-
- News
- Books
Featured Books
- design007 Magazine
Latest Issues
Current IssueSignal Integrity
If you don’t have signal integrity problems now, you will eventually. This month, our expert contributors share a variety of SI techniques that can help designers avoid ground bounce, crosstalk, parasitic issues, and much more.
Proper Floor Planning
Floor planning decisions can make or break performance, manufacturability, and timelines. This month’s contributors weigh in with their best practices for proper floor planning and specific strategies to get it right.
Showing Some Constraint
A strong design constraint strategy carefully balances a wide range of electrical and manufacturing trade-offs. This month, we explore the key requirements, common challenges, and best practices behind building an effective constraint strategy.
- Articles
- Columns
- Links
- Media kit
||| MENU - design007 Magazine
AltiumLive Frankfurt 2019: Rick Hartley Keynote
November 25, 2019 | Pete Starkey, I-Connect007Estimated reading time: 8 minutes
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.
Page 2 of 2Testimonial
"Our marketing partnership with I-Connect007 is already delivering. Just a day after our press release went live, we received a direct inquiry about our updated products!"
Rachael Temple - AlltematedSuggested Items
Closing the Loop on PCB Etching Waste
09/09/2025 | Shawn Stone, IECAs the PCB industry continues its push toward greener, more cost-efficient operations, Sigma Engineering’s Mecer System offers a comprehensive solution to two of the industry’s most persistent pain points: etchant consumption and rinse water waste. Designed as a modular, fully automated platform, the Mecer System regenerates spent copper etchants—both alkaline and acidic—and simultaneously recycles rinse water, transforming a traditionally linear chemical process into a closed-loop system.
Driving Innovation: Depth Routing Processes—Achieving Unparalleled Precision in Complex PCBs
09/08/2025 | Kurt Palmer -- Column: Driving InnovationIn PCB manufacturing, the demand for increasingly complex and miniaturized designs continually pushes the boundaries of traditional fabrication methods, including depth routing. Success in these applications demands not only on robust machinery but also sophisticated control functions. PCB manufacturers rely on advanced machine features and process methodologies to meet their precise depth routing goals. Here, I’ll explore some crucial functions that empower manufacturers to master complex depth routing challenges.
Trouble in Your Tank: Minimizing Small-via Defects for High-reliability PCBs
08/27/2025 | Michael Carano -- Column: Trouble in Your TankTo quote the comedian Stephen Wright, “If at first you don’t succeed, then skydiving is not for you.” That can be the battle cry when you find that only small-diameter vias are exhibiting voids. Why are small holes more prone to voids than larger vias when processed through electroless copper? There are several reasons.
The Government Circuit: Navigating New Trade Headwinds and New Partnerships
08/25/2025 | Chris Mitchell -- Column: The Government CircuitAs global trade winds continue to howl, the electronics manufacturing industry finds itself at a critical juncture. After months of warnings, the U.S. Government has implemented a broad array of tariff increases, with fresh duties hitting copper-based products, semiconductors, and imports from many nations. On the positive side, tentative trade agreements with Europe, China, Japan, and other nations are providing at least some clarity and counterbalance.
How Good Design Enables Sustainable PCBs
08/21/2025 | Gerry Partida, Summit InterconnectSustainability has become a key focus for PCB companies seeking to reduce waste, conserve energy, and optimize resources. While many discussions on sustainability center around materials or energy-efficient processes, PCB design is an often overlooked factor that lies at the heart of manufacturing. Good design practices, especially those based on established IPC standards, play a central role in enabling sustainable PCB production. By ensuring designs are manufacturable and reliable, engineers can significantly reduce the environmental impact of their products.