AltiumLive Frankfurt 2019: Rick Hartley Keynote
Introduced by Lawrence Romine, Altium’s VP of corporate marketing, as a “low impedance presenter with a passion for his topic,” Rick Hartley delivered the opening keynote at the AltiumLive 2019 European PCB Design Summit in Frankfurt, Germany. His inspirational, relaxed style—founded on the wisdom of 50 years of experience in printed circuit design and his expertise in resolving noise, electromagnetic interference, and signal integrity issues—encouraged the packed audience to listen, observe, and understand.
“Now the learning begins!” Hartley recalled his first couple of years after graduation when he was able to get by on what he had learned in college, although it became increasingly apparent that there were things he didn’t understand. He had been accumulating knowledge ever since, through books, and by associating himself with brilliant people. Hartley’s reading was selective, however. For example, he believed there was little value in reading IC application notes; although they described the schematic function of the component, they were often written without an appreciation of the influence of board layout. An opinion Hartley had shared for many years with Lee Ritchey was, “Circuit application notes produced by IC manufacturers should be assumed wrong until proven to be right.”
Hartley had recognised that many designers and engineers didn’t fully understand the features of differential pairs used to create balanced transmission systems for carrying high-speed signals across PCBs, eliminating problems associated with ground returns. He made it clear that the rules for differential pairs were not the same in a PCB as they were in a cable or twisted pair of wires. In his keynote, entitled “What Your Differential Pairs Wish You Knew,” Hartley set out to discuss the advantages of differential pairs, which format gave the best impedance control, what was the right spacing between lines of a pair, what was important in differential pair routing, and how much skew was really acceptable.
“A couple of things to understand: The frequency of a circuit is not driven by the clock, but by IC output rise time. It’s all about the rate of change of energy with respect to time and has nothing to do with clock frequency,” Hartley declared. He continued, “Design to the rise time, which, by the way, you probably won’t find in the datasheet.” Hartley made special mention of a feature of Altium’s new tool that enabled the tweaking of line length based on timing: “It’s all about timing, not about length.”
Hartley displayed a table he had put together many years ago that indicated how long a transmission line could be, based on rise time, before it was necessary to pay attention to it. And there were differences in inner-layer and outer-layer lines because energy travelled faster on outer layers—another source of problems in matching line length. And with modern devices having rise times between 0.3 and 0.7 nanoseconds, any traces longer than 10–25 mm needed careful attention.
“Where does the energy travel in a circuit?” Hartley asked. Then, he answered his own question: “It’s in the electric and magnetic fields, not in the current and voltage.” Hartley added, “Where do the fields travel in a transmission line? In the plastic of the PCB, or in the plastic between the wires of a twisted pair, and the air around it. Because all the energy is in the fields, and if they move position, they’re going to couple energy into other things. That’s why we have electromagnetic interference. Forget voltage and current and start thinking about the fields.”
Hartley illustrated a transmission line—a pair of conductors that moved energy from A to B—and reiterated that the energy moved in the dielectric space; the voltage was across the copper features, and the current was in the copper features. The fields travelled in the dielectric space between the line and what he had shown as a ground plane. Energy did not come from the power plane; it came from the dielectric space between the power plane and ground, which was a reason for putting power and ground as close as possible to each and avoiding routing signals in between them.
In its most basic form, a differential pair was two single-ended signals, containing equal amplitude and usually opposite polarity fields. It was not “special” in any other respect than that it ignored ground offsets. And the receiver was simply a crossing detector, a differential-input amplifier. Most of the coupling from each of the lines was to the plane below, not to the other line. The amount of coupling between them was a function of how far apart they were, but it was not necessary to have them really close together. In fact, it was irrelevant; the main reason for routing them together was so that they would be about the same length so that they would cross in the linear region of the rising and falling edges.
Each line had its own impedance relative to ground, and the fields that coupled between them defined Z-coupling. As an example, two lines that were 65 ohms each, and close enough together to have 15 ohms coupling between them, would constitute a 100-ohm differential pair. If the lines were 55 ohms, and further apart so that there was only 5 ohms of coupling, they would still constitute a 100-ohm differential pair. If they were moved so far apart that they had no coupling, they would still constitute a 100-ohm differential pair because they would be two single-ended signals within the PCB operating independently of each other. And whether or not they lined up mattered only when going through a non-grounded connector, and at the receiver.
Tight coupling did create different line widths: the advantage with tight coupling was that it gave a narrower line for a given impedance, which made the design easier to route. The disadvantage with tight coupling was that it gave a narrower line for a given impedance, which made the design more difficult to manufacture and hence more expensive. And there were signal integrity issues associated with skin effect; sometimes, separating differential lines by greater distances and making the lines wider could be justified for reasons of signal integrity and/or cost of manufacturing.
Hartley discussed crosstalk between tightly-coupled lines sandwiched between planes, where interference from the outside world was reduced because high-frequency fields would not conduct through copper planes. But the close proximity of an aggressive signal on the same layer would result in unbalanced crosstalk, however tightly the differential pair were coupled.
Hartley also made some interesting comments about skew, which, in his opinion, was not nearly as critical as stated in the application notes. He went on to say that he never length-matched the two lines of a differential pair, even at 10-gigahertz frequencies; instead, he ran them side by side, made them approximately the same length, and they had always worked. It was much more important to reference ground on the next layer of the board.
What else could impact timing skew? Board materials. As signals travelled through the dielectric of the composite material, and the dielectric constants of epoxy and glass were different, they travelled at different speeds as they crossed the weave of the glass cloth, and the two lines of the differential pair were always effectively jockeying for position. Hartley named glass styles 1080 and 106 as the worst for this effect because of the width of spaces in the weave could result in 5 mm of skew in 75 mm of routing in a typical example, putting a different perspective on the concept of length matching and causing real signal integrity problems in high-speed designs. The message was to choose one of the newer spread-glass styles designed to minimise this effect, although there could still be some electromagnetic interference issues.
Hartley stressed that one of the biggest causes of electromagnetic interference was changing layers, and he showed an example of a signal line on layer 1 of a circuit board traversing a ground-plane on layer 2 through a via to a signal layer 3. The energy in that circuit was in the dielectric space between layer 1 and the ground-plane layer 2. If it was necessary to change layers in order to change routing direction from X to Y, then the fields would couple through the clearance hole in the plane, the fields would continue on in the dielectric space between layers 2 and 3, and everything would work perfectly with no danger of spreading fields and no electromagnetic interference problems. And for the most part, signal integrity would be maintained.
But if the fields spread out and there were other vias in that region, they would couple into those other vias, and there was a strong possibility of introducing electromagnetic interference. And if it was necessary to go from one ground plane to another, the best way to do it was to place a ground via next to it. Hartley discussed various field-spreading and coupling effects and their consequences and commented that he spent most of his consulting time solving electromagnetic interference problems, admitting that his job was so easy because the majority could be resolved simply by adding return vias or changing positions of decoupling capacitors.
People wouldn’t need to hire Hartley if they would take the trouble to gain some basic knowledge “There is no current inside of a via,” was another forthright statement. The beauty of the fields was that the return current was on the outside of the via barrel. Therefore, contrary to popular opinion, there was no justification to fill the via with conductive material; “You could use peanut butter; it doesn’t matter electrically.”
What about differential pairs? Was a return via necessary when transitioning layers? A lot of people believed not. But Hartley depicted them as two single-ended signals, referencing the plane above or below, rather than them having magical, mystical properties because they were a differential pair. Without a return via, their fields would spread in exactly the same way as a single-ended signal, and create a common-mode current in one or the other line. He illustrated the best way to change layers with a differential pair using a pair of vias, or even a single via: “But you have to take the fields through the dielectric from one dielectric layer to the next. You can’t just ignore the fields because when you do, you set yourself up for problems.”
Rick Hartley’s keynote set people thinking. He had blown away a lot of popular mythology and could support his statements and design principles with factual examples drawn from many years of practical experience. The Q&A session ran for some time.