Printer Friendly

Integrating RF into PCB design: in RF designs, it's important to identify and correct circuit interactions as the system design evolves to reduce cycle time and prevent unnecessary re-spins.

Today, RF (radio frequency) circuitry is sneaking into more and more products. As this happens, more designers are faced with allowing RF circuitry to share board space with other technologies such as high-speed digital and analog circuits.

The combination of RF and non-RF circuitry in close proximity can cause a lot of pain to design teams. Multiple design iterations and very long design times are common. Traditional design techniques have not been very helpful as they typically focus on RF alone and don't consider the interactions of the complete system.

In this article, we will take a practical look at modern RF design in the context of a complete system and see how careful planning and design can significantly improve the success rate, as well as shorten design times.

RF design can be painful, especially so when seen in the context of system design. Why is that? In the past, RF was typically isolated modules--boards with solely RF content. Today, we combine all kinds of technology on the same dense board, and as dimensions are constantly shrinking, the risk of interaction between technologies, such as high-speed digital and RF, increases.

Currently, this interaction cannot fully be avoided. We are typically not able to design out all interactions but are instead faced with designing a system with interaction but not more than the circuit can accept and still perform as intended. With this in mind, we can identify three areas of interest (each topic could fill a book or more):

Design methodology. How to best design a mixed-technology product.

Circuit interaction. How to manage the interaction between modules of different technologies.

Verification. How to verify and validate a mixed-technology design.

Design Methodology

Today's methodologies go back over 10 years when RF design was a different ball game. In the classic flow, the RF designer is a contributor of technology that eventually will end up on a circuit board. The RF modules are designed in a dedicated RF design solution and, when ready, transferred to the system PCB layout using design translation.

The benefit of this method is that the designer can focus on the RF by itself, not bothered by non-RF issues, and there are cases where this is a real advantage. The downside is that the RF engineer can't see the impact he may cause or what will be affected by other circuits, and he stays as a contributor while the desired situation, in this case, is a team player role.

For multi-technology designs, much can be gained in a methodology where all technologies can be co-designed in a manner where everyone is a team player rather than module contributors. By providing a collaborative environment, concurrent design teams can design their technology in parallel while being aware of what is being designed by other teams, thus eliminating some re-spins.

Circuit Interaction

Multi-technology design is about circuits living in harmony. You avoid being a noisy neighbor, and you don't walk in your neighbor's garden. The issue is that the circuits are becoming noisier. Plus, they are placed closer together than in the past ... a trend that will continue no matter what.

Hence, circuits do impact each other, and the challenge is to manage how and how much so the circuits still perform as specified. There are several areas impacting the interaction; the most obvious one is parts placement. Unfortunately, parts placement is not free since everything has to fit, and each technology has specific placement requirements.


Unwanted Coupling

We also have to deal with unwanted coupling. Unwanted coupling is any coupling of energy from one system to another where it is not intentionally designed as a part of the circuit.

There are several sources or "entries" for unwanted coupling: the most obvious path is direct coupling in the form of inductive and capacitive coupling between signal conductors. Today, it is commonly understood that wide traces at narrow spacing far from ground will have large mutual capacitance and inductance and, hence, be able to couple energy between them. Since this is obvious, it becomes second nature to control this direct coupling.


The really nasty and sneaky scoundrel is indirect coupling from the power/ground system, and signal return paths. In a circuit schematic, we only draw the signal paths, and the return path is implicit. Everyone knows that a return path is needed, or the circuit remains open and will not work. You don't typically wire them as you do with signal conductors. They appear indirectly as a consequence of your wiring and the design of your power/ground system. The smart thing about return paths is that the circuit will find one if one exists, or we would have an open circuit. The bad thing is that if this return path is not where you want it to be, you can (most likely will!) get into trouble.

This means that, to be successful, we must change from "indirect" creation of return paths to actively considering return paths in the design work. For every routed signal, we have to ensure that we have a proper return path that is located where we want it and that we don't obstruct already created paths, because signals sharing a part of the return path have common impedance coupling (energy coupled from one signal to the other).

The larger the area spanned by signal and return path, the larger the radiation and susceptibility. (EMI is proportional to the loop area.)

Where is the Return Path?

At DC, the return path is a straight line (path of least resistance), but as frequency increases, we cannot simplify and just say "the path of least resistance" anymore. It is in fact the path of least impedance. At the low to medium-high frequency of the digital high-speed spectrum, inductance is the dominating part of impedance. Therefore, we can somewhat simply say that the return path is the path of least inductance.

In today's circuit boards, this path is usually in the ground plane right under the signal conductor. This deviates only if there are obstacles in the form of a slotted or split ground plane or where vias perforate the ground plane enough to cut the return path.

At RF frequencies (this includes ultra-high-speed digital), capacitance becomes dominant. Thus, the signal will typically find its return path as the path of least capacitance. This makes things extremely complicated as the path of "least capacitance" is not as predicable as for inductance. It may very well include any conductive surface in proximity, such as shield boxes or a metal cabinet. At the same time, the return path is really critical to circuit function. We need to establish where the path is and that it is not shared for two sensitive signals to avoid common impedance coupling between them.

The key to controlling indirect coupling is proper grounding. Obviously, we don't want RF and digital (or analog) to share return paths. This is why we work with separate grounds. Connecting all ground in a single point helps ensure that the return paths are not shared between the systems. However, within the same ground system, we need to manage the return paths--keeping in mind the rule that it will be the path of least impedance for the frequency with which we are working.

Power Feed Leaks

Return path and separate grounding helps, but in an RF system, we also need to ensure that RF energy must not leak onto the power supply itself and radiate or cause other problems there.

When I started doing RF design, we used closed metal cabinets for each module, with each cabinet carefully grounded. We used so-called feed-through capacitors for every signal or power entering or leaving the shielded compartment. This was a conductor with a coaxial capacitance to ground intended to short circuit any RF energy trying to escape. We also used RF chokes made of a quarter-wavelength of wire wound as a coil. Connected in a series with power or LF lines, they acted as a high-impedance obstacle to further limit RF leaks.

Today, this is too cumbersome of an approach, and integrated board compartments are more practical replacements. We still need to decouple interconnects very carefully to prevent RF leaks via power and low-frequency lines in the design.

Ground Fences

In RF system designs, we frequently see each module in the design encapsulated by a narrow ground guard stitched with via holes: either a single row of vias or a dual staggered row. When designers are asked why they use a certain via spacing or pattern, the answer often includes wind direction and shoe size. Luckily, some work has been published on this topic; so there is no reason to resort to black magic.

We can use via fencing for both power lines" and signal lines. As we all know, currents in power planes are overlaid with transients. This can make the power bus radiate the same way as a microstrip patch antenna (1).

Xin Wu et al. suggest that setting the via spacing in the fence to less than 1/10th wave length can give up to 25 dB suppression compared to no fencing (1).

You would think that the closer a via fence is placed to an RF line the better. However, when placed too close, the radiation losses increase. This will actually increase the coupling (2). As a rule of thumb, the via fence must be set away from the RF trace by at least four times the distance between the signal layer and the ground layer of a multilayer PCB (2).


FIGURE 1 shows the field distribution for a stripline with widely spaced via fencing. The vias are 1X height over ground away from the strip line, and the via spacing is 5.2X height over ground. The radiation losses are clearly visible.

FIGURE 2 shows the same strip with a much narrower via spacing of 1.3X height over ground. The radiation losses are significantly lower here. Dr. Ponchak (recommended reading on this topic!) suggests that the smaller the via spacing, the better (2). A solid wall would be ideal if it could be manufactured.

In RF systems, we also need to manage the ground and power planes. We have already covered that the currents on these planes have a transient component and that transient currents through a conductor mean radiation, which we obviously don't want. This leads us to via peppering of power/ground planes. Again, we have an area ruled by "black magic;" "This is what we've always done so it must be good ..." Still, there are some published papers that can help us better understand what really happens to the power and ground planes.

If we inject a current between two parallel plates, they will radiate due to something called parallel plate excitation that allows signals to propagate between the plates. Trust me, if the "parallel plates" are your ground plane, you will want to suppress this. Typically, we have multiple ground layers, and we pepper the ground areas and stitch the edges of ground areas with vias to short the planes together preventing this propagation mode in the ground plane. (3)

Interestingly, via array acts as band pass filters at high frequencies. The via to via spacing controls the pass band poles, and we will soon see that the via-to-via spacing is very important (4).

Takeshi Yuasa et al. have found the pass band frequency to be as shown in FIGURE 3 where r is the relative permittivity of the dielectric material, and c is the speed of light, a function of via diameter, via spacing and dielectric material (3). However, this calculated frequency is not the same as the usable upper limit!

The space enclosed by four via holes forms a cavity, which will resonate at about 0.65X the center frequency (Fc) (3). This becomes the real upper limit. At resonance, the grounding effect of the via array is lost, and the structure will no longer prevent the parallel plate mode excitation. From this, it is clear that how we arrange the vias, their diameter and their pitch is important, and does impact the effectiveness of the via fencing and via peppering.


In a classic RF design flow, RF modules are simulated in the RF design environment (initially), not taking into account the actual PCB implementation. Verification includes repeating that simulation, but now with all known PCB features included, such as surrounding non-RF signals, metal planes and shapes, via stitching, via peppering and other techniques. Ideally, the differences in simulation results are negligible, but the reality is that serious issues are always found. The tool integrations of the traditional flow make it very cumbersome to set up and run this type of simulation with incremental updates while the circuit design and layout are in progress. Typically, Gerber, DXF or GDS-II files are used, which means that all design intent is lost in the interface due to primitive data formats.

New methodologies combined with new design tools that use a more elegant integration, where design data keeps its "intelligence," make it possible to keep the intent of the design and run repeated simulations very quickly.

This makes it possible to quickly identify problems caused by circuit interaction and correct them as you go along in a "correct by design" flow. Interactions will happen. Identifying and correcting these interactions as the system design evolves, rather than in the end, offers the potential to yield much shorter design cycles and fewer of those cycles. This is because the earlier the issues can be identified, the easier they can be corrected. Making substantial changes to a dense and complete design can take a very long time.


(1.) Wu, Xin, Mahammad H. Ke~mani and Omar M. Ramahi. "Mitigating Multilayer PCB Power Bus Radiation Through Novel Mesh Fencing Techniques:' Mechanical Engineering Department, Electrical and Computer Engineering Department, and CALCE Electronic Products and Systems Center, University of Maryland College Park, MD.

(2.) Ponchak, George E., Donghoon Chen, Jong-Gwan Yook, and Linda P. B. Katehi. "Characterization of Plated Via Hole Fences for Isolation Between Stripline Circuits in LTCC Packages," IEEETHIF61.

(3.) Yuasa, Takeshi, Tamotsu Nishino, and Hideyuki Oh-hashi. "Simple Design Formula for Parallel Plate Mode Suppression by Ground Via-Holes," Mitsubishi Electric Corp., 5-1-10funa, Kamakura, Kanagawa, 247-8501 Japan.

(4.) Tischler, Thorsten, Matthias Rudolph, Andreas Kilk, and Wolfgang Heinrich. "Via Arrays for Grounding in Multilayer Packaging Frequency Limits and Design Rules, Ferdinand-Braun-Institut fur Hochstfrequenztechnik (FBH), D-12489 Berlin, Germany.

PER VIKLUND is director of IC packaging & RF with Mentor Graphics, Systems Design Division; per_viklund@
COPYRIGHT 2007 UP Media Group, Inc.
No portion of this article can be reproduced without the express written permission from the copyright holder.
Copyright 2007 Gale, Cengage Learning. All rights reserved.

Article Details
Printer friendly Cite/link Email Feedback
Title Annotation:RF DESIGN
Author:Viklund, Per
Publication:Printed Circuit Design & Fab
Date:Dec 1, 2007
Previous Article:Plating voids, Part 2: careful control of the drilling can lead to improved plating quality.
Next Article:Benefits of implementing differential pairs: when using differential circuits, specific, design rules can maximize the advantages while minimizing...

Related Articles
Trending toward profitability: there's money to be made through efficient PCB design. But you'll have to extract every spare second and dollar to do...
Managing the challenges in RF/microwave designs: because of the growth in mixed-technology products, designers often can't use traditional PCB layout...
Technical conference.
Virtual RF: PCB prototypes: gone are the days when designers had to jury-rig layout tools to do RF designs. Now, even virtual RF prototypes are...
Microminiaturization, Motorola style: enabling wickedly compelling mobile devices with greater functionality and elegant form factors.
Design reuse software tool.
Effectively managing RF design in utility metering applications EMS companies can be the missing link between meter expertise and distribution.

Terms of use | Privacy policy | Copyright © 2020 Farlex, Inc. | Feedback | For webmasters