DesignCon: The Place to Go to Find Out What You Don’t Know You Don’t Know
In engineering, it’s what you don’t know you don’t know that can ruin your day and keep you awake at nights. Especially after you get your prototypes in the lab, or worse, field returns from the customer. This is one reason why I have been going to DesignCon for the last few years, and this year has been no exception.
One of the sessions I attended was the Power Integrity Boot Camp, hosted by Heidi Barnes, from Keysight Technologies, and Steve Sandler from Picotest. What I didn’t know I didn’t know from this boot camp was how important it was to match the voltage regulator module (VRM) output impedance to the power distribution network (PDN) input impedance. Steve and Heidi recently presented a webcast which was a condensed version of the DesignCon Bootcamp session. If you are involved in PDN design, this webcast will provide you with an introduction to power integrity and give some insight into the latest tips and techniques to achieve flat impedance designs.
Of course, I always try and attend some of Eric Bogatin’s presentations because I always come away with something I didn’t know I didn’t know. Eric is an Adjunct Professor at the University of Colorado and the Dean of Teledyne LeCroy’s SI Academy. He was honored at this year’s DesignCon with a welldeserved Engineer of the Year Award.
The speed training event, he hosted along with Larry Smith from Qualcomm, was on the top of my list to attend. During the session, Eric described the most critical feature of PDN design was controlling the “Bandini Mountain”.
The Bandini Mountain expression has often been used to describe a tall pile of manure. Originally it referred to a 100 foot tall mound of fertilizer built by the Bandini Fertilizer Company in California prior to the 1984 Los Angeles summer Olympics for advertisement purposes. When the company went bankrupt, this large mound of smelly fertilizer was left behind and everyone wished it would go away.
Because of this little bit of trivia, it was the term coined by the late Steve Weir to describe the large resonant frequency peak formed by the parallel combination of the on die capacitance and the package lead inductance, as seen from the die looking into the PDN. This peak is inherent in all PDN networks, and almost impossible to get rid of. And like the Bandini Mountain, it was something PDN designers wish could go away.
Steve used to be a regular Icon at past DesignCons until his sudden passing in August 2015. Steve was one of the smartest guys I knew, and I always looked forward to catching up with him when I visited DesignCon. If you knew Steve, like many of us did, you know that he often had very humorous analogies to describe empirical or simulated results. This example is no exception. He will be sorely missed for his contribution the engineering community.
What I learned I didn’t know I didn’t know from Eric’s and Larry’s presentation was that every PDN design will have a “Bandini Mountain”, and unless you know what frequency it is at, and take steps to try and mitigate its peak, it could ruin your day! Even though the system seems to “work” in the lab, it doesn’t mean it’s robust enough and won’t fail under certain operating conditions in the field that affect the transient currents.
Eric has made available the speed training slides and the associated video off his SI Academy web site. If you look under Video Recordings, Presentations and Webinars (VRPW) and scroll down to the bottom you will find the slides titled, “VRPW6035 DesignCon 2016 PDN speed training”. If you watch the whole presentation you will learn all about the “PDN Bandini Mountain” and techniques to mitigate its effects. And while you are there, have a look at the many other videos and presentations available for free and by paid subscription.
Eric and Larry have also coauthored a new book, scheduled for release in June 2016 titled, “Principles of Power Integrity for PDN Design”. I can’t wait to buy this book to add to my library so that I can find out more of what I don’t know I don’t know about PDN design. If it’s anything like Eric’s other books, I won’t be disappointed.
Practical Conductor Roughness Modeling with Cannonballs
In the GB/s regime, accurate modeling of conductor losses is a precursor to successful highspeed serial link designs. Failure to model roughness effects can ruin you day. For example, Figure 1 shows the simulated total loss of a 40 inch printed circuit board (PCB) trace without roughness compared to measured data. Total loss is the sum of dielectric and conductor losses. With just 3dB delta in insertion loss between simulated and measured data at 12.5 GHz, there is half the eye height opening with rough copper at 25GB/s.
So what do cannon balls have to do with modeling copper roughness anyway? Well, other than sharing the principle of close packing of equal spheres, and having a cool name, not very much.
According to Wikipedia, closepacking of equal spheres is defined as “a dense arrangement of congruent spheres in an infinite, regular arrangement (or lattice)” [8]. The cubic closepacked and hexagonal closepacked are examples of two regular lattices. The cannonball stack is an example of a cubic closepacking of equal spheres, and is the basis of modeling the surface roughness of a conductor in this design note.
Figure 1 Comparisons of measured insertion loss of a 40 inch trace vs simulation. Eye diagrams show that with 3dB delta in insertion loss at 12.5GHz there is half the eye opening at 25GB/s. Modeled and simulated with Keysight EEsof EDA ADS software [14].
Background
In printed circuit (PCB) construction there is no such thing as a perfectly smooth conductor surface. There is always some degree of roughness that promotes adhesion to the dielectric material. Unfortunately this roughness also contributes to additional conductor loss.
Electrodeposited (ED) copper is widely used in the PCB industry. A finished sheet of ED copper foil has a matte side and drum side. The drum side is always smoother than the matte side.
The matte side is usually attached to the core laminate. For high frequency boards, sometimes the drum side of the foil is laminated to the core. In this case it is referred to as reversed treated (RT) foil.
Various foil manufacturers offer ED copper foils with varying degrees of roughness. Each supplier tends to market their product with their own brand name. Presently, there seems to be three distinct classes of copper foil roughness:
· Standard
· Verylow profile (VLP)
· Ultralow profile (ULP) or profile free (PF)
Some other common names referring to ULP class are HVLP or eVLP.
Profilometers are often used to quantify the roughness tooth profile of electrodeposited copper. Tooth profiles are typically reported in terms of 10point mean roughness (R_{z }) for both sides, but sometimes the drum side reports average roughness (R_{a }) in manufacturers’ data sheets. Some manufacturers also report RMS roughness (R_{q }).
Modeling Roughness
Several modeling methods were developed over the years to determine a roughness correction factor (K_{SR }). When multiplicatively applied to the smooth conductor attenuation (α_{smooth }), the attenuation due to roughness (α_{rough }) can be determined by:
Equation 1
The most popular method, for years, has been the Hammerstad and Jensen (H&J) model, based on work done in 1949 by S. P. Morgan. The H&J roughness correction factor (K_{HJ }), at a particular frequency, is solely based on a mathematical fit to S. P. Morgan’s power loss data and is determined by [2]:
Equation 2
Where:
K_{HJ} = H&J roughness correction factor;
∆ = RMS tooth height in meters;
δ = skin depth in meters.
Alternating current (AC) causes conductor loss to increase in proportion to the square root of frequency. This is due to the redistribution of current towards the outer edges caused by skineffect. The resulting skindepth (δ ) is the effective thickness where the current flows around the perimeter and is a function of frequency.
Skindepth at a particular frequency is determined by:
Equation 3
Where:
δ = skindepth in meters;
f = sinewave frequency in Hz;
μ_{0}= permeability of free space =1.256E6 Wb/Am;
σ = conductivity in S/m. For annealed copper σ = 5.80E7 S/m.
The model has correlated well for microstrip geometries up to about 15 GHz, for surface roughness of less than 2 RMS. However, it proved less accurate for frequencies above about 5GHz for very rough copper [3] .
In recent years, the Huray model [4] has gained popularity due to the continually increasing data rate’s need for better modeling accuracy. It takes a real world physics approach to explain losses due to surface roughness. The model is based on a nonuniform distribution of spherical shapes resembling “snowballs” and stacked together forming a pyramidal geometry, as shown by the scanning electron microscope (SEM) photo in Figure 2.
Figure 2 SEM photograph of electrodeposited copper nodules on a matte surface resembling “snowballs” on top of heat treated base foil. Photo credit OakMitsui.
By applying electromagnetic wave analysis, the superposition of the sphere losses can be used to calculate the total loss of the structure. Since the losses are proportional to the surface area of the roughness profile, an accurate estimation of a roughness correction factor (KSRH) can be analytically solved by [1]:
Equation 4
Where:
K_{SRH} (f ) = roughness correction factor, as a function of frequency, due to surface roughness based on the Huray model;
A_{flat}= relative area of the matte base compared to a flat surface;
a_{i} = radius of the copper sphere (snowball) of the i^{th} size, in meters;
Ni = number of copper spheres of the i^{th} size per unit flat area in sq. meters;
δ (f ) = skindepth, as a function of frequency, in meters.
Cannonball Model
Using the concept of cubic closepacking of equal spheres, the radius of the spheres (a_{i }) and tile area (A_{flat }) parameters for the Huray model can now be determined solely by the roughness parameters published in manufacturers’ data sheets.
Why is this important? Well, as my friend Eric Bogatin often says, “Sometimes an OK answer NOW! is more important than a good answer late”. For example, often during the architectural phase of a backplane design, you are going through some whatif scenarios to decide on a final physical configuration. Having a method to accurately predict loss from data sheets alone rather than go through a design feedback method, described in [7] can save an enormous amount of time and money.
Another reason is that it gives you a sense of intuition on what to expect with measurements to help determine root cause of differences; or sanitize simulation results from commercial modeling tools. If you are like me, I always like to have alternate ways to verify that I have used the tool properly.
Recalling that losses are proportional to the surface area of the roughness profile, the Cannonball model can be used to optimally represent the surface roughness. As illustrated in Figure 3, there are three rows of spheres stacked on a square tile base. Nine spheres are on the first row, four spheres in the middle row, and one sphere on top.
Figure 3 Cannonball model showing a stack of 14 uniform size spheres (left). Top and front views (right) shows the area (A_{flat}) of base, height (H_{RMS}) and radius of sphere (r).
Because the Cannonball model assumes the ratio of A_{matte}/A_{flat} = 1, and there are 14 spheres, Equation 4 can be simplified to:
Equation 5
Where:
K_{SR} (f ) = roughness correction factor, as a function of frequency, due to surface roughness based on the Cannonball model;
r = sphere radius in meters; δ (f ) = skindepth, as a function of frequency in meters;
A_{flat} = area of square tile base surrounding the 9 base spheres in sq. meters.
In my white paper [16] the radius of a single sphere is:
And the area of the square flat base is:
You can approximate the RMS heights of the drum and matte sides by Equation 6 and Equation 7 below:
Equation 6
Where: R_{z_drum} is the 10point mean roughness in meters. If the data sheet reports average roughness, then R_{a_drum} is used instead.
Equation 7
Where: R_{z_matte} is the 10point mean roughness in meters.
Practical Example
To test the accuracy of the model, board parameters from a PCBDesign007 February 2014 article, by Yuriy Shlepnev [5] was used. Measured data was obtained from Simbeor software design examples courtesy of Simberian Inc. [9]. The extracted deembedded generalized modal Sparameter (GMS) data was computed from 2 inch and 8 inch singleended stripline traces. They were originally measured from the CMP28 40 GHz HighSpeed Channel Modeling Platform from Wild River Technology [14].
The CMP28 Channel Modeling Platform, (Figure 4 left credit Wild River Technology) is a powerful tool for development of highspeed systems up to 40 GHz, and is an excellent platform for model development and analysis. It contains a total of 27 microstrip and stripline interconnect structures. All are equipped with 2.92mm connectors to facilitate accurate measurements with a vector network analyzer (VNA).
The PCB was fabricated with Isola FR408HR material and reverse treated (RT) 1oz. foil. The dielectric constant (Dk) and dissipation factor (Df), at 10GHz for FR408HR 3313 material, was obtained from Isola’s isoStack® webbased online design tool [10]. This tool is a free, but you need to register to use it. An example is shown in Figure 5.
Typical traces usually have a trapezoidal crosssection after etching due to etch factor. Since the tool does not handle trapezoidal crosssections in the impedance calculation, an equivalent rectangular trace width was determined based on a 2:1 etchfactor (60^{ }deg taper). The as designed nominal trace width of 11 mils, and a 1oz trace thickness of 1.25 mils per isoStack® was used in the analysis.
Figure 5 Example of Isola’s isoStack® online software used to determine dielectric thicknesses, Dk, Df and characteristic impedance for the CMP28 board.
The default foil used on FR408HR core laminates is MLS, Grade 3, controlled elongation RT foil. The roughness parameters were easily obtained from Oakmitsui [11]. Reviewing the data sheet, 1 oz. copper roughness parameters R_{z} for drum and matte sides are 120μin (3.175 μm) and 225μin (5.715μm) respectively. Because this is RT foil, the drum side is the treated side and bonded to the core laminate.
An oxide or microetch treatment is usually applied to the copper surfaces prior to final lamination. This provides enhanced adhesion to the prepreg material. COBRA BOND® [12] or MultiBond MP [13] are two examples of oxide alternative microetch treatments commonly used in the industry. Typically 50 μin (1.27μm) of copper is removed when the treatment is completed. But depending on the board shop’s process control, this can be 70100 μin (1.782.54μm) or higher.
The etch treatment creates a surface full of microvoids which follows the underlying rough profile and allows the resin to squish in and fill the voids providing a good anchor. Because some of the copper is removed during the microetch treatment, we need to reduce the published roughness parameter of the matte side by nominal 50 μin (1.27 μm) for a new thickness of 175μin (4.443μm).
Figure 6 shows SEM photos of typical surfaces for MLS RT foil courtesy of Oakmitsui. The left and center photos are the treated drum side and untreated matte side respectively. The right photo is a 5000x SEM photo of the matte side showing microvoids after etch treatment.
Figure 6 Example SEM photos of MLS RT foil courtesy of Oakmitsui. Left is the treated drum side and center is untreated matte side. SEM photo on the right is the matte side after etch treatment.
The data sheet and design parameters are summarized in Table 1. Respective Dk, Df, core, prepreg and trace thickness were obtained from the isoStack® software, shown in Figure 5. Roughness parameters were obtained from Oakmitsui data sheet. R_{z} of the matte side after microetch treatment (R_{z} = 4.443μm) was used to determine K_{SR_matte }.
Table 1 CMP28 test board parameters obtained from manufacturers’ data sheets and design objective.
Parameter 
FR408HR 
Dk Core/Prepreg 
3.65/3.59 @10GHz 
Df Core/Prepreg 
0.0094/0.0095 @ 10GHz 
R_{z} Drum side 
3.048 μm 
R_{z} Matte side before Microetch 
5.715 μm 
R_{z }Matte side after Microetch 
4.443 μm 
Trace Thickness, t 
31.730 μm 
Trace Etch Factor 
2:1 (60 deg taper) 
Trace Width, w 
11 mils (279.20 μm) 
Core thickness, H1 
12 mils (304.60 μm) 
Prepreg thickness, H2 
10.6 mils (269.00 μm) 
GMS trace length 
6 in (15.23 cm) 
Keysight EEsof EDA ADS software [14] was used for modeling and simulation analysis. A new controlled impedance line (CIL) designer enhancement, in version 2015.01, makes modeling the transmission line substrate easy. Unlike earlier substrate models, the CIL model allows you to model trapezoidal traces.
Figure 7 is the general schematic used for analysis. There are three transmission line substrates; one for dielectric loss; one for conductor loss and the other for total loss without roughness.
Figure 7 Keysight EEsof EDA ADS generic schematic of controlled impedance line designer used in the modeling and simulation analysis.
Dielectric loss was modeled using the Svensson/Djordjevic wideband Debye model to ensure causality. By setting the conductivity parameter to a value muchmuch greater than the normal conductivity of copper ensures the conductor is lossless for the simulation. Similarly the conductor loss model sets the Df to zero to ensure lossless dielectric.
Total insertion loss (IL) of the PCB trace, as a function of frequency, is the sum of dielectric and rough conductor insertion losses.
Equation 8
To accurately model the effect of roughness, the respective roughness correction factor (K_{SR} ) must be multiplicatively applied to the AC resistance of the drum and matte sides of the traces separately. Unfortunately ADS, and many other commercial simulators, do not allow access to these surfaces to apply the correction properly. The best you can do is to apply the average of (K_{SR_drum }) and (K_{SR_matte }) side to the smooth conductor loss (IL_{smooth }), as described above.
The following are the steps to determine K_{SR_avg} (f ) and total IL with roughness:
1. Determine H_{RMS_drum }and H_{RMS_matte }from Equation 6 and Equation 7.
2. Determine the radius of spheres for drum and matte sides:
3. Determine the area of the square flat base for drum and matte sides:
4. Determine K_{SR_drum} (f ) and K_{SR_matte} (f ) :
5. Determine the average K_{SR_drum} (f ) and K_{SR_matte} (f ):
6. Apply Equation 8 to determine total insertion loss of the PCB trace.
Summary and Results
The results are plotted in Figure 8. The left plot compares the simulated vs measured insertion loss for data sheet values and design parameters. Also plotted is the total smooth insertion loss (crosses) which is the sum of conductor loss (circles) and dielectric loss (squares). Remarkably there is excellent agreement up to about 30GHz by just using algebraic equations and published data sheet values for Dk, Df and roughness.
The plot shown on the right is the simulated (blue) vs measured (red) effective dielectric constant (Dkeff ), and is determined by the equations shown. As can be seen, the measured curve has a slightly higher Dkeff (3.76 vs 3.63 @ 10GHz) than published. According to [6], the small increase in the Dk is due to the anisotropy of the material.
When the measured Dkeff (3.76) was used in the model, for core and prepreg, the IL results shown in Figure 9 (left) are even more remarkable up to 50 GHz!
Figure 8 IL (left) for a 6 inch trace in FR408HR RTF using supplier data sheet values for Dk, Df and R_{z}. Effective Dk is shown right.
Figure 9 IL (left) for a 6 inch trace in FR408HR RTF and effective Dk (right).
Figure 10 compares the Cannonball model against the H&J model. The results show that the H&J is only accurate up to approximately 15 GHz compared to the Cannonball model’s accuracy to 50GHz.
Figure 10 Cannonball Model (left) vs HammerstadJensen model (right).
Conclusions
Using the concept of cubic closepacking of equal spheres to model copper roughness, a practical method to accurately calculate sphere size and tile area was devised for use in the Huray model. By using published roughness parameters and dielectric properties from manufacturers’ data sheets, it has been demonstrated that the need for further SEM analysis or experimental curve fitting, may no longer be required for preliminary design and analysis.
When measurements from CMP28 modeling platform, fabricated with FR408HR and RT foil, was compared to this method, there was excellent correlation up to 50GHz compared to the H&J model accuracy to 15GHz.
The Cannonball model looks promising for a practical alternative to building a test board and extracting fitting parameters from measured results to predict insertion loss due to surface roughness.
For More Information
If you liked this design note and want to learn more, or get more details on this innovative roughness modeling methodology, you can visit my web site, LAMSIM Enterprises.com , and download a copy of the white paper [16], or my award winning DesignCon 2015 paper, [1]. And while you are there, feel free to investigate my other white papers and publications.
If you would like more information on our signal integrity and backplane services, or how we can help you achieve your next highspeed design challenge, email us at: info@lamsimenterprises.com
References
[1] Simonovich, Bert, “Practical Method for Modeling Conductor Surface Roughness Using Close Packing of Equal Spheres”, DesignCon 2015 Proceedings, Santa Clara, CA, 2015, URL: http://lamsimenterprises.com/Copyright2.html
[2] Hammerstad, E.; Jensen, O., “Accurate Models for Microstrip ComputerAided Design,” Microwave symposium Digest, 1980 IEEE MTTS International , vol., no., pp.407,409, 2830 May 1980 doi: 10.1109/MWSYM.1980.1124303 URL: http://ieeexplore.ieee.org/stamp/stamp.jsp?tp=&arnumber=1124303&isnumber=24840
[3] S. Hall, H. Heck, “Advanced Signal Integrity for HighSpeed Digital Design”, John Wiley & Sons, Inc., Hoboken, NJ, USA., 2009
[4] Huray, P. G. (2009) “The Foundations of Signal Integrity”, John Wiley & Sons, Inc., Hoboken, NJ, USA., 2009
[5] Y. Shlepnev, “PCB and package design up to 50 GHz: Identifying dielectric and conductor roughness models”, The PCB Design Magazine, February 2014, p. 1228. URL: http://iconnect007.uberflip.com/i/258943pcbdfeb2014/12
[6] Y. Shlepnev, “Sink or swim at 28 Gbps”, The PCB Design Magazine, October 2014, p. 1223. URL: http://www.magazines007.com/pdf/PCBDOct2014.pdf
[7] E. Bogatin, D. DeGroot , P. G. Huray, Y. Shlepnev , “Which one is better? Comparing Options to Describe Frequency Dependent Losses”, DesignCon2013 Proceedings, Santa Clara, CA, 2013.
[8] Wikipedia, “Closepacking of equal spheres”. URL: http://en.wikipedia.org/wiki/Closepacking_of_equal_spheres
[9] Simberian Inc., 3030 S Torrey Pines Dr. Las Vegas, NV 89146, USA. URL: http://www.simberian.com/
[10] Isola Group S.a.r.l., 3100 West Ray Road, Suite 301, Chandler, AZ 85226. URL: http://www.isolagroup.com/
[11] Oakmitsui 80 First St, Hoosick Falls, NY, 12090. URL: http://www.oakmitsui.com/pages/company/company.asp
[12] Electrochemicals Inc. COBRA BOND®. URL: http://www.electrochemicals.com/ecframe.html
[13] Macdermid Inc., Multibond. URL: http://electronics.macdermid.com/cms/productsservices/printedcircuitboard/surfacetreatments/innerlayerbonding/index.shtml
[14] Keysight Technologies, EEsof EDA, Advanced Design System, 2015.01 software. URL: http://www.keysight.com/en/pc1297113/advanceddesignsystemads?cc=US&lc=eng
[15] Wild River Technology LLC 8311 SW Charlotte Drive Beaverton, OR 97007. URL: http://wildrivertech.com/home/
[16] Simonovich, Bert, “Practical Method for Modeling Conductor Surface Roughness Using The Cannonball Stack Principle”, White Paper, Issue 1.0, April 8, 2015,
URL: http://lamsimenterprises.com/Copyright.html
Dr. Eric Bogatin Launches New Signal Integrity Academy
Last year, Signal Integrity Evangelist, Dr. Eric Bogatin announced the end of his famous signal integrity classes. At the time I remember thinking to myself, “What’s next for Eric”? If you know Eric, like I do, you realize that the end of one phase of his career usually means the start of the next one. And now we know what that is. You see, Eric has been busy the last six months (JanuaryJune2014) preparing to launch his new Teledyne Lecroy Signal Integrity Academy web portal.
Eric is currently a Signal Integrity Evangelist with Teledyne LeCroy, and on the faculty at the University of Colorado at Boulder, where he recently moved to from Kansas. He has a BS degree in physics from MIT, and MS and PhD degrees in physics from the University of Arizona in Tucson. He has held senior engineering and management positions at Bell Labs, Raychem, Sun Microsystems, Ansoft, and Interconnect Devices. Prior to being acquired by Teledyne Lecroy, he ran his successful company, Bogatin Enterprises, along with his wife Susan, where they provided signal integrity training.
I met and got to know Eric back in 2008, when we collaborated on our first DesignCon paper for 2009 titled, “Practical Analysis of Backplane Vias”. We were privileged to win a best paper award that year. Since that time we have worked on several projects together, and have become good friends. The last project we worked on was for a DesignCon2013 paper titled, “Dramatic Noise Reduction using Guard Traces with Optimized Shorting Vias”, which also won a best paper award.
Over the years, I have studied much of Eric’s work through his many papers, articles, webinars, blogs and content from his previous web site. I always made it a point to attend all of his presentations at any conferences I attended. I have his first edition “Signal Integrity Simplified” book as well. It has been one of my goto books when starting any of my research projects or concepts I am trying to grasp. Like my other goto signal integrity books in my library, it is well marked and used; although this one seems more so than others. Having the privilege of working with Eric has also enriched my learning experience.
Over the years, I always wished I could have attended some of his classes; but due to travel cost and time away from the office, it could never be justified. Now, with the beauty of the internet, the classes can come to me. I can choose to watch what I want; when I want; as many times as I want; on whatever device I want. My iPad is a perfect choice! For a yearly subscription fee for individuals or corporations, you have the opportunity of watching any class or lesson anytime.
All the content is in the form of short, concise video lessons lasting 5 to 15 minutes. Slides are available for download and I suggest downloading the respective slides prior to watching the presentation so you can make notes as you go along. The initial three courses: Essential Principles of SI; Advanced Gigabit Channel Design; SParameters for SI; are based on his most popular public classes. Once subscribed, you are offered an “all you can eat buffet” of all the lessons. There are more courses and lessons planned in the future.
If you have always wanted to accelerate your signal integrity learning curve, then the Teledyne Lecroy Signal Integrity Academy may be the right place for you to start. You can learn more by visiting Eric’s web site at: Bethesignal.com
Dr. Howard Johnson; a great teacher, mentor and friend.
The other day, in my inbox, I received the link to the June 2013 electronic edition of EDN magazine, and promptly clicked to Howard Johnson’s signal integrity column. I have looked forward to reading them for many years now, and when I used to receive the magazine, in print, I faithfully cut out the respective month’s articles, and filed them away for future reference. This month I was saddened to read it was to be his last article for EDN. After a long and distinguished career, he decided to retire from his consulting and seminar business. I knew it was going to happen soon, but when I actually read it in print, I started to think about my career, and how influential he has been teaching me about signal integrity. Ironically, the title of the article, “Seek inspiration”, touched on the importance of mentorship and has inspired me to write this post.
Dictionary.com defines a mentor as “a wise and trusted counsellor or teacher”. Over the years H.J. became mentor to thousands of engineers and students all over the world, including myself, through his teachings, publications and films. The main thing I learned from him was to think about problems differently and try to apply other disciplines to understand what’s going on.
H.J. always had a way of presenting complex signal integrity topics simply by relating the subject to other things in life we are most familiar with. I remember one article he wrote, years ago, about wave propagation along a transmission line, and how it was analogous to slowly filling an icecube tray by tilting it at one end, and letting the water slowly fill each compartment at a time before overflowing and filling the next, and the next, and the next, until all were full. Now, I cannot fill an icecube tray without thinking about transmission lines, or my friend.
I was first introduced to his teachings by reading, “Highspeed Digital Design, a handbook of black magic”. Back in 1999 it was my first book on signal integrity, and ultimately was the lure that got me hooked. I remember going through each section, taking notes, highlighting some text, and book marking certain sections throughout with little cutup strips of postit notes. The F_knee = 0.5/tr equation is still etched in my nonvolatile memory. Not everything made sense to me the first time, but over the years I found myself going back to those sections and rereading them, depending on the problem of the day I was trying to solve.
Over the years, I would occasionally email him with questions and ask for clarification of parts of his books. Each time he was more than willing to respond back with a more detailed explanation. When email didn’t work, he took time from his busy schedule to arrange a phone meeting where we could discuss the subject in more detail.
When I look back now, I realized just how much I have grown and learned, thanks to Howard Johnson sharing his knowledge and experience. But then again, it is only natural for a true mentor to do. How has Howard Johnson mentored and inspired your career?
Are Guard Traces Worth It?
Originally published in, The PCB Design Magazine, April 2013 issue.
By definition, a guard trace is a trace routed coplanar between an aggressor line and a victim line. There has always been an argument on whether to use guard traces in highspeed digital and mixed signal applications to reduce the noise coupled from an aggressor transmission line to a victim transmission line.
On one side of the debate, the argument is that the guard trace should be shorted to ground at regular intervals along its length using stitching vias spaced at 1/10th of a wavelength of the highest frequency component of the aggressor’s signal. By doing so, it is believed the guard trace will act as a shield between the aggressor and victim traces.
On the other side, merely separating the victim trace to at least three times the line width from the aggressor is good enough. The reasoning here is that crosstalk falls off rapidly with increased spacing anyways, and by adding a guard trace, you will already have at least three times the trace separation to fit it in.
In our DesignCon2013 paper titled, “Dramatic Noise Reduction using Guard Traces with Optimized Shorting Vias”, I coauthored along with Eric Bogatin, we showed that sometimes guard traces were effective, and sometime they were not; depending on how the guard trace was terminated. By correct management of the ends of the guard trace, we demonstrated it can reduce coupled noise on a victim line by an order of magnitude over not having the guard trace present. But if the guard trace was not optimized, the noise on the victim line can also be larger with the guard trace, than without.
Analysis Using Circuit Models
We started out the investigation by building circuit models for the topologies studied. Agilent’s EEsof EDS ADS software was used exclusively to model and simulate both stripline and microstrip configurations. The generic circuit model, with a guard trace, is shown in the top half of Figure 1. The circuit model, without a guard trace, is shown in the bottom half.
For the analysis, we used lossless transmission line models. The guard trace length was exactly matched to the coupled length. The ground stitching and the endtermination resistors, on the guard trace, could be deactivated, and/or shorted, as required. The linewidth space geometry was set at 555 mils, and the spacing for the nonguarded topologies was set to three times the line width.
Figure 1 ADS schematic for generic topologies with a guard trace (top) and without (bottom). The transmission line were segmented and parameterized to easily change the lengths as required. The ground stitching and the endtermination resistors, shown in top schematic, can be deactivated and/or shorted as required.
Figure 2 is a summary of results when a guard trace was terminated in the characteristic impedance, left open, or shorted to ground at each end. The red waveforms are the results for topologies without a guard trace, and the blue waveforms are with a guard trace.
Depending on the nature of the termination, the reinfected noise on the guard trace can add or subtract to the directly coupled noise on the victim line. This often makes the net noise on the victim line worse than without a guard trace.
Unlike a simple twoline coupled model, where the near end crosstalk (NEXT) and far end crosstalk (FEXT) can be easily predicted from the RLGC matrix elements, trying to predict the same for a threeline coupled model is more difficult. Manually keeping track of all the noise induced on the guard trace, and its reinfection onto the victim line, is extremely tedious. First you must identify the directly coupled reinfected backward and forward noise on the victim line from the voltage on the guard trace. Then the problem is keeping track of the multiple reflections of the noise on the guard trace. Because of this, the only real way to analyse the effect is through circuit modeling and simulation.
In microstrip topologies, as you can see, there is little to no benefit to adding a guard trace; regardless of how the ends are terminated. This is because microstrip topologies are inherently prone to far end crosstalk. Therefore any far end noise, coupled onto the guard trace, will subsequently reinfect the victim with additional far end noise; as seen by the additional ringing superimposed on the blue waveform.
In stripline topologies, without a guard trace, there is no farend cross talk generated. But when a guard trace is added, and depending on how the ends are terminated, any near end coupled noise on the guard trace can reinfect the victim. It is only when the ends are shorted to ground we see such a dramatic reduction of both near and far end noise.
Figure 2 Summary of simulation results when the ends of the guard trace was terminated, left open or shorted to ground for microstrip and stripline geometries.
Distributed Shorting Vias
When practically implementing a guard trace, to act as a shield, a rough rule of thumb suggests the spacing of shorting vias should be at least 1/10 the wavelength of the highest frequency content of the signal. For a risetime of 100 psec, the stitching via spacing, to meet l/10, is 0.18 inches; or 9 stitching vias over 1.5 inches.
Figure 3 summarizes the results when a guard trace was stitched to ground at multiple wavelengths; compared to the case of no guard. As you can see, in the case of microstrip, when the guard trace is shorted with fewer than 9 vias, there is still considerable ringing noise on the guard trace which can reinfect the victim line. But in the case of stripline, having two shorting vias at each end, or any number up to 9 shorting vias has the same result. This suggests there is no need for multiple shorting vias, other than at the end of the guard trace; as long as the guard trace is the same length as the coupled length. This dramatically simplifies the use of guard traces in stripline.
Figure 3 Summary of simulation results with guard trace stitched for microstrip and stripline geometries.
Practical Design Considerations
Up until now we have modeled and simulated ideal cases of shorting the guard traces to ground. But in reality, there are additional practical design considerations to consider. First is via size, and the impact it has on the line to line spacing. Next is the finite via inductance; since its impedance will prevent complete suppression of the noise on the guard trace. And finally, the extension of the guard trace compared to the coupled length.
Because through hole manufacturing design rules limit the smallest via and capture pads, the smallest mechanical drill size most PCB vendors will spec is 8 mils. By the time you factor in the minimum pad diameter and pad to copper spacing, the minimum space between the aggressor and victim lines would have to be at least 28 mils, as shown in Figure 4; just to fit a guard trace with grounding vias down its length.
At this point, you have to ask yourself if it is even worth it; especially for microstrip topologies. If the two signal lines were to be increased to 28 mils, the reduction in cross talk from just the added separation would likely be more significant than adding the shorted guard trace.
Figure 4 Minimum track to track spacing to fit an 8 mil drilled via and pad in throughhole technology.
Fortunately, the circuit analysis has shown there is little benefit to adding a guard trace to microstrip topologies, even if it was ground stitched appropriately. But to gain a dramatic reduction in cross talk in stripline all that is required is to short the guard trace at each end, and ensure the guard trace is exactly the same length as the coupled length. This means the minimum space to fit a via and guard trace can remain at three times the line width; as long as the guard trace is extended slightly, as shown in Figure 5(a). Alternatively, the guard trace can be made equal to the coupled length, as illustrated in Figure 5(b).
Agilent’s ADS Momentum planar 3D field solver was used to explore and quantify the implications vias and guard trace lengths have on noise reinfection. Figure 5 details a portion of the 3D model on the left end of the respective topologies. The right hand sides are identical. The reference planes are not shown for clarity.
Figure 5 Two examples of adding a grounded guard trace with minimum spacing of 3 x line width. Figure (a): guard trace is extended past the coupled length (A) by dimension B on both sides in order to satisfy minimum 5 mil padtrack spacing requirements. Figure (b): guard trace is equal to coupled length by separating the traces at each ends. Modeled in Agilent Momentum 3D field solver. Reference planes are not shown for clarity.
After simulation, the Sparameter data was saved in Touchstone format and brought into ADS for transient simulation analysis and comparison. Figure 6 shows the results. The plot on the left used 100 psec risetime for the step edge, while the plot on the right used 50 psec. Both plots are consistent with the dramatic noise reduction observed in Figure 2, except here we see some added noise ripple after about 0.8 nsec.
At 100 psec risetime, there is effectively no difference in near end noise signature for either (a) or (b) topology. But when the risetime was reduced to 50 psec, the noise ripple is more pronounced. The blue waveform shows that even when dimension B is 0 mils, there is still a small amount of noise due to the inductive length of the vias to the reference plane. The red waveform shows that adding just 12 mils to the guard trace length, at each end, the ripple magnitude is almost doubled.
It is a wellknown fact that technology advancements over time results in faster and faster rise times. If you have engineered your design on the technology of the day, any future substitution of parts, with faster rise time, may cause your product to fail, or worse be intermittent.
Figure 6 Momentum transient simulation results comparing near end crosstalk at Port 1 when aggressor voltage was applied to Port 3. The red and blue waveforms are with a guard trace. The green waveform is with no guard and 15 mils separation. Aggressor voltage = 1V, 100 psec risetime (left) and 50 psec risetime(right)..
To explore this phenomenon, the guard trace was varied by 50 and 100 mils at each end, as illustrated in Figure 7. Here we can see that as the guard trace gets longer at each end, the noise ripple grows in magnitude quite rapidly. It is remarkable to note that when the guard trace is just 100 mils longer, at each end, the peakpeak amplitude of the noise just about equals the peak magnitude of the no guard case.
Figure 7 Momentum transient simulation results with guard trace extended. B = 12 mils (red), B = 50 mils (blue) and B = 100 mils (magenta) compared to no guard (green). Aggressor voltage = 1V, 100 psec risetime. Dimensions in mils.
When the guard trace was removed, and the space was increased to five times the line width, the near end crosstalk was reduced in magnitude and was approximately equal to the guard trace scenario, as seen in Figure 8. Furthermore, because there is no guard trace, there is no additional noise ripple.
Figure 8 Momentum transient simulation results comparing near end crosstalk at Port 1 when aggressor voltage was applied to Port 3. Aggressor voltage = 1V, 100 psec risetime.
So getting back to the original question, “Are guard traces worth it?” You be the judge. Using a guard trace, shorted at each end, can be effective, if you need the isolation. But it does have caveats. If you decide to go down this path, it is imperative for you to model and simulate your topology, preferably with a 3D field solver, before signing off on the design.
Reference

Eric Bogatin, Bert Simonovich,“Dramatic Noise Reduction using Guard Traces with Optimized Shorting Vias”, DesignCon2013, Santa Clara, CA, USA, Jan 2831, 2013.
Noncontact Interconnect: When Crosstalk Is Your Friend
Originally published in, The PCB Design Magazine, November 2012 issue.
In normal PCB designs, crosstalk is usually an unwanted effect, due to electromagnetic coupling, of two or more traces routed in close proximity to one another. We usually consider it to be our enemy, in any highspeed design, and go to great lengths to avoid it. So how, you may ask, can crosstalk ever be your friend?
To answer that question, I would like to start out by taking you back to the fall of 1994. This was the era of wide parallel busses running up to 33 MHz across backplanes. Highspeed serial, pointpoint interfaces, and serdes technology, as we know and love today, was just a twinkle in some bright young engineer’s eye.
Nortel, a.k.a. Northern Telecom at the time, was looking to replace the computing module shelf of the DMS Supernode platform because it was projected to run out of steam a few years later. In order to address the issue, the system architects decided that a scalable, multiprocessing, shared memory, computing architecture was needed to replace it.
My job was to develop a concept to package all these cards in a shelf, and then design a backplane to interconnect everything. It quickly became evident that a single shared bus could not support the bandwidth required for multiprocessing. Nor could multiple parallel buses solve the problem, because of the lack of highdensity backplane connector technology needed for all the I/O. Even if we had a suitable connector, and it could magically fit within the confines of the card slot, then the layer count of the backplane would have grown exponentially.
No, something else was needed. Fortunately, Bell Northern Research (BNR), the R&D lab of Nortel where I was working at the time, had an advanced technology group, that liked to play in the sand. I remember going to a meeting one day to see some presentations on some of the neat technology they were playing with.
One presentation they gave, was of a unique noncontact interconnect technology. I immediately saw the practical application that technology offered for our architecture, and it instantly became my friend. It allowed us to eventually invent a patented, proprietary point to multipoint interconnect solution, running at 1GB/s per pair [1].
The noncontact technology actually relied on controlled electromagnetic coupling, or simply crosstalk. See Figure 1. In this simple highlevel block diagram, each card on the shelf would transmit their data differentially across the backplane. As the differential pairs traversed through the connector fields of the card slots, the transmit signal was edgecoupled to an adjacent small trace, about three quarters of an inch long, connected to the respective receiver pin. After the last card slot, the transmit differential pairs switched layers where they returned back to the originating card and were terminated.
The beauty of this architecture was that each card only needed one set of transmitters to broadcast its data to all the other cards. Since each card had enough receivers to listen to the other cards, the point to multipoint interconnect achieved the equivalent of a multipoint to multipoint architecture; but without the overhead of additional pins and PCB layers. Furthermore, an effective line rate of 1GB/s was achieved using simple, inexpensive 2mm connectors; the same ones chosen for compact PCI standard.
Figure 2 is a photograph of an inner layer, doublesided core of the backplane, prior to lamination and drilling. It shows the couplers in more detail. The round pads are for the connector vias, and are used to attach the coupler traces to the connector pins. The rows of pads on the left are for one card slot, while the rows of pads on the right are for another card slot.
If we look at the two traces entering the picture from the bottom left side, we can see how they are routed through the connector field. These two traces are part of a differential pair where each are routed as singleended traces, i.e. with no coupling to one another. As these traces approach the first row of pads, they jog down to minimum spacing to ensure close coupling to the coupler traces attached to the pads. The close spacing continues to ensure maximum coupling to the next set of pads, where the pattern stars all over again at the bottom right. This pattern repeats all the way up the photo for each differential pair.
You may be astute to notice that the bottom coupler trace connects to a pad at each end, while the mate coupler, above it does not. When two, coplanar parallel traces are in close proximity to one another, there are two types of crosstalk generated; backward or NearEnd crosstalk (NEXT); and forward or FarEnd crosstalk (FEXT).
As the transmit signal propagates, from left to right in the photo, the rising edge of the signal initiates NEXT at the beginning of the coupled length. The NEXT voltage saturates after a critical length equal to the risetime divided by twice the propagation delay; where the risetime is in seconds, and propagation delay is in seconds per unit length. It stays saturated for twice the time delay of the coupled length. Because of differential signalling, the NEXT voltages are of opposite phase on the respective couplers.
At the coupler pin, there is a reflection caused by the via. Since the couplers, at the farend, are not terminated, in the characteristic impedance, and left open, any secondary reflections due to coupler via reflects back towards the receiver, again with opposite phase. When both reflections arrive back at the receiver, they will add together and add additional noise to the eye, causing intersymbol interference, as shown by the shoulder in Figure 3(A). By leaving one end open, and shorting the other one to ground, means that any secondary noise will have the same phase, and when they arrive at the receiver, they will cancel, thereby eliminating the intersymbol interference and increasing the eye amplitude as shown in Figure 3(B).
You will notice that the eye waveforms do not resemble the traditional eye diagram we are used to seeing. Instead we observe a typical NEXT eye, when the coupled length is short, compared to the bit time. There is also a line right in the middle.
Figure 4 can help to explain the reason. The blue waveform is the NEXT voltage, seen at the nearend of the coupler, in response to the red transmitted waveform. Notice that there are only pulses at an edge transition of the transmitted waveform. A rising edge creates a positive pulse, and a falling edge generates a negative pulse. The duration of each pulse is twice the time delay of the coupler length.
The receiver uses simple peakdetectors and latch to regenerate the signal back to the original waveform. A positive going pulse is detected by the positive peakdetector. When it crosses the positive voltage threshold (+V_{th}), it sets the latch output to logic high. The output remains high until a negative pulse crosses the negative threshold (V_{th}), of the negative peakdetector, and resets the latch to logic low.
And that is how crosstalk can be your friend! Of course the small coupled crosstalk signal means we have to guard against CROSSTALK from other digital signals on board. But that’s nothing that mixed signal layout design rules can’t solve. ……Wait a minute! ……We both share the same enemy? …….. Who would have thought an old Proverb, “The enemy of my enemy is my friend” [sic], would apply here too?
Reference:
[1] L. Simonovich et al, U.S. Patent 6,091,739, “HIGH SPEED DATA BUS UTILIZING POINT TO MULTIPOINT INTERCONNECT NONCONTACT COUPLER TECHNOLOGY ACHIEVING A MULTIPOINT TO MULTIPOINT INTERCONNECT.”
[2] J. Williamson et al, U.S. Patent 6,016,086, “NOISE CANCELLATION MODIFICATION TO NONCONTACT BUS.”
[3] Alexandre Guterman, Robert J.Zani, “PointtoMultipoint Gigabit Backplane Design”, IEEE International Symposium on EMC, May 1116, 2003.
To Know The Bit Error Rate Is To Know The Bit Error Ratio
Recently I came across a blog post titled, “Can Oscilloscopes Really Calculate BERs?”, written by Ransom Stephens.
I liked this article. I liked it because, as usual, Ransom likes to challenge your way of thinking and makes you go back to basics in order to understand. For example, when he debates whether BER is “bit error ratio” or “bit error rate”, it stopped me in my tracks to question if I was using the correct terminology, and why. For the record, when I started my career working on T1 line repeaters, I was taught it was “rate”. But, technically, Ransom’s assertion that it really is “ratio” is also correct.
Before you discount this and say, “In mathematics, there can be only one answer”, stay with me here, and let me try to explain where I’m coming from. According to MerriamWebster dictionary, the definition of ratio is, “the indicated quotient of two mathematical expressions”, or “the relationship in quantity, amount, or size between two or more things: proportion”. If you take the number of bit errors and divide them by the total number of bits, then you have, by definition, a ratio, as Ransom claims. For example, if you have 1 error in 1 TBits of data, then you have a “bit error ratio” of 1E12.
When you look up the word rate, in the same dictionary, the definition is, “reckoned value: valuation” or “a fixed ratio between two things”. In terms of BER, when it is defined as rate, the fixed ratio between two things is the number of errors over some period of time. Since a bit has a time component associated with it, you can convert the total number of bits into time by multiplying it by the bit time. For example, at 10 GB/s, the bit time is 100 ps. So 1TB of data takes 100 seconds to transmit all of the bits. If there was 1 bit error during that time, you would have a “bit error rate” of 1 error per 100 seconds.
In mission critical applications, we usually aspire to have errorfree performance for the life of the product. As bit rates continue to climb, that’s an awful lot of bits. Theoretically, if you want your product to have a bit error rate of 1 error in 25 yrs, then, at 10GB/s, you would need to transmit 7.884E+18 bits;[25yrs*(60*60*24*365)sec/yr*10GB/s] to have a bit error ratio of 1.268E19!
Bit error ratio, or bit error rate? It kind of reminds me of part of the song, “Let’s Call the Whole Thing Off”, by George and Ira Gershwin; “You like tomaytoes, and I like tomahtoes”. At the end of the day, it’s still tomatoes. In the right context, I think both terms are equally valid. You need to be ambidextrous, so to speak, in your analysis and how you quote the number.
PCB Vias Are Capacitive But Not Necessarily Capacitors
Huh? …… What do you mean by that? ……
For years now the popular opinion was that PCB vias were capacitive in nature, and therefore could be modeled with lumped capacitors. Although this might be true when the rise time of the signal is greater than or equal to 3 times the delay of the via discontinuity, I’ll show you why it is no longer appropriate to think this way; even risky to continue to model your highspeed channel using this methodology.
Let’s start the discussion by saying vias are transmission lines with excess parasitic capacitance or inductance. Vias are considered transparent when their impedance equals the characteristic impedance of the transmission lines attached to them. In almost all cases, vias passing through multilayer PCBs are capacitive because of the distributed capacitance between the via barrel and antipads. As a result, they end up having lower impedance than the traces connected to them. Like any other transmission line, when a rising edge of a signal encounters a lower impedance, it will cause a negative reflection for the length of the discontinuity.
Getting back to the point, it is best demonstrated by an example as summarized in Figure 1. Consider a via at the far end of a long 50 Ohm transmission line. The via has a short through section and a long stub section. The through section is 15 mils and the stub is 269 mils for a total via length of 284 mils. This is not unusual for modern backplane designs.
For this particular via geometry, the impedance is 33 Ohms and the excess via capacitance is 1.9pf. Even with a fast 50ps rise time at the source, by the time the signal reaches the via at the far end, the rise time will degrade due to dispersion caused by the lossy dielectric. In this example, after 23 inches, the rise time has degraded to approximately 230ps.
If the total delay (TD) of the via discontinuity is 60 ps, then the 230 ps rise time at the via is greater than 3TD (180ps). As expected, when modeling the via with a lumped capacitor equal to the excess capacitance, and comparing it with the transmission line via model, the TDR plot of the reflections are virtually the same using a 230ps rise time.
Figure 1 Via model TDR comparison after 23 inches. Top topology uses 33 Ohm transmission lines for both the through and stub portion of the via. The bottom topology models the via with a 50 Ohm transmission line to represent the delay of the through portion and a 1.9pf capacitor to represent the excess capacitance. Modeled and simulated with Agilent ADS.
So far so good, right? Well maybe so. The only way to know is to explore this topology even further and compare eye diagrams. Let us say your circuit needs to work at XAUI rate of 3.125 GB/s. You modify both topologies by adding a driver and receiver. After simulating you end up with eye diagrams as shown in Figure 2.
Figure 2 Eye comparison at 3.125Gb/s. Top topology uses 33 Ohm transmission lines for both the through and stub portion of the via. The bottom topology models the via with a 50 Ohm transmission line to represent the delay of the through portion and a 1.9pf capacitor to represent the excess capacitance. Modeled and simulated with Agilent ADS.
Still ok. So what is your point, you might ask?
You are correct when you comment there is a good match for reflections and the eyes are wide open. Ah, but now let us say you want to run this at 10GB/s down the road. So you dial up the bit rate on the transmitters and simulate both topologies again. But this time, you get some unexpected results as shown in Figure 3.
Figure 3 Eye comparison at 10Gb/s. Top topology uses 33 Ohm transmission lines for both the through and stub portion of the via. The bottom topology models the via with a 50 Ohm transmission line to represent the delay of the through portion and a 1.9pf capacitor to represent the excess capacitance. Modeled and simulated with Agilent ADS.
Ouch! What happened here? Looking at the TDR, the reflections at the end of the channel look the same so why doesn’t the receive eyes match? To answer this question, we really need to look at the Sparameter plots of both channels. Figure 4 shows the insertion and return losses of both topologies. Red is the transmission line model and the blue is the capacitor model.
Figure 4 Insertion and return loss of both topologies. Red curves are the transmission line via model and blue curves are the capacitor model.
The insertion loss plot represents the transmitted output power vs. frequency while the return loss is the reflected power vs. frequency. In the time domain, the insertion loss and return loss is equivalent to the TDT and TDR plots respectively. As you can see, the return loss matches pretty well; just like the TDR plot we observed earlier, but It is only obvious when we view the insertion loss plot as to the real reason for the eye discrepancy of Figure 3.
Notice the first resonant null at approximately 4.5 GHz. This null represents the quarter wave resonant frequency fo, and is due to the long 269 mil via stub. The other null at 13.5GHz is the 3rd harmonic of fo. The longer the stub length, the lower the resonant frequency. When there is a null at or near onehalf the bit rate, then the eye will be devastated. In our example, 4.5GHz is approximately half of 10GB/s and as you can see from Figure 3 the resultant eye is totally closed.
But the Sparameters tell us even more. We can use them to confirm the rule of thumb used earlier with respect to the rise time of the signal being greater than, or equal to, 3 times the delay through the via discontinuity.
If you study the return loss plot, you will see there is an excellent match up to about 1.83GHz. This is the effective bandwidth for which the capacitor model is good for. Put another way, a bandwidth of 1.83GHz means you could use an equivalent capacitor model for the via for bitrates up to 3.6GB/s.
Equation 1 is a commonly used to convert 3dB bandwidth to equivalent 1090 rise time. Substituting 1.83 GHz for the 3dB bandwidth, the rise time equals approximately 185 ps.
Equation 1
When you divide 185 ps by 3, you end up with approximately 62ps compared to approximately 60ps for the propagation delay through the via we originally determined earlier.
Figure 5 is a summary of a simulation with the transmission line length reduced to 18 inches to reduce the rise time to 185 ps. As you can see the transmission line via model’s eye at 3.6 Gb/s is just starting to distort while the capacitor model is still relatively smooth; confirming our bandwidth rule of thumb. Using a capacitor as a via model past this bitrate will result in optimistic results and long nights when your 10 Gig prototype hits the lab.
So now you see what I mean when I say that vias are capacitive, but not necessarily capacitors.
Figure 5 Eye comparison at 3.6Gb/s. Top topology uses 33 Ohm transmission lines for both the through and stub portion of the via. The bottom topology models the via with a 50 Ohm transmission line to represent the delay of the through portion and a 1.9pf capacitor to represent the excess capacitance. Modeled and simulated with Agilent ADS.
For more Information:
If you liked this design note and want to learn more, or get more details on modeling vias using transmission lines, you can visit my web site, LAMSIM Enterprises.com , and download a copy of the white paper I wrote along with Eric Bogatin and Yazi Cao titled, “Method of Modeling Differential Vias” .
While you are there, feel free to investigate my other white papers and publications.
If you would like more information on our signal integrity and backplane services, or how we can help you achieve your next highspeed design challenge, email us at: info@lamsimenterprises.com.
T1C Line Repeater–A Blast From The Past
I recently came across some souvenir pictures and artwork of work I had done early in my career at Bell Northern Research. For those of you who are old enough to remember, it will bring back some fond memories of the technology back in the day; and for you young designers, this is how we did things back in the late ‘70s, early ‘80s.
Figure1 Northern Telecom T1C line repeater circa 1980.
Figure 1 is a T1C line repeater I helped to design early in my career circa 1980. Line repeaters were used to regenerate digital signals along a span between two central offices. There were two regenerators per line repeater, and one repeater for every 4pairs (2Tx, 2Rx) in the cable. They were housed in apparatus cases mounted on telephone poles or pedestals every mile or so. In the city they were usually installed in manhole vaults buried underground.
T1 digital transmission was introduced in 1961 as a way to replace older analog voice frequency technology, and is still in use today. T1 data rate is 1.544 Mb/s and carries 24 channels of DS0 at 64Kb/s. As digital technology exploded through the 1970’s, it became more affordable, allowing T1 to become more popular. By the early 1980’s, the installed base was reaching capacity especially in large cities, and the industry was looking for ways to increase its bandwidth. Sound familiar? To address this issue, a new T1C standard was developed to double the bandwidth. T1C stands for T1concatenated, and doubles the data rate to 3.152 Mb/s allowing it to carry 48 DS0 channels.
As part of the T1C project team, my primary responsibility was to package the design and lay out the printed circuit board. Because of the limited real estate available and because throughhole component technology was the only choice for PCBs, we needed to use thickfilm technology for the receiver equalization circuitry.
Thickfilm technology was quite popular at the time, and was the predecessor to today’s surfacemount technology on PCB’s. It allowed for the miniaturization of circuitry by screen printing conductive traces and resistive ink onto a ceramic substrate, then firing it to a high temperature. Surface mount components were limited to capacitors, SOT transistors and diodes.
At the time, Northern Telecom (NT) had their own inhouse thickfilm design and manufacturing facility located in Aylmer, Quebec. All of the thickfilm designs used in NT’s products prior to the T1C project were single inline packages (SIPs). Because of the height restriction, and the amount of circuitry needed to be integrated onto the substrate, SIPs were impractical, so we had to develop dual inline manufacturing capability at the same time we were developing the product.
The final dual inline thickfilm packages are shown near the faceplate. Since the packaging of the repeater was so dense, I needed to place components under the thickfilm substrates. This was all well and good until I was testing a bunch of repeaters for a field trial in California coming up in December of that year. I accidentally dropped one and it happened to land flat with component side up. After I picked it up, I had noticed both thickfilm substrates were cracked. How could this be? There was enough clearance from the highest component underneath, and enough pins to support the ceramic substrate, so why did it break?
Fortunately, we had a state of the art photography lab in the building with highspeed camera equipment. So we set up a controlled experiment to capture what went wrong. We built up some test samples and dropped them while capturing it all at highspeed. Well it wasn’t a fluke. Every one that we dropped and filmed showed the same result. It turns out there was enough flex in the long right angle pins, that the momentum of the substrate caused it to hit the radial capacitor underneath, then spring back as if nothing had ever happened. Under other circumstances, this would have been cool to see, but not when the project was in jeopardy.
To make a long story shorter, I eventually came up with an elegant solution for a plastic carrier that would support the substrate and keep it at a fixed height above the board. Not only did it solve the reliability problem, but it also solved the shipping and handling protective packaging issue for the thickfilm assembly at the same time.
Figure 2 shows the actual artwork for the repeater’s PCB. Back then, all our boards were doublesided and all layouts were done by hand; first in colored pencil, then using red/blue tape and pads on mylar film for final artwork. Red usually represented the solder (bottom) side of the board and blue was the component (top) side. The artwork was usually done at 2:1 scale and later photo reduced to produce the 1:1 photomasks. Red and blue filters were used during the photo reduction process to separate individual layer masks. A red filter generated the component side and blue filter produced the solder side photomasks respectively. All drilled holes were manually specified on a separate drawing with various symbols for the drill sizes. Line widths and space were typically 25 mils and components were on 100 mil pitch. All components were throughhole mounted on one side only and passed through a solder wave.
Figure 2 Example of doublesided artwork for the T1C line repeater. Red is solder side, blue is component side.
The T1C line repeater project from its inception, to designing, testing, building 50 prototypes by hand and completing a successful field trial in California, took about 6 months; all with a team of three plus our manager, and mechanical design support staff. Finding these pictures truly was a blast from the past. Looking back, I sometimes wonder if we could have done it any faster with today’s modern technology, CAD tools and outsourcing business model. What do you think?
Born in Hamilton, Ontario, Canada, Bert graduated in 1976 from Mohawk College of Applied Arts and Technology in Hamilton, Ontario, Canada as an Electronic Engineering Technologist. Over a 32 year career at Bell Northern Research and Nortel, he helped pioneer several advanced technology solutions into products and has held a variety of R&D positions, eventually specializing in highspeed signal integrity and backplane design. He is the founder of Lamsim Enterprises Inc. providing innovative signal integrity and backplane solutions. He is currently engaged in signal integrity, characterization and modeling of highspeed serial links associated with backplane interconnects. With three patent applications and two patent grants to his name, he has also (co)authored several publications, including an awardwinning DesignCon2009 paper related to PCB via modeling. His current research interests include signal integrity, highspeed characterization, and modeling of highspeed serial links associated with backplane interconnects. To contact Bert, email him at: info@lamsimenterprises.com
The Poor Man’s PCB Via Modeling Methodology
You are a backplane designer and have been assigned to engineer a new highspeed, multigigabit serial link architecture from several line cards to multiple fabric switch cards across a backplane. These links must operate at 6GB/s day one and be 10GB/s (IEEE 802.3KR) ready for product evolution. The schedule is tight, and you need to come up with a backplane architecture to allow the rest of the program to progress on schedule.
You come up with a concept you think will work, but the backplane is thick with over 30 layers. There are some long traces over 30 inches and some short traces of less than 2 inches between card slots. There is strong pressure to reuse the same connector you used in your last design, but your gut tells you its design may not be good enough for this higher speed application.
Finally, you are worried about the size and design of the differential via footprint used for the backplane connectors because you know they can be devastating to the quality of the received signal. You want to maximize the routing channel through the connector field, which requires you to shrink the antipad dimensions, so the tracks will be covered by the reference planes, but you can’t easily quantify the consequences on the via of doing so.
You have done all you can think of, based on experience, to make the vias as transparent as possible without simulating. Removal of nonfunctional pads on the inner layers, and planning to backdrill the connector via stubs will help, but is it enough? You know in the back of your mind the best way to answer these questions, and to help you sleep at night, is to put in the numbers.
So you decide to model and simulate the channel. But to do so, you need accurate models of the vias to plug into your favorite circuit simulator. But how do you get these? You have heard it all before; “for highspeed, the best way to model a via is with a 3D electromagnetic field solver”. Although this might be true, what if you don’t have access to such a tool, because the cost is more than your company wants to spend, or because you don’t have the expertise nor the time to learn how to build a model you can trust to make a timely decision?
On top of that, 3D field solvers typically produce Sparameter behavioral models. Since they represent only one sample of a given construction, it is impossible to perform whatif, worst case, min/max analysis with a single behavioral model. Because of this, many iterations of the model are required; causing further delay in getting your answer.
A circuit model on the other hand, is a schematic representation of the actual device. For any physical structure, there can be more than one circuit model to describe it. All can give the same performance, up to some bandwidth. When run in a circuit simulator, it predicts a measurable performance of the structure. These models can be parameterized so that worst case analysis can be explored quickly.
The problem with a circuit model is that you often need a behavioral model to calibrate it, or need to use analytical equations to estimate the parameters. But, as my friend Eric Bogatin often says, “an OK answer NOW! is better than a great answer late”.
In the past, it was next to impossible to develop a circuit model of a differential via structure without a behavioral model to calibrate it. These behavioral models were developed through empirical formulas, measured data, or through the use of 3D EM field solvers.
Now, there is another way. I have nicknamed it, “The Poor Man’s PCB Via Modeling Methodology”. Here’s how it works.
Anatomy of a Differential Via Structure:
An example of a differential via structure, shown in Figure 1, is representative of vias used to connect surface mounted components or backplane connectors to internal layer traces.
The via barrel is a plated through hole extending the entire length of a PCB stackup. The outside diameter equals the drill diameter. The inside diameter is the finished hole size (FHS) after plating. Pads are used on layers to ensure there is sufficient copper for track attachment after drilling operation. When used in this fashion, they are referred to as functional pads. Antipads are the clearance holes in the plane layers allowing the via barrel to pass through them without shorting.
The via portion is the length of the barrel connecting one signal layer to another. It is often referred to as the through via since it is part of the signal net. The stub portion is the rest of the barrel extending to the outer layer of the PCB. In highspeed designs, a good rule of thumb to remember is that a via stub should be less than 300mils/BR in length; where BR is the bit rate in Gb/s.
Building a Simple Scalable Circuit Model:
On close examination of Figure 2, a differential via structure can be represented by a twinrod transmission line geometry with excess capacitance (shown in red) distributed over its entire length. The smaller the antipad diameter, the greater the excess capacitance. This ultimately results in lower via impedance, causing higher reflections.
In all highspeed serial link designs, it is common practice to remove all nonfunctional pads and to maximize the antipad clearance as much as practically possible. Oval antipads are often used in this regard to further mitigate excess via capacitance.
Figure 3 illustrates the equivalent circuit for a differential via that could be used in a channel topology simulation. Here it is modeled with Keysight ADS software using a coupled line transmission line model for each section. This equivalent circuit model can be scaled for any combination of layer transitions and integrated in any channel simulation scenario.
Since the crosssection of the via is constant throughout its length, the differential impedance of all sections of the via are the same. We only need to know the physical length of each segment and the effective dielectric constant (Dkeff) to get the time delay of each segment.
When driven differentially, the oddmode parameters of each via are of major importance. Since the evenmode parameters have no impact on differential performance, both odd and evenmode parameters are set to the same values in the model.
The challenge then is to calculate the odd mode impedance (Zodd), representing the individual via impedance (Zvia), of a differential via structure and the effective dielectric constant (Dkeff) based on its geometry. Simple equations are used to determine these parameters.
Developing the Equations:
Antipads can vary in size and shape. They can be anything from round, to oval around each via, or even a large oval surrounding both vias as illustrated in Figure 4. Square, or rectangular variations (not shown) are similar.
Referring back to Figure 2, we see the structure of each via looks a lot like two coaxial transmission lines with the inner layer reference planes acting like a shield. Electrostatically this is a good approximation, but because the shield is not continuous, the magnetic fields are not contained like they are in a coaxial structure. Instead they behave more like magnetic fields around a twinrod structure.
So here lies the secret in modeling a differential via. We take the best of both geometries to calculate the oddmode impedance representing Zvia.
For inductance, we will use the oddmode inductance formula from the twinrod transmission line geometry to calculate Lvia :
Referring to Figure 4, we then calculate the oddmode capacitance for Cvia derived from an approximate formula for an elliptic coaxial structure developed by M.A.R. Gunston in his book, “Microwave Transmission Line Impedance Data” . In the original formula, both shield (W’+b) and inner conductor (w+t) are elliptical in shape and are dimensioned as shown. When the antipads are circular, then ln[(W’+b) /(w+t)] reduces to just ln[b/t)]; which is the denominator in the Coax equation. If we use Gunston’s approximation to calculate Cvia, then the equation becomes:
Since conventional FR4 type laminates are fabricated with a weave of glass fiber yarns and resin, they are anisotropic in nature. Because of this, the dielectric constant value depends on the direction of the electric fields. In a multilayer PCB, there are effectively two directions of electric fields.
The one we are most familiar with has the electric fields perpendicular to the surface of the PCB; as is the case of stripline shown here in Figure 5. The dielectric constant, designated as Dkz in this case, is normally the bulk value of the dielectric specified by the laminate manufacturer’s data sheet.
The other case has the electric fields running parallel to the surface of the PCB, as is the case when a signal propagates through a differential via structure. In this situation, the dielectric constant, designated as Dkxy, can be1520% higher than Dkz .
Therefore, assuming a nominal 18% anisotropic factor, Dkxy = 1.18(Dkz)
Now that we have defined Lvia, Cvia and Dkavg, Zvia can be estimated using the following equation:
But we are not finished yet. We still need to determine the effective dielectric constant (Dkeff) in order to accurately model the delay through the via and stub portion. Without the correct value, the quarterwave resonant nulls in the insertion loss plot, due to the stub length, cannot be accurately predicted. The value for Dkeff is determined based on how much the via’s oddmode impedance is decreased due to the distributed capacitive loading of the antipads.
To help us with this task, we start with the twinrod formula. The oddmode impedance (Zodd) is half the differential impedance (Ztwin), and is expressed as:
By substituting Equation 1 for Zodd into the equation above, and solving for Dkeff we eventually come up with the following equation:
Validating the Model:
A simple 26 layer test vehicle was fabricated to compare the accuracy of the differential via circuit model to real vias. It consisted of two differential via pairs separated by 6 inches of 100 Ohm stripline differential pairs. Three sample via structures representing long, medium and short via stubs, as summarized in Figure 6, were measured using an Agilent N5230A VNA.
The differential vias had the following common parameters:
Via drill diameter; D = 28 mils
Center to center pitch; s = 59 mils
Oval antipads= 53 mils x 73 mils
Dk of the laminate = 3.65
Anisotropy in Dkxy = 18%
Zvia = Zstub = 31.7 Ohms (per Equation 1)
Dkeff = 6.8 (per Equation 2)
Agilent ADS software was used to model and facilitate simulation correlation of the measured data as captured in Figure 7. This simple model accounts for the discontinuity of the long through section and the long stub section. The top half is the measured channel using an Sparameter file. The bottom half is a circuit model of the channel. Since the probes were not calibrated out, they are part of the device under test. The balun transformers are used to facilitate the display of the Sparameter and TDR results.
The comparison between the measured and simulated results of the insertion loss and TDR response for the three via stub cases using this simple approximation methodology is summarized in Figure 8. The insertion loss plots, in the frequency domain, are shown on the left, while the TDR plots are shown on the right.
The resonant nulls in the SDD21 plots are due to the stub lengths. As you can see, the longer the stub, the lower the resonant frequency null. If this null happens at the Nyquist frequency of the bit rate, the eye will be totally closed. This is why we backdrill them out after the board has been fabricated.
The simulation correlation is excellent up to about 12 GHz. The TDR plots show excellent impedance matching and delay for all three cases, while the simulated stub resonant frequencies match the measured frequencies very well. As you can see, these simple approximations for Dkeff and Zvia are perfectly adequate in providing a quick and accurate circuit model for differential through hole vias typically used in backplane applications.
Summary:
As illustrated, a simple twinrod model (Figure 2) is used as the basis for a practical differential via circuit modeling methodology. By using Equation 1 and Equation 2, you can quickly determine the oddmode impedance and effective dielectric constant needed for the circuit model.
Of course, you should use this methodology first as a rough starting point to quickly estimate the performance of your differential via design. If your worst case topology simulations show the performance is marginal, then it is worth while to invest the time and money to develop a 3D full wave model to perform a more accurate analysis.
On the other hand, if you find this approximation shows the vias have little impact on the channel performance, it may be of greater value for you to invest your time and money in resolving other critical issues with your design.
Try it the next time you are losing sleep over your design challenges.
For more Information:
If you liked this design note and want to learn more, or get more details on this innovative via modeling methodology, you can visit my web site, LAMSIM Enterprises.com , and download a copy of the white paper I wrote along with Eric Bogatin and Yazi Cao titled, “Method of Modeling Differential Vias” .
While you are there, feel free to investigate my other white papers and publications.
If you would like more information on our signal integrity and backplane services, or how we can help you achieve your next highspeed design challenge, email us at: info@lamsimenterprises.com.
UPDATE: In collaboration with Saturn PCB, I am pleased to announce my differential via equations above have been incorporated in a new impedance calculator available now in Saturn PCB Tool Kit software suite.