-
-
News
News Highlights
- Books
Featured Books
- design007 Magazine
Latest Issues
Current IssueAll About That Route
Most designers favor manual routing, but today's interactive autorouters may be changing designers' minds by allowing users more direct control. In this issue, our expert contributors discuss a variety of manual and autorouting strategies.
Creating the Ideal Data Package
Why is it so difficult to create the ideal data package? Many of these simple errors can be alleviated by paying attention to detail—and knowing what issues to look out for. So, this month, our experts weigh in on the best practices for creating the ideal design data package for your design.
Designing Through the Noise
Our experts discuss the constantly evolving world of RF design, including the many tradeoffs, material considerations, and design tips and techniques that designers and design engineers need to know to succeed in this high-frequency realm.
- 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 2Suggested Items
The Evolution of Picosecond Laser Drilling
06/19/2025 | Marcy LaRont, PCB007 MagazineIs it hard to imagine a single laser pulse reduced not only from nanoseconds to picoseconds in its pulse duration, but even to femtoseconds? Well, buckle up because it seems we are there. In this interview, Dr. Stefan Rung, technical director of laser machines at Schmoll Maschinen GmbH, traces the technology trajectory of the laser drill from the CO2 laser to cutting-edge picosecond and hybrid laser drilling systems, highlighting the benefits and limitations of each method, and demonstrating how laser innovations are shaping the future of PCB fabrication.
Day 2: More Cutting-edge Insights at the EIPC Summer Conference
06/18/2025 | Pete Starkey, I-Connect007The European Institute for the PCB Community (EIPC) summer conference took place this year in Edinburgh, Scotland, June 3-4. This is the third of three articles on the conference. The other two cover Day 1’s sessions and the opening keynote speech. Below is a recap of the second day’s sessions.
Day 1: Cutting Edge Insights at the EIPC Summer Conference
06/17/2025 | Pete Starkey, I-Connect007The European Institute for the PCB Community (EIPC) Summer Conference took place this year in Edinburgh, Scotland, June 3-4. This is the second of three articles on the conference. The other two cover the keynote speeches and Day 2 of the technical conference. Below is a recap of the first day’s sessions.
Preventing Surface Prep Defects and Ensuring Reliability
06/10/2025 | Marcy LaRont, PCB007 MagazineIn printed circuit board (PCB) fabrication, surface preparation is a critical process that ensures strong adhesion, reliable plating, and long-term product performance. Without proper surface treatment, manufacturers may encounter defects such as delamination, poor solder mask adhesion, and plating failures. This article examines key surface preparation techniques, common defects resulting from improper processes, and real-world case studies that illustrate best practices.
RF PCB Design Tips and Tricks
05/08/2025 | Cherie Litson, EPTAC MIT CID/CID+There are many great books, videos, and information online about designing PCBs for RF circuits. A few of my favorite RF sources are Hans Rosenberg, Stephen Chavez, and Rick Hartley, but there are many more. These PCB design engineers have a very good perspective on what it takes to take an RF design from schematic concept to PCB layout.