencies all in their own areas by function within a given family or voltage and all I see is routing two connectors must be placed very near their respective connector why because if I have an IC that's out whose outputs or inputs come from or through a connector to another board or to a cable if I have long routes from that IC to the connector what's going to happen there will be common mode currents in circuits it's almost impossible to completely eliminate them what we want to do is design to minimize them but eliminating them nearly impossible if you route traces across the surface of a board and don't filter before you go into the connector common mode energy is going to couple into that and go to the next board or worse yet go out onto a cable that common mode energy will drive the cable as an antenna and you're gonna have an EMI failure so you want to keep ICS that are driving through connectors as near connectors as you can get them keep all routes confined to the stager section to which they're assigned all digital in its own area all analog low-level analog in its own area all high-frequency analog or RF in its own area don't allow these things to intermingle if traces are isolated to their own sections the need to splint and and digital ground planes is only necessary when the voltage or when the frequency level of the analog side dips well down into the the audio region well below 20 kilohertz if everything is operating above 20 kilohertz and you can physically isolate things from one another there is absolutely no reason to split ground planes and a lot of people don't seem to get that but I've solved a lot of EMI problems by getting rid of split ground planes so think about that taking a look at this in another way if we have analog and digital in their own areas you have an A to D converter in this particular example that's allowing the two to communicate with one another if I can physically keep the analog and digital stuff this thing's responding rather slowly if I can keep the analog and digital stuff far enough away from each other that I don't have coupling of fields between digital and between analog on on the circuit board in other words how far apart imagine if you will you've got ICS and traces on layer 1 and layer 2 is a ground plane what is the spacing between layer 1 and 2 whatever that dielectric spacing is if you can physically keep the analog stuff and the digital stuff including routes and everything 20 times that spacing apart the fields as because the fields will bloom out as they couple to the plain below no matter how much they bloom they will be still separated by enough distance that they'll have zero chance of coupling into one another I've put analog and digital stuff on a board where we had digital operating at gigahertz speeds and where we had analog stuff on the analog side of the board that had to have 100 DB or greater isolation from the digital put them on the same board with a continuous ground plane and not had a problem by simply putting enough isolation between them it is about physical separation if you can do that no matter how much isolation you need you'll be able to obtain it without having to worried about cross coupling between the analog and digital sections when you do this you won't need to split the ground plate speaking of splitting planes a lot of I see companies recommend if they have very sensitive ICS a good example our video controllers a lot of a lot of video controller manufacturers will say to you put our IC in an isolated section of the board for example this one that you see I'm trying to point to it right there in that area of the board and they'll suggest that you split both power and ground around this IC and that you feed power and ground into that area using low-pass or PI filters an LC CCLC right PI filter so that you can get low frequency energy from the DC planes they're not really DC but close from the main power section into this section up here without coupling noise across that area because there will be switching noise and the power and ground planes the reality is some of this to a degree is necessary but is doing it the way they suggest a good idea to think about what happens if you split both power and ground how are you going to get signals digital signals or analog signals for that matter data address all these other things how are you gonna get them from that IC that's in that confined area out to other ICS on the board without routing across the split in the planes well there's no way to get them there you can't do it so the reality is think about what really happens in a circuit the problem is the people who write these kinds of papers they say to themselves well the energy is traveling in the copper of the planes no it is not the energy isn't traveling in the power plane or the ground plane the energy is traveling in the dielectric space between the power and ground plane so is the noise energy that you're trying to keep out the noise be the switching noise being generated by this area of the board over here is all switching over to this area through the dielectric space between the planes not through the copper through the space if you break either the power or ground plane either one you'll stop the end you'll stop the noise energy from coupling across the gap so what I recommend to engineers and it took me a long time in the telecom world to get the engineers to think this way because boy they constantly wanted to split both well all you need to do is split the power plane only that's all it's necessary to get everything to function correctly without having noise coupling between the two power sections split power only leave a continuous ground plane and now you have a reference for stuff to route in and out of the area you can reference the power play or the ground plane speaking of that if we have a split power two powers of the same level that we've done for the reasons we just discussed can we route a signal across that split power plate and the answer is yes and no yes if the planes are physically close enough together if they're eight mils separated or less the planes will be close enough together what's going to happen when you route across that split well the fields are coming down through this dielectric space right here and they're headed toward this gap and when they get to this gap they couple through the gap and create capacitive coupling across the gap back up into the dielectric space between one and two the fields will expand a little as they couple through the gap and you'll get a displacement current between the power plane and ground plane for the return current to travel as long as that gap is short enough that it's a lumped distance and long story how we determine that but it's at today's signal speeds the gaps that we put between planes trust me it's not going to be a problem it's an impedance discontinuity but if it's short enough you don't care and is it going to create an EMI problem well the answer is if the two planes are close enough together no now that said if the two planes are fart if by the way if these were gigahertz level signals gigabit signals or gigahertz analog signals I would never route across this split power plane because there's too much risk involved in doing that and if both planes are split of course you wouldn't want to route across that gap dr. Bruce R Shambo did a study years ago remember I said a short while ago four layer boards have a thick dielectric between layers 2 & 3 between layers 2 & 3 so I said on this previous slide as long as these two planes are within eight mils of one another you can probably do this and get away with it but on a four layer board planes aren't within eight mils of one another planes on a four layer board are generally separated by 30 to 40 mils and 40 mils is not an uncommon spacing neither is thirty thirty-five is an extremely common dielectric between layers two and three of a four layer board so if we're out across a split power plane like we did on this slide and there's 30 or 40 mils of spacing between them is that a problem oh you bet it's a problem dr. Bruce R Shambo ran a study to verify this he took a four layer board with a ground plane on layer two he set up a signal and a receiver he set up a driver and a receiver with a signal line that routed across layer one referencing the ground plane on layer two and he drove this and he used a near field probe and a spectrum analyzer to sense the energy coming off this board all the way around and he measured the worst-case energy radiating from this board then he turned this signal off and he turned on a1 in the exact same location on the bottom of the board that was referencing a split power plane and he drove this one and he made another measurement of EMI coming off the board then of course everyone knows that all you have to do is put a capacitor across the planes just bridge those with a capacitor and all your problems go away right so let's test that Bruce said he put a set of point on one micro fur capacitors bridging the two splits in the plane made a third measurement and put a second set of capacitors and made a fourth measurement this is what the first measurement looked like when he was measuring the EMI coming off the board with the signal referencing ground when he switched the signal to the one referencing the split power plane it looked more like this depending upon frequency this EMI signature in red is anywhere from 20 to 40 dB worse than the signature in blue we're talking about not a little bit worse yeah my problem here we're talking about holy mackerel are you kidding me worse EMI problem this is a massive difference between these two signals 30 to 40 DB is night and day then with the capacitors added he made a measurement and lo and behold look what happens at low frequencies under one to two hundred megahertz the capacitors do a wonderful job of reducing the energy coming off the board but look what happens at high frequencies above five 600 megahertz is no help at all the capacitors do nothing at high frequencies then with the second set of capacitors things got a little bit better at all frequencies but only got a lot better again at low frequencies why did the capacitors help at low frequencies but did little to nothing to be beneficial at high frequencies what is the reason for this very simple a capacitor has an impedance due to capacitance that starts at a high level and goes down towards zero as you go up in frequency it has an impedance due to inductance inductance of what the plates in the capacitor the metal in the pins of the IC r the device itself all of these things form an inductance and that inductance starts at a low frequency and goes up as you go up in frequency there's a point where they cross one another where they're the same impedance at that impedance there are a hundred and eighty degrees out of phase from which means they cancel each other out and their impedance at that point is zero because they totally cancel each other out the only impedance in the capacitor at that point is the resistance of the copper in the structure so the O this is called the self resonant frequency the overall frequency response looks like the red curve shown here that's what capacitor curves tend to look like capacitors do all of their best work right here at the frequency referred to as self resonant frequency on this side of the device their impedance is higher but at least they're a capacitor on this side of the device their impedance is going up and the worst part of all is it's going up why because of increased inductance on the right-hand side of self resonance they're becoming a bigger and bigger inductor and there's a point where they don't do anything beneficial anymore hence these curves that you see here at high frequencies the capacitors offer no benefit bottom line don't route across ground splits and don't route across power splits in thick dielectrics it's a bad idea so keep all that in mind as you're designing do not route signals on ground layers if you can avoid it now if you have to route a really if you have to do a real short route across the ground plane like we've shown here you might be able to get away with that if we've only got two or three signals crossing that ground split because that's such a small cavity it's not going to be able to resonate probably not resonate at the frequencies we're concerned about anyway so you're probably going to get away with that you're going to get some field expansion when you do this and you're going to get some coupling between the lines and that's a reality but the coupling will be small because the coupling distance will be short if these are sensitive analog signals really bad idea really bad idea we did this we did a board years ago when I was at l3 where we put a 24 bit A to D converter on a two layer flex board and we brought in the outputs of three accelerometer circuits that were in the aircraft to sense pitch roll and yaw and we brought those three outputs through amplifier stages to boost their signal level and then took them to the a to D there were places on because it was a two-layer flex board where we had to do this on that flex board but the reality is we only did it which with the digital signals that were less sensitive the sensitive analog signals we gave absolute priority to and made absolutely certain that they in no place nowhere on that board lost their ground reference from point A to point B so do this but do it sparingly and do it with less sensitive signals when you're dealing with really low frequency lines like control lines when I say low-frequency what do I mean low rise slow rise time control lines tend to have slow rising and falling edges and even when they have fast rising and falling edges because they are clocked at a low frequency rate we don't care if we attenuate them and slow the edges down it's not a big deal so when you're dealing with control lines you can run them through you know bridge across other lines using a zero ohm resistor don't ever try this with high frequency lines because a zero ohm resistor at high frequencies is not zero ohms a zero ohm resistor at high frequencies is some high impedance due to its inductance all these parts have inductance and inductance drives up impedance neither of these is ideal but used properly can be helpful when you're dealing with low layer count boards so what happens when you want to change layers how do we change the layers what's the right way to do this well why do we change layers we change layers because we have to bridge we have to change direction let's say the top layer of the bore is routed in the X direction the next routing layer which may be layer three is routed in the Y the next layers and the X the next and the Y and so on going down through the board so if I want to change direction where's the best place to go I'm routed on layer one with a plain on layer to go from one to three why because the fields that are try pulling through this dielectric space right here between one and three when they get to this via those fields will couple through the hole on the plane and they will continue on right through the dielectric between two and three without any spreading of the fields at all there'll be no field spread so if there are other vias nearby you'll never see the impact of doing this what if we have to change layers in a high layer count board and go from one ground plane to another what's the best way to do that well the best way to do it is using a ground via coupling between the two planes that's relatively close to the signal via so in this case we put a ground via here with the signal via being the red red line here this is a picture from dr. Howard Johnson he did a study of this and determined that there is a lot of benefit from an EMI standpoint to do this now there are some signal integrity people in our industry and I'm thinking of two in particular now I'm not going to mention their names both of whom will tell you that from a signal integrity standpoint this is unnecessary and they're probably right now I would argue with them that at gigahertz frequencies this is unnecessary and they would argue with me that I'm wrong and you know whatever so from a signal integrity standpoint yeah this is probably not a necessity but if you care about EMI or if these are sensitive analog signals I would think twice about routing them without using a nearby return via from layered layer if this was a sensitive analog signal I'd probably put for return vias around the signal because in the analog circuits especially at high frequencies we've got plenty of space between everything and there's lots of room around vias in analog circuits to put multiple return vias so I would likely put four around why do you think an SMA connector has four ground posts there's a reason for that it's to contain fields putting four vias around a sensitive analog signal would contain the fields with digital signals you just need to get a return via nearby now I'm a realist as said have designed thousands of circuit boards over the years the last project I worked on at l3 was a three inch by 4 inch circuit board that happened to have 1,300 components on it 10 BGA's of those BGA's two of them were 1,300 pin parts and it was a densely packed board and we obviously were not going to put a return via next to every signal via what we did is we would clump groups of signal vias and put if possible a return via between them and return vias around groups of signal is because the idea is to contain fields if you don't put the return via there the fields will spread out across the dielectric just as it would with power and ground planes when you're coupling between power and ground you get a displacement current between the planes you get the same thing here the beauty of ground planes is you have the advantage to add a return via so you can tightly contain the fields in this space between the vias if you don't put them there these fields are gonna spread out across this area and they're gonna cause no end the problems for you and you don't want that to happen one thing to keep in mind a lot of people say to me Rick I need to fill vias because I have to put solder mask over all the holes on the board that aren't component holes is it okay to fill them with non conductive fill the answer is you can fill them with peanut butter if you like think about where the fields are in this case the fields are in this dielectric space between these two vias and they're forming current on the outside of the two via barrels there is no current inside the via the current flows on the outside of the vias fill them with whatever you like it just doesn't matter what if you're going to change layers from power to ground well how do you get there well the capacitor will help with the low frequency energy the capacitor will carry the low frequency energy from the power plane to the ground plane or vice versa well what about high frequency energy we just said a minute ago capacitors don't do a good job at high frequencies no they don't and with today's digital circuits you will have lots of high frequency energy so how do you get the high frequency energy across there the answer is very simple the planes need to be close together if they are within eight mils of one another then the combination of the capacitors and the close-set planes will allow you to get the energy across without getting excessive field spread between them and that will work very very effectively what if the planes are widely spaced what if they're like the planes of a four layer board well rule number one don't put power and ground on layers two and three of a four layer board it's one of the worst board stack ups you can use also don't put power and ground on layers two and five of a six layer board wait a minute Rick we do that all the time yes I know a lot of people do and it's a tragic mistake and it's one you don't want to make why because the layers are so far apart there's no way for signals that have to change layers to couple between them the fields are going to spread out in this case four inches how many other vias are going to be in that area with all those square inches of coupling you're going to have via a coupling to be cdefg and via B is gonna couple to AC D F and G and so on all of these vias are all gonna be coupling all of their fields into one another and all these circuits are going to be creating common mode currents in one another because of the field spread will it create signal integrity problems possibly in a very sensitive analog signal possibly in a very high frequency digital signal maybe in a low frequency digital signal below a few gigahertz who cares from a signal integrity standpoint who gives a rip but if you care about EMI you better care you better care a lot because when it comes to EMI this is a tragic mistake don't go there Lee Ritchie had a client who contacted him years ago with a six-layer board stack and this is a picture out of Lee second volume two of his right the first time signal integrity book and it shows a six layer circuit board that these people contacted him about and said Lee we've got a board with signals on one signals on three signals on four and six power on to ground on five and we're having an EMI problem Lee determined after much consideration that it was a power bus delivery problem and they talked about more layers and the guy said nope nope not a chance in the world management I'll never they're gonna fire all of us if we even recommended so Lee said alright here try this I want you to pour copper on the signal layer one I want you to pour copper all over signal layer one and I want you to pour copper all over signal layer three and I want you to attach all of that randomly poured copper to the ground plane that's on layer five with lots and lots of ground vias as many as you can squeeze in then I want you to pour copper on layer four and on layer six as well and I want you to couple all of the random copper on these two layers to the power plane on layer two with lots and lots of vias as many as you can fit into the structure before they started this before they did the copper pours they had 500 and then this just basically shows where they did the copper pours they had 500 Pico farad's of total plane capacitance in the board itself created by the planes that were on layers 2 & 6 which are very far apart planes on 2 & 6 of a 62 Milotic board are going to have about 50 mils between them about one and a quarter millimeters of spacing between them way too much to give any decent capacitance and they ended up with 500 Pico farad's after they added the copper pours the capacitance of the planes themselves without adding the coupling went up to 4100 Pico farad's and that helped improve the emi signature due to power delivery because they had better they had higher they had more capacitance at high frequency's the physical capacitors we put on boards help a lot with the delivery of low frequency energy in circuit boards the capacitors don't do much at high frequencies so we have to have some means of putting power delivering power to ICS through the board without the physical caps themselves and planes help a lot and we increase they increased plane capacitance by doing this even bigger than increasing plane capacitance they reduced plane inductance by a factor of eight think about reducing plane inductance by eight times eight hundred percent reduction eighty percent I'm sorry reduction in in inductance simply by putting copper pores on the board why because inductance is a proximity event instead of having power and ground on two and five they now had power and ground on 1 & 2 2 & 3 3 & 4 4 & 5 5 & 6 6 & 7 and so our 5 & 6 and they had multiple structures of power and ground all with closely spaced planes and yes they were only partial planes but the fact that they were closely spaced drastically reduced inductance and we're going to come back and visit this a little more in just a minute before we do I want to talk about Oh here's the EMI signature by the way of this before and after the copper pours all we did was add copper pours to this board what did that do to produce ability everyone out there who's familiar with manufacturability is saying than themselves you made it better absolutely you pay for copper removed not copper left on the board the more copper you can leave on the board the less that board's gonna cost you it's that simple if you can leave every layer as full of copper as possible that boards going to be easy to manufacture and cost-effective and if you don't believe that call your fabricators and ask them leaving copper on boards is a benefit so they got that benefit out of it plus the EMI signature shown in green here was before the copper fill and the blue is after the copper fill they got an 8 to 10 DB improvement in the emi signature just by adding copper pores which cost them how much zero there was time to design it but once it was designed the cost adder was zero so let's look at four layer boards in 1994 we had a product when I was in the tell care now in the the avionics world working for good resource base we had a product that that had to be extremely cost effective it had to sell for $1000 which is in that world nothing that's like giving it away the pre cos avionics world has some really high costs associated with it and we had one for layer board in this product and it failed emi testing first time out and it was a four layer board with signals and components on the top power and ground on two and three and signals and components on the bottom and we failed by a lot we failed by 8 10 12 DB it was ridiculous so we got together we were starting by this time this was like nineteen ninety five or six and we were just starting to understand emi problems by then and we got together and said we need to change this four layer board and we all talked about it decided to move the signals from layer 1 down to layer 2 and move the signals from the bottom of the board up to layer 3 and we poured next to the components on 1 & 4 ground everywhere and attached every place were ground on one and ground on 4 overlapped one another we attached him with lots of vias through the entire board structure we then reconnected all the signals to the ICS with with you know signal vias and so on and all and what amazed me when I saw when I looked at layer 1 of the board with components and signals on it it was so packed it was ridiculous but when I moved the signals to layer 2 and none of those pesky components were in the way I was shocked how much open space there was between signals and we poured all that open space with copper that we attached to power and we had to report a few times to get it to connect to all of the points where power had to go it took a while it wasn't a 5-minute operation but when we did this we improved the emi signature of this board by something like fifteen or sixteen DB it was night and day how much better it was I was stunned at the improvement and the reason is several things one the signals went from outer layer to enter they so they were strip line instead a micro strip biggest cause of all we had signals changing layers between layer 1 and layer 4 which means they were referencing power on one layer and ground on another and when you change signals from 1 to 4 you've got to move those fields from that dielectric and 1 and 2 to the dielectric and 1 & 4 are between 3 & 4 and how are you going to do that with a power and ground on 2 & 3 well you're not you don't move the fields well and you a lot of the high frequency energy causes interference and spreading of fields and EMI problems and outrageous levels so you don't want to have 4 layer boards with power and ground on 2 & 3 and we quickly learn that reality and when we went to this look at all the signals on this board reference ground on 1 & 4 every signal reference is ground so when we had to change layers we simply dropped to ground via next to the signal via and voila problem solved this is a night and day difference between a standard four layer board in this this is the other version of this board that I like putting ground ground planes on both of the inner layers yes this is not easy to do you have to have a really low density board to do this in a four layer board if you have a lot of signals and a lot of components this won't happen in this type four layer board you'd be pretty much stuck with using the one that's on the left-hand side of the screen this is the this is the impedance of the planes of a four layer board with power and ground on two and three once we redesign this board that's marked figure a and measured its power bus impedance it went from what you see in gray to what you see in red that's a logarithmic scale that's an improvement of about 60 to 80 percent lowering of the impedance at all the frequencies where it's performing is this a great power ground structure no it's a four layer board you want great power and ground structures you better start thinking ten twelve fourteen sixteen layer boards because you aren't going to get a really low impedance power and ground structure in a four layer six layer board it is not going to happen but this is as good as you'll ever get out of a four layer board I can guarantee that six layer boards to avoid the one on the left is the one we had at goodrich years ago and I explained why it was an EMI problem the one on the right is the one Lea Ritchie's customer had prior to to adding the copper pores think about where power came from I asked engineers all the time where does power come from and the board and the answer I get all the time is Oh from the power plane wrong the power comes from the dielectric space between the power plane and the ground plane in this case that's a dielectric space between layers two and five what else is in that dielectric space oh I don't know a couple of signal layers oh gee really well guess where their fields are there in the same dielectric space where the power is coming from if you think those fields aren't going to interfere with one another think again because they will interfere with one another and that's exactly part of the problem that leads customers board had so when he added the copper pours yes he improved power delivery but he also got rid of this problem by adding the copper pores because once they added the copper pores as you can see this board on the right I'm having trouble getting my finger lined up power now instead of coming from two to five comes from this dielectric space and this dielectric space and this dielectric space and this one and this one so you get power delivered from five dielectric spaces that are all close together and yes there are partial pores of it of copper but they're also much closer together capacitance is higher and inductance is lower and power delivery will absolutely be improved but not only that these signal layers on two and three now their signals couple next to the area where powers coming from so powers coming from here and the signal fields are next to them here and instead of intermingling with them when everything existed between two and five this just night and day difference in performance think about that when you're designing circuit boards these are the planes of a six layer board with power and ground on two and five these are the same point these are the planes of this board on the right look like that look at the difference that's an order of magnitude ten times reduction in impedance an order of magnitude think about that what would you do to get an order of magnitude improvement in your power delivery I don't know I'd spend a lot we don't have to you just have to design the board correctly it all comes down to proper structure and grounding this I got a call years ago from a company in Montreal said we have a four layer board it's failing testing management's willing to let us go to six layers what would you do and I said you just answered your own question you have a four layer board management's willing to let you go to six layers move layers one through four to two and five put power on the top layer ground on the bottom layer pour copper on the signal layer two and five and connect them to power and ground with lots of vias and your problems will be solved now this is a very non cost-effective board because you only have two signal layers in a six layer board I mean with anybody in their right mind do this some scratch no this is not something you do from scratch this is an oh my gosh are we in trouble and need to get out of jail free card you're playing Monopoly and you're in jail and you need to get out and this is your get out of jail free card that's exactly what this is these guys eventually redesigned their four layer board to get one that would pass testing and but they use this ship product in the meantime they had a market window they had to hit and this is how they hit their market window think about that this is a six layer board that I love remember I mentioned the company earlier with the analogue amplifier that had a six layer board with three signal layers this is the board they went to to solve their problem notice there are three signal layers one on one three and five with ground on two four and six think about it it's perfect everything references ground you go layered layer you drop ground via you absolutely if you're going from one to three you don't need to ground via if you're going from five to three you don't need to ground via if you go from one to five you'll need a ground view but other than that you're really okay as far as as vias go it's really not a problem and this is another six layer board that I like it's it's it's an improvement over many of the others and you can see that everything in this board references ground all the power Porter's allow you to to create good power delivery the one in the middle by the way the first time I did this I was concerned that it was going to create an imbalanced construction to have three signal layers and three plain layers but I poured the signal layers with copper I did it first one I designed I did an auto router the signals on three layers I poured copper on the three signal layers and I sent the Gerber files which were Gerber's back then to one of our fabricators and said how hard would this board be to produce and they said the fact that you've put copper pours on all the signal layers they look like plain layers to us this looks like six plain layers we could fabricate this easily so even though it might normally be imbalanced in that case it wasn't eight layer stack UPS this is an eight layer stack if I don't have time to get in you know if you think about what we just said about four and six layer boards and you continue this mentality into other board stack ups you'll find it it'll work for you no matter what the case may be you just have to think about every signal layer referencing either the right power plane or a ground layer and you you you don't route signals between power and ground unless there's a ground layer much closer to the power layer because you don't want to create a problem this is an eighth layer recommendation from a major ic company and I'm not going to mention who they are but this is a major IC company and I can believe that this board actually worked in their lab this had a 1300 pin microprocessor on it and they said the only way we could lay this thing out in low layer count was an 8 layer board and this was the best we could come up with and I can believe that with enough on dye and on package capacitance in their IC they made this thing work but one thing I'm a hundred percent sure of there is no prayer that this thing could pass EMI testing not a prayer that this thing could pass am i testing why where's power come from from power layer one don't say the power plane it comes from the dielectric space between power 1 and power 2 which means where are the return currents going to be from power 1 they're going to be in power too some of them are also going to be in the ground plane but look what's above power 1 there's a signal layer there which means the power that's coupled to the ground plane is going to be interfering with the signal fields that are in that dielectric space this is a lose-lose situation this is a very poor board stack if you care about EMI if all you care about is is signal integrity you'll probably get away with this if you care about EMI good luck because you ain't going to get there from here this is a 10 layer board that has everything in the world wrong with it I mean number one look look at the center there's a power layer there's a power layer here above it there's a layer with signals and power then signals and power then power so way over way over here somewhere you've got power power power power you have 4 power layers in a row who in their right mind could possibly think this was an okay thing to do this is an outrageously bad concept and it should never be done you never put a power plane in the board without having a ground plane immediately adjacent to it period and that's basically what this is talking about this is a 12 layer board that we used when I worked at l3 we used it in a lot of our structures look at it layer one is referencing a ground plane on to power and ground are on two and three why because it puts them close to the surface where the ICSR gets rid of via inductance to attach power to the IC great idea you've got a signal between a power and ground plane there but you also have a ground plane referencing this signal so a nap and a ground plane above the power plane to pull the power energy into that dielectric space so it won't corrupt these signal layers this is a great board stack up we use this on a lot of our structures the three by five board I mentioned that was packed full the stuff used this particular 12 layer board stack up it's got a lot of things wrong with or right with it and almost nothing wrong with it the sickness if you really want to minimize cost don't make this a 62 Milotic board in order to keep dielectrics to a producible thickness we made this board a 75 to 80 mil thick board and with that I will thank you all for attending do we have any questions that we would like to have answers to yes we do thank you no boy by the way those questions that we can't get to now did these people leave a way to get back to them and EMI address or something I mean India might got him so my head so yeah my email email address did they leave an email address okay all right cuz we probably won't get to I mean I'll stay here as long as you want if you guys want to go overtime I'm fine with that okay let's go let's go talk at all team life 2018 ah there's some legitimate disadvantages of ground flooring ground flooding yeah ground ground flooding or ground ground pouring or ground ground floods you will change the impedance of nearby transmission lines that you poor ground floods around and that is one disadvantage unfortunate or fortunately the advantages are many we talked about this the reality is you balance copper I don't know how much you've thought about balancing copper on signal layers the balancing copper is one of the secrets to creating a low-cost highly producible board and when you put ground pours ground floods on signal layers you do exactly that and as we just mentioned going through this last section when you put ground and not just ground pours ground and power pours on signal layers you create alternate dielectrics of power ground power ground power ground and that delivers power from multiple dielectric spaces instead of from one or two or three dielectric spaces and that will always improve power delivery so there are some minor disadvantages but when it comes to cost it's an improvement when it comes to performance it's an improvement if anybody I'm gonna speak my email address for those attending and you're welcome to write me if you want to know more about this please send me any information you have on disadvantages of this because I'd like to see it myself my email address is our H a R T L e Y all one word at Columbus Co l um bu s dot RR dot com it's my email address email me if you want to talk more about this because I think we need to move on to the next question hello Andre good for layups why exactly a signal power layer on 2 & 3 better than 1 & 4 for density signs ah ok let's go back here because we'll get there eventually we're almost there here we are if you think about what's going on here there's components on the top layer of the board and when you pour a ground when you put a ground plane on layers 2 & 3 of the board the example on the right-hand side then that means that you have to squeeze all of the signals and components and power pours on layer 1 of the board and when you have to squeeze everything on that top layer of the board if it's a dense design it's not going to happen the reality is the board that we redesigned in 1994 when I was at Goodrich aerospace that we made the example on the left the a example the only reason we were able to get it into still four layers is because we poured ground in and around the components on the top and then made sure that all of our signals were routed so they referenced that ground port and then we poured all the open space between those signals with power and that's the only reason we were able to do this because then a dense board if you lay out the components of a four of a board in four layers on a four layer stack up and try to get this two components the signals and the power pour on one layer you're gonna find that you can you you won't be able to do it in terribly high density board I I hope that answers the question open source projects meaning I'm trying to oh I see like projects that are out on the internet you know that's a great question and I don't I I can't really answered the question because I haven't looked at a lot of the circuit boards that are available through open source projects what I can tell you is that in their board stack ups if they don't have power next to ground and if they don't have all signals one dielectric layer away from power or ground then it's not a good stack up that's the best answer I can give you every signal must reference a ground plane or at worst power that generated it and every power plane needs to be one dielectric space away from ground if those boards stack ups do that then the other good board stack ups if they don't well good luck and that is a problem parallel there's there's two schools of thought on multiple values of decoupling and all the board's we did over the years and telecom and aerospace we always used one value of decoupling now we had obviously we had medium frequency decoupling that was much much higher in value 25 50 mics those types of things but we're talking about high frequency decoupling in this case we would use one mic 3/4 of a mic and so on and so on going down in in very small increments because of parallel resonances I think what we really need to do is this is a hard question to answer without lots and lots of pictures but the reality is if you pick the values correctly you can get capacity whose resonance point is under the crossing point of two other capacitors where a parallel resonance will tend to occur and if you have a lower impedance from a third capacitor that is underneath the crossing point of two caps you'll help dampen out the anti resonant peak so antsy resonant Peaks are a problem but that usually happens when there's huge separation between values like one mic point one mic and point O one mic that's a very large separation between values and that's where an T resident Peaks tend to occur there's two schools of thought there again I hope that answers the question for you reasonably well if you pick the values right and simulate it the key is simulation power buffs design these days if you're not simulating you're guessing and guessing is not the way to get good power design in this day and age there are some really good tools out there my personal favorite is the ANSYS tool for power delivery it's hyperlinks is also good there are others as well that are really really excellent tools for power delivery but I would encourage you to simulate that for for input/output the lines from oh I see the connector well if you have an IC that's driving through a connector to go to a cable and it's differential I mean if it's single ended the common mode chokes not going to do anything but if it's a differential signal then yes you want you generally want a common mode choke and you want it to be as near the connector as possible all filters that are attached to lines that are going into a cable should be right at the connector whether it's a low-pass filter for i/o lines that are single ended low frequency single ended or whether it's a transformer that's used for a very high frequency high-end like high-end Ethernet and that sort of thing because those transformers generally have common mode chokes in them as well so a common mode choke is very effective with differential signals if it's placed close enough to the connector to keep common load energy off the cable but it has to be chosen size-wise based on frequencies as well that's sure you know what I mean I hate to be rude and I'm going to try not to be I PC 2 2 2 1 and all the other IPC standards have a lot of good things in them but they also have some things than them that that aren't worth using for example their impedance equations unless you're doing digital design with low layer count boards that have dielectrics relatively low that have dielectrics in the 4 to 10 mil range and traces in the 4 to 10 mil range those impedance equations are basically useless and even in the range where they're where they work well there are only five to ten percent accurate so it means the answer you're gonna get is only going to be within five percent maybe only within ten percent so there are a lot of things in the IPC standards that once made sense when the standards were written the problem is they don't update them often enough and then our industry changes much faster than they can change the standards so the stack ups in those standards really are not good examples that's fine we can answer as many as you want when you're dealing with Flex boards they have a huge advantage because if you're if you if you have a board that is a static flex board where it's going to be bent one time and then kept in that position we did that at l3 all the time we had lots and lots of flex boards that had a solid ground plane in it because we didn't make him real thick we made them two three four layer boards and speaking of that flex boards you can make two or three or four layers rigid boards you never go three layers or five layers or seven layers with rigid boards you always do two four six eight ten and so on but in our Flex boards we would often make them two three four layers and as long as the dielectrics weren't too thick we didn't stretch the copper when we bent them and it ended up not creating a problem when you have a dynamic flex that is constantly moving when it's in service if you don't use hats planes you can fatigue the copper and you can damage the board and create all sorts of problems so that's one of the biggest advantages to crosshatch planes in a circuit board with a r4 board or any rigid type board the only advantage I have ever seen to cross-hatched planes is allows you per given line width to raise the impedance of the line for given spacing and line width and that's the only advantage I could see in a rigid board would be to raise impedance without having to decrease and the answer is with any cable shield and we talked about this briefly as we were going through the material with any cable shield I mentioned on one of the early slides that a box a metal enclosure around electronics is a Faraday cage meaning what meaning it will contain the fields that are within it and it will keep out fields from the outside from getting in provided the openings in it are small enough to filter to effectively be a Faraday cage at all frequencies a shield on a cable is not you're not every everybody ever all the things I read say to quote unquote ground the shield you're not grounding the shield the purpose of the shield is to continue the Faraday cage so you've got a box you have a box here and coming through the Box you have circuitry inside you come through the wall of the box to a cable out here the purpose of the shield is to continue the Faraday cage effect of the box so that this signal can go from a circuit board through a connector into a cable without ever experiencing the fields of the outside world don't think of it as grounding the shield to the chassis or the internal signal layer think of it as continuing the Faraday cage now with that thought in mind never ever attach the shield to the internal ground that is absolutely the wrong place to put it because now you're allowing any energy that couples on the outside of the shield to couple right through the opening in the box and couple right into the ground structure of the board and that's the last thing you want so you attach it to the box itself in a with a large number of with a 360 degree attachment you choose connectors that are designed to give you a 360 degree attachment of the shield to the box and that's how you attach cable shields I hope that helps boy this is a loaded question I don't know could everybody hear that here your question no no I don't get doesn't that beat your I just want to make sure everybody listening could hear you okay good the question is repeat the question again and then I'll designed poorly how feasible is it and that is a great question the answer is yes no no meaning that in a nutshell yes you do need to know all the rise times beforehand why because you can't determine what distributed and lumped link lines you have until you know rise time they're all a function of rise time frequency as I'm sure everyone listening to this understands so you do need to have the rise times of all your major ICS before you start the layout of the system how do you get that oh that's the good question and that's the part of your question that's really loaded because there is no easy way to get that wouldn't it be fabulous if I see companies would publish that data well they don't go to the app notes go to the data sheets and try to find rise times some IC companies today do publish rise time but most do not this is something I've been needling IC company's about for years I don't know why they don't want to do it but they don't now the reality is the ibis model has rise times embedded in it it has to think about what an Ibis model does it's going to simulate the energy moving down a transmission line relative to the lines impedance and what's going to happen when it hits the loads on the line and the only way it can simulate that accurately is to know rise time so the rise times are embedded in the Ibis and in the spice models so you can download those there text files which you can read with any text editor and you simply download those files from the IC company's website and once you have them you open them up with the text editor and you look for either rise and fall time or dv/dt sometimes they're listed as rate of change of voltage with respect to time which means then you have to determine what your rising signal level will be let's say you are driving with 3.3 volts and you're going to have an output that goes to three volts you then take that DV DT number and extrapolate it so that you can determine rise time there's no easy way to get this information I'm sorry to say but you do need it every project I worked on in the telecom world and at l3 which was the last 25 years of my career in every single project we downloaded every Ibis model before we started the project and we extrapolated all of this data from those models prior to starting the project I hope that is helpful go ahead it's not a good idea to overlap power from if if you are splitting ground and you shouldn't but if you are by overlapping I assume you mean in a case where you have say a split ground and you have an analog ground and you have digital power that on the next layer comes and overlaps that if that's what you mean then no that's a terrible thing to do oh I think I know what he means you're probably talking about at the edge of a board do you want to have power and ground run all the way out to the edge and be right above and below one another or do you want to pull power back from the edge there's a there's a rule that was dreamed up and I can say dreamed up because it's been proven wrong that says that if you pull the power plane back from the ground plane by 20 times the spacing between them it will improve the EMI signature we tested that in the telecom world and found no benefit to it dr. Todd huming dr. Bruce R Shambo dr. Tom Van Doren and a host of other high-level PhDs have tested this and have proven that not only does it not help that it can actually be harmful and I'm not going to say who dreamed this up but it was a nightmarish dream that that a person had and told the world that it helps and it doesn't and if that's what you meant then you know I hope that's what you meant if you didn't let us know what do you think of a 16 layer 63 mils Wow well first off I think it's a mistake to do 16 layers and in a 1.6 millimeters thick board which is what you're saying 62 mils is one point six millimeters because it's going to be nearly impossible to manufacture cost-effectively because the dielectrics are going to be so thin that it's going to be an absolute nightmare for a fabricator to produce that board I mentioned when I talked about the 12 layer board that we used a lot at l3 that we intentionally made it 70 to 80 mils we typically we targeted 75 mils plus or minus 5 mils I mean if a board has to plug into a card guide where the spacing between the card guide is 62 mils one point six millimeters well then you make it one point six millimeters thick but if you don't have to plug into that card guide there's absolutely no good reason at all to make a board 62 mils thick we do it out of habit I mean if you have a mechanical reason that's forcing you that's one thing but I can tell you right now the cost of that boards gonna go through the roof and it's going to be really hard to fabricate because the dielectrics are going to be two to three mil dielectrics between every layer and good luck it's just not going to be producible PCIe what's that always so it what meaning what well that's fine PCIe is is very high-speed and I get that and I understand why you're doing a high layer count I understand that you've probably got a lot of power and ground layers in the board you know referencing signals and all that and that would be the right thing to do for PCIe but are you saying by that comment that that determines the thickness of the board because I'm not familiar enough with the physical parameters of PCIe to know if they drive board thickness so if you could respond to that that'll help we'll wait for your response and we'll go on to another question sigh links design what about it that's it that's another comment sign links I mean again unless there's something mechanical driving a 60 to milk board then there's no reason to make a sixteen layer board 62 mils I mean if your mechanical structure insists that you plug it into something on card rails with a 62 milling well then that's what you have to do but other than that I mean there's no reason to do that we mounted most of our boards in telecom and avionics on standoffs so we could make them any thickness we wanted you know and when the mechanical guy came to me the first time and said this is gonna be a cig somebody told me this is gonna be a 16 layer board and by the way I want you to make it 62 mils thick I laughed at him and said no we're gonna mount it on four screws on standoffs why does it have to be 62 mils thick and he scratched his beard for a while and looked at me when god you're right it doesn't have to be 62 mils he said we've just always done that so I just assumed you know understand unless there's a mechanical reason driving it there's no reason to do that good thank you yes please do you have my email please direct any questions to me and I'm busy as heck so I may not get to them immediately but I will answer them eventually right thank you we're done

Channel: Altium

Views: 94,734

Rating: 4.9656444 out of 5

Keywords: rick hartley, altium, grounding, emi, live training

Id: ySuUZEjARPY

Length: 139min 29sec (8369 seconds)

Published: Mon Nov 11 2019

Reddit Comments

[u/phils94]

Possibly the best PCB-related video I‘ve ever watched and well worth the ~2hrs. Honestly changed the way I designed (and thought about) PCBs.

[u/mroebuilds]

attended some of his lectures, legit guru

[u/alfgan]

watched this video about 5 times and every time I learn something new

[u/zarx]

This is great. Changing the perspective from charges moving through conductors to fields moving between them, really transformed my thinking of PCB layout and design.

[u/coherentpa]

I have a love/hate relationship with Rick...

[u/zarx]

One thing I'm confused about - 4-layer stackup, the top layer usually has signals and poured ground, which is referenced to the GND layer just below. He advocates instead putting the GND layer on the top and signals just below.

I understand the benefit from having GND on the outside, but now every signal trace needs a via, and (unless I use blind vias) this via has to extend all the way through all layers. If you're using all the pins of a chip, now your planes are all chopped up with vias. This seems troublesome to me; wouldn't it be better to minimize the vias used?

[u/IKnowWhoYouAreGuy]

Saw the other post mentioning it :) Good work

[u/cholz]

Great stuff!

[u/wongsta]

I also posted this to /r/electronics, and there was a comment stating "...at the beginning he confuses grounding with bonding in regards to safety electrical installations...." (it's a long comment with a link to a video) which I thought was worth linking here.