Managing the challenges in RF/microwave designs: because of the growth in mixed-technology products, designers often can't use traditional PCB layout tools for RF, and RF tools won't work with non-RF circuits. So what's the solution?

Not long ago, a cell phone was a cell phone and a car sound system was just a car sound system. Today, the sound system and the cell phone are integrated via a Bluetooth RF link to provide built in hands-free functionality. More traditionally "pure" RF or analog/digital products are integrated system designs, with RF systems embedded as "system on board," and all technologies sharing a rapidly shrinking board space. This is true not only for consumer products, but for defense and aerospace applications and all varieties of designs.

Anyone who has placed a cell phone close to an office phone or a sound system is aware of how easily unwanted RF energy can be coupled into other systems. If a cell phone three feet away from another system can ruin that system's performance, how can RF circuits be placed on the same board as other circuits? For one thing, it leads to a completely new set of design requirements. And managing RF system design--which very much includes managing EMI/EMC--has become a critical focus area.

But performing RF design in a traditional CAD environment causes severe pain. And at the same time, specialized RF design tools cannot be used as the sole solution, because most RF circuits must coexist with substantial sections of digital/analog technology. Moreover, the interdependent challenges involved have made the design of RF system boards a slow and highly iterative process. This is unacceptable, and there is a strong focus on streamlining the process with tools that understand the characteristics of RF and that supply automation in critical areas.

There are a number of separate tasks to manage, each with its own issues. These include:

* Design the RF circuitry and layout.

* Instantiate the RF circuitry in schematic and layout.

* Isolate/separate RF from non-RF circuitry.

* Manage power and grounds.

* Analyze couplings and parasitics.

* Design rule check (DRC).

To facilitate effective RF design, layout tool functionality is extended with drafting, snapping and align features more commonly found in mechanical design systems. Without them, RF design becomes a painfully slow task.

For many types of designs, a strictly schematic-driven flow is optimal. But since RF design is a very iterative process, with the circuit often being designed as it's being laid out on the board, a schematic-driven flow is not always best. On top of that, purely layout-driven design is not feasible either, because we have large non-RF sections in the same design. The solution often used is a mixed schematic/layout-driven design flow where non-RF circuits are driven from the schematic and selected parts of the RF circuitry are designed bottom-up, directly in the layout tool.

RF interference

With the basic design foundation in place, managing electromagnetic interference (EMI) becomes the next major complexity to manage. EMI is all unwanted coupling of signal energy within a design or between the design and other systems.

After years of high-speed challenges, many designers have become experienced at controlling crosstalk and achieving signal integrity. A key to their success is a good understanding of how signal currents flow on a board. With a signal propagating down a trace, there has to be a return current to form a closed circuit. What we have learned is that the return path tries to find the way back that has the least impedance. In a low-speed design this was the same as the path of least resistance or typically a straight line, but a high-speed signal will have the path of least inductance, which typically is right under the trace in the ground plane.

Managing return paths allows designers to control unwanted coupling and radiation/susceptibility as the amount of radiation is proportional to the loop area formed by the conductor and its return path. Furthermore, if two signals share the return path, energy from one signal may be coupled into the other in the form of common impedance coupling. So knowing where the return path is, making sure the loop area is minimized and making sure that two critical signals don't share the return path--at the same time--is always at the back of the high-speed designer's mind.

With RF circuitry, the signal typically returns by way of the path of least capacitance. This is a complicating factor, as it actually may include any conductive surface in reasonable proximity, such as a neighboring shield box or a metal cabinet. For this reason, RF function blocks are kept compact, with different blocks separated by grounded compartments, and RF specialists use small capacitors to control RF grounding and return paths. Avoid having a circuit's input and output stages share a return path, as we otherwise risk causing enough feedback coupling (from the higher power output stage to the sensitive input stages) to cause oscillation.

Ground Via Fences

Having created ground shields and ground planes, it is common to generate arrays (peppering with vias) or fences of vias (contour stitching) connecting the planes together. Why do we do this? Often we hear vague explanations like "It will make the ground better/tighter" or "It will stop RF leaks."

The real reason for these techniques may not be well understood. There is little research available, but the included references provide some good information.

For all of you RF designers who just pepper with vias without really knowing why, read on. Because we almost never have a single ground layer, designers pepper the ground areas with vias and stitch the edges of ground areas with vias to avoid coupling. This coupling is due to the parallel ground planes' being excited into the so-called parallel plate mode, letting signals propagate between the two planes. The vias are shorting the planes together, preventing this propagation mode in the ground plane. (1) Via fences at very high frequencies behave as band pass filters and the via-to-via spacing controls the pass band poles and thereby the cut of frequency of the filter. (2) Hence the via-to-via spacing is very important.

The center frequency of the band pass filter is shown in FIGURE 1: a function of via diameter, via spacing and dielectric material. (1) ([epsilon]r is the relative permittivity of the dielectric material; c is the speed of light.)

[FIGURE 1 OMITTED]

The center frequency is not the same as the usable upper limit. The space enclosed by four via holes is cavity that resonates at about 0.65 times the center frequency, and we have to keep our RF frequencies out of that region. (1) In other words, how we insert the vias, their pitch and diameter have a great impact on their effectiveness at preventing unwanted coupling in our design.

This leads to bow the ground vias are to be inserted in the layout. Manually inserting many thousands of ground vias, only to move them when the design is to be changed, is not a feasible solution. On the other hand, this is precisely what EDA tools are for: providing design automation. With routines that can trace objects and automatically insert multiple row via fences, understanding the boundaries of a ground fill and peppering its surface with ground-assigned vias saves tremendous time. By recognizing the resonance effects from ground vias, one can let the tool apply a random variance to the via pattern to avoid having all via-formed cavities resonating at the same frequency.

FIGURE 2 shows a contour stitching and a surface via pepper with random variance applied. Although these vias also form cavities, the cavity sizes are randomly different, giving different resonance frequencies for every little section of the planes.

[FIGURE 2 OMITTED]

At this point we have the circuit under control but are still missing a critical part: power supply. In the old days, RF compartments were closed metal cabinets connected to ground. Every signal and power source entering or leaving such a compartment was passed through a feed-through capacitor, basically a conductor with a coaxial capacitance grounded to trap any RF that tried to escape. RF chokes, typically one quarter wavelength of wire wound as a coil, were connected in serial to further limit RF leaks. Needless to say, this was a very expensive way to build; today's integrated board compartments are much more practical. However, now we can't use feed-through capacitors, which theoretically provide an almost perfect decoupling with low inductance, and we need to decouple interconnects more carefully to prevent RF leaks via power and low-frequency lines in the design.

With the RF section designed on a mixed technology board, it becomes important to be able to analyze whether non-RF structures in the design have a negative impact on the RF structures and vice versa. The RF circuit may or may not originate from an RF design and simulation tool. But no matter what, there is now a need to define regions around the RF circuits, including surrounding non-RF circuitry, and send the entire region into the RF analysis tools for a detailed analysis.

Because of this, the integration requirements between layout tools and analysis tools have increased dramatically. With an analysis tool link that preserves model and parameter data through a tool round-trip and still allows inclusion of non-RF board features, the RF engineer can verify the design without using the very slow manual modeling process.

DRC For RF

Why is DRC a naughty word in RF design? In many aspects, this is where using traditional PCB layout tools for RF design becomes painful. If the design only contained a bit of RF, a skilled RF designer would scrutinize the layout manually and make sure all is well. But today's RF designs have not only very complex and large RF sections but also large sections of analog and digital circuits.

We can safely say that signals behave very differently in the RF world than they do in the not-so-high-frequency world: With RF, the signal wavelength in relation to the length of the conductors on the circuit board is such that resonance and standing waves can occur. This fact is used to generate passive RF components as metal patterns on the board. These metal patterns connect to each other, and often to the ground, to form an RF circuit. To a classic analog digital design system, this would all look like a massive short-circuit. To make matters even worse, with a large number of nets shorted to ground, it's common that the remaining nets cannot be properly DRCed either, leaving us with a complex design that cannot be checked.

On the other hand, we cannot just pretend that the RF elements are nonconductive, because we need DRC to verify that the RF components also are properly connected to each other. The solution is to use a design system that can differentiate between RF structures and non-RF structures and provide DRCs that makes sense in each discipline.

Following the paradigm that every time you succeed in doing a design, the next one will be much worse, we can count on more integrated RF, more complex RF modules and with much higher frequencies making it even harder to control return paths and coupling.

The future of RE/microwave design will no doubt be harsh, but exciting.

REFERENCES

(1.) Takeshi Yuasa, Tamotsu Nishino, and Hideyuki Oh-hashi, "Simple Design Formula for Parallel Plate Mode Suppression by Ground Via-Holes in Multi-Layered Packages," Mitsubishi Electric  Corp., May 2001, Ofuna, Kamakura, Kanagawa, Japan.

(2.) Thorsten Tischler, Matthias Rudolph, Andreas Kilk, and Wolfgang Heinrich, "Via Arrays for Grounding in Multilayer Packaging--Frequency Limits and Design Rules," Ferdinand-Braun-Institut fur Hochstfrequenztechnik, Berlin, Germany.

PER VIKLUND is a product marketing manager at Mentor Graphics. He is responsible for RF, embedded components and advanced packaging solutions. Viklund can be reached at [e-mail].