Bert Simonovich's Design Notes

Innovative Signal Integrity & Backplane Solutions

Archive for the ‘Modeling’ Category

Perils of Crossing Split Planes

with 2 comments

imageI recently came across this YouTube video spoof of Chuck Norris doing the spits across two aircraft wings above the clouds and it occurred to me that it was a perfect metaphor for what happens when a digital signal, propagating along a microstrip trace, crosses a split plane on a printed circuit board (PCB). If Chuck Norris and his merry band of paratroopers standing on his head were the signal, then at the split of two reference planes, we would see an impedance mismatch which manifests itself as a positive peak in the time domain reflection (TDR) plot for the duration of the discontinuity.

When discussing signal integrity (SI) issues there is always a great debate when signals on one layer of PCB crossing over split or a slot in the reference planes. On the one hand, some argue that this should never be done because of the increased risk in crosstalk and possible failure to pass electromagnetic compatibility (EMC) compliance. On the other hand, others stressed that if the width of the gap and power/ground layers in the stackup were engineered carefully, this may not be as big of an issue. So who’s right?

Well, like all things involving signal integrity, the answer is, “it depends”. And the best way to answer “it depends” is to put in the numbers.

When I decided to investigate this, I thought to myself I would just set up a couple of simple simulations to explore the issues. Of course, once you get into it, you find other scenarios to check out, then another, and before long you have amassed a lot of data. So I decided to capture it all in a white paper.

Here is a brief summary of the results.

To see just how much of an issue this is I set up a topology using Keysight ADS as shown in Figure 1. Two transmission line segments before and after the gap section (TL17, TL18) were modeled with internal 2D field solver. The gap section (SNP139) was modeled and simulated with Momentum 3D planar field solver in order to properly capture the electromagnetic effects as the signals cross the gaps. The S-parameter results were saved as touchstone format and brought back into the ADS schematic.

A 50 mil gap was chosen for worst case and a 5 mil gap was chosen for best case. As expected, when the topology was driven differentially from Port 1, the 50 mil gap results, shown in red, had a higher impedance discontinuity compared to the 5 mil gap, shown in blue.

image

Figure1 Keysight ADS general schematic (top) used to model and simulate a microstrip crossing a split plane. Red and blue plots (bottom) are differential impedance comparison of 50 mil vs 5 mil gaps respectively.

Figure 2 shows simulated results of incident/transmitted signals; near-end/far-end crosstalk (NEXT/FEXT) when the gap between the split planes was reduced from 50 mils (blue plots) down to 5 mils, and the thickness of dielectric from layer2 to layer 3 was reduced from 45 mils to 2 mils (red plots). Compared to the scenario with no gap (black plots) there was no appreciable increase in crosstalk.

image

Figure 2 Comparison of SE Incident/Transmitted voltage, NEXT/FEXT for 50 mil gap (blue) and thick dielectric under the gap vs 5 mil gap and thin dielectric under the gap (red). As expected the closer proximity of reference plane under the gap results in less incident reflection and NEXT while minimizing risetime degradation in transmitted signal and FEXT.

From a signal integrity perspective, one may conclude that crossing a split plane may be ok, with certain caveats. But in terms of passing EMC, there is still risk and doubt. For instance we see that there is still some current flow along each side of the split when we reduce the thickness between Layer 2 and 3. The combination of the split plane and diverted return current along the split creates an efficient slot antenna which will radiate noise.

Since a real design may have many interdependencies affecting the final performance, it is difficult to come up with a general rule that says if you do this, and minimize that you will be ok; and because of that, I’m still on the side of staying away from crossing split planes. When you can’t, then a more detailed analysis should be done based on the actual layout and stackup of the board; or look for other alternatives that can mitigate noise radiation; like adding extra external shielding for instance.

In the end it is what I always like to say about engineering, “it’s what you don’t know you don’t know that can ruin your day”. In today’s high-speed designs we can no longer restrict our thinking in terms of signal integrity, power integrity or EMC alone. We must consider all three and become educated or at least aware of the other disciplines. Had we only been concerned about signal integrity, without being aware of EMC we would have probably made the wrong conclusion, and in the end the final product might well have failed EMC compliance tests.

For more detail you can down load the white paper I wrote titled, “Split Planes and What Happens When Microstrip Signals Cross Them” from my web site here.

 

Written by Bert Simonovich

December 11, 2017 at 10:52 am

Practical Modeling of High-speed Channels

leave a comment »

As Dave Dunham from Molex Corp. likes to say, “When designing high-speed serial links beyond 10 GB/s, everything matters”. In order to ensure first time success at these speeds, accurate channel modeling is a prerequisite. This is especially true for long backplane channels.

imageAlthough many EDA tools include the latest and greatest models for conductor surface roughness and wide-band dielectric properties, obtaining the right parameters to feed the models is always a challenge. Often the only sources are from data sheets alone. But in most cases, the numbers do not translate directly into parameters needed for the EDA tools. So how do we get these parameters?

One way is to follow the design feedback method which involves designing, building and measuring a test coupon, then extracting the parameters through tuning simulation to measurement. Although this method is pretty practical and accurate, a significant amount of expertise and equipment is required to design, build and measure the test coupon, which takes significant amount of time and money.

But, as Eric Bogatin often likes to say, “Sometimes an OK answer NOW! is better than a good answer late.” As a high-speed signal integrity practitioner and backplane architect, I often have to come up with an answer sooner, rather than later because of the impact to time and cost to my clients. And that’s why I have been motivated over the last few years to research and develop simple methodologies to accurately determine parameters to feed into modern EDA tools.

If you went to this year`s EDICon 2017 in Boston, and attended the High-speed Digital Symposium session, you would have heard me speak on a “Practical Modeling of High-speed Channels Based on Data Sheet Input”, which was the title of my presentation.

For those of you who could not attend, I have made available an annotated slide deck. You can download a copy from my web site.

What you will learn:

  • How to use my Cannonball model to determine Huray roughness parameters from data sheet alone
  • How to determine effective dielectric constant due to roughness from data sheets alone
  • How to apply these parameters in the latest version of Polar Si9000e Field Solver
  • How to pull it all together using Keysight ADS software

And this is an example of simulation results compared to measurements you can expect to see:

image

Written by Bert Simonovich

October 20, 2017 at 10:19 am

Via Stubs Demystified

leave a comment »

imageWe worry about via stubs in high-speed designs because they cause unwanted resonant frequency nulls which appear in the insertion loss plot (IL) of the channel. But are all via stubs bad? Well, as with most answers relating to signal integrity, “It depends.”

If one of these frequency nulls happen to line up at or near the Nyquist frequency of the bit- rate (i.e. 1/2 of the bit-rate), the received eye will be devastated, resulting in a high bit-error-ratio (BER), or even link failure.

Figure 1 shows simulation results of two backplane channels. On the left are measured SDD21 insertion loss and eye diagram of a 10 GB/s, non-return-to-zero (NRZ) signal, with short through vias and long stubs ~ 270 mils. On the right, shows measured SDD21 IL and eye diagram of a channel with long through vias and shorter stubs ~ 65 mils

Because the ¼ -wave resonant null occurs at a frequency ~ 4. 4 GHz, this is near the Nyquist frequency for 10 GB/s. As can be seen, the eye is totally closed for the long stub case. But when the shorter stub case is simulated, the eye is open with plenty of margin.

So how does a via stub cause ¼ -wave resonance? This question can be explained with the aid of Figure 2. Starting on the left, we see a via with two sections. The through (thru) part is the top portion connecting a device pin to an inner layer trace of a printed circuit board (PCB). The stub portion is the lower portion and is an open circuit.

On the right a sinusoidal signal is injected into the pin at the top of the via and travels along the thru portion until it reaches the junction of the internal trace and stub. At that point, the signal splits. Some of it travels along the trace, and the rest continues down the stub. Once it reaches the bottom, it reflects back up. When it reaches the trace junction, it splits again with a portion traveling along the trace and the rest back to the source.

If f  is the frequency of a sine wave, and the time delay (TD) through the stub portion equals a ¼ -wavelength, then when it reflects at the bottom and reaches the junction again, it will be delayed by ½ a cycle and cancels most of the original signal.

image

Figure 2 Illustration of a ¼ -wave resonance of a stub. If f = frequency where TD = ¼ wavelength, then when 2TD = ½ cycle minimum signal received.

Resonance nulls occurs at the fundamental frequency ( fo) and at every odd harmonic. If you know the length of the stub (in inches) and the effective dielectric constant (Dkeff), surrounding the via hole structure, the resonant frequency can be predicted by:

Equation 1

image

Where: fo is the ¼ -wave resonant frequency (GHz); c is the speed of light (~11.8 in/ns); Stub_length is inches.

You will find that Dkeff is not the same as the bulk Dk published in laminate manufacturers’ data sheets. It is typically higher. A higher Dkeff increases phase delay through the via resulting in a lower resonant frequency.

One reason is excess capacitance from the via pads as well as the via barrel’s proximity to the clearance hole openings (also known as anti-pads) in plane layers. The other is because of the anisotropic nature of the laminate material.

For the example in Figure 1, the ¼ -wave resonant frequency of the long via stub is ~ 4.4 GHz. With a stub length of ~ 270 mils, this gives a Dkeff of 6.16, which is considerably higher than the published bulk Dk of 3.65. When you model a via in an electro-magnetic (EM) 3D field solver, it automatically accounts for the excess capacitance, but you will still need to compensate for the anisotropic nature of the dielectric.

A material is anisotropic when there are different values for parallel (x-y) vs perpendicular (z) measured values for dielectric constant. Dielectric constant and loss tangent, as published in manufacturers’ data sheets, report perpendicular measured values. For FR-4 fiberglass reinforced laminates, anisotropy can range from 15% -25% higher. The bad news is these numbers are not readily available from data sheets.

For differentially driven vias with plane layers evenly distributed throughout the entire stackup, Dkeff can be roughly estimated by:

Equation 2

image

Where: Dkxy is the dielectric constant adjusted for anisotropy (15%-25% higher); Dkz is the bulk dielectric constant from data sheets; s is via-via spacing; drillØ is drill diameter; H and W are anti-pad shape dimensions as shown in Figure 3 .

image

Figure 3 Anti-pad parameters for Equation 2.

The effects of via stubs can be mitigated by: using blind or buried vias; back-drilling; or by using thru vias only (i.e. from top layer to bottom layer). Practically, the shortest stub that can be achieved by back-drilling is on the order of 5 to 10 mils.

As a rule of thumb, we usually strive to have an interconnect bandwidth (BW) to be five times the Nyquist frequency of the bit-rate. Since a ¼-wave resonant null behaves somewhat like a notch filter, depending on the high-frequency roll-off due to Q-factor, frequencies near resonance will be attenuated. For that reason a good rule of thumb to follow is making sure the first null should occur at the 7th harmonic, or higher, of the Nyquist frequency to maintain the integrity of the 5th harmonic frequency component that makes up the risetime of a signal.

With this in mind, for a given baud-rate (Baud) in GBd/s, the maximum stub length (lmax), in inches can be estimated by:

Equation 3

image

For NRZ signaling, the baud-rate is equal to the bit rate. But for pulse-amplitude modulation (PAM-4) signaling, which has 2 symbols per bit time, the baud-rate is ½ of that. Thus a 56 GB/s PAM-4 signal has a baud-rate of 28 GBd/s, and the Nyquist frequency is 14 GHz, which happens to be the same as 28 GB/s NRZ signalling.

Figure 4 presents a chart of maximum stub length vs baud-rate based on Equation 3, using a Dkeff = 6.16 (blue) vs 3.65 (red). It shows us the higher the baud-rate, the more the stub length becomes an issue, especially past 10 GBd/s. We also get a feel for the sensitivity of stub length to Dkeff . Even though there is ~ 70% difference in Dkeff, there is only ~ 30% delta in stub lengths for the same baud-rate. This means that even if we use the bulk Dk published in data sheets, we are probably not dead in the water.

If the respective stub length is greater than this, it does not mean there is a show stopper. Depending on how much longer means the eye opening at the receiver will be degraded and we lose margin. We see this by the example in Figure 1. Even though the stub lengths in the channel were almost double the value at 10 GBd/s from the chart, there is still plenty of eye opening.

image

Figure 4 Chart showing estimated maximum stub length vs baud-rate with Dkeff of 6.16 (red) vs 3.65 (blue) based on Equation 3

To further explore design space and test out the rule of thumb, a generic circuit model was built using Keysight ADS with the ability to vary the via stub lengths

Referring to the chart, at 28 GBd/s, the maximum stub length should be 12 mils, assuming a Dkeff of 6.16. Figure 5 shows simulation results for NRZ signalling. As can be seen, there was a difference of only 17 mV in eye height (1.5%), and no extra jitter for 12 mil stubs compared to 5 mil stubs.

image

Figure 5 Eye diagrams comparison with BER at 10E-12 for stub lengths of 5 mils vs 12 mils. Modeled and simulated with Keysight ADS.

But if we use the exact same channel model, and use the generic PAM-4 IBIS AMI model from Keysight Technologies, we can see the results plotted in Figure 6. On the left are the eye openings with 5 mil stubs and the right with 12 mil stubs. In this case, there was an average reduction of ~7 mV (6%) in eye heights, and 0.24 ps (2%) in eye widths at BER 10E-12 across all three eyes.

image

Figure 6 PAM-4, 28 GBd/s (56 GB/s) eye height and width comparison at BER of 10E-12 for 5 mil vs 12 mil stub lengths. Modeled and simulated with Keysight ADS.

Because PAM-4 signalling has three smaller eyes, that are one-third the size of an NRZ eye for the same amplitude, it is more sensitive to channel impairments. From the above examples, we can see NRZ had only 1.5% reduction in eye height compared to 6% for PAM-4. Similarly there was no increase in jitter for NRZ compared to 2% increase for PAM-4 when stub lengths changed from 5 mils to 12 mils.

What this says is maintaining a BW to 5 times Nyquist rule of thumb, when estimating via stub lengths, is quite conservative for NRZ signalling. There is almost the same BW as the channel with 5 mil stub, which was the original objective. But because PAM-4 is more sensitive to impairments, it shows there is less margin.

In summary then, rules of thumb and related equations are a good way to reinforce your intuitions or to give you an answer sooner rather than later. They help you know what to expect before you take any measurements or perform any simulations. But they should never be used to sign off on any high-speed design.

Because every system will have different impairments affecting BER, the only way to know how much margin you have is by modeling the via with a 3-D EM field solver, based on the actual stackup and simulating the entire channel complete with crosstalk, if margins are tight. This is even more critical for data rates above 10 GBd/s.

So to answer the original question, “are all via stubs bad”? Well, the answer is it still depends. For NRZ signalling, there is more leeway than for PAM-4. But you now have a practical way to quickly quantify the answer if you know the stub length, baud-rate and delay through the via.

Written by Bert Simonovich

March 8, 2017 at 2:35 pm

Obsessions with Conductor Surface Roughness – What’s the Dk Because of it?

leave a comment »

clip_image002You know you have an obsession when you are flying 6 miles over Colorado; look out your window at the beautiful scenery; and all you can think about is how the rocky mountain topology reminds you of conductor surface roughness! Well call me obsessed because that’s exactly what I thought on my way to DesignCon 2017 in Santa Clara, CA.

For those of you who know me, you know that I have been researching practical methods to model conductor surface roughness, and its effect on insertion loss (IL). I have presented several papers on the subject over the last couple of years. It’s one of my pet projects. This year, at DesignCon, I presented a paper titled, “A Practical Method to Model Effective Permittivity and Phase Delay Due to Conductor Surface Roughness” .

Everyone involved in the design and manufacture of printed circuit boards (PCBs) knows one of the most important properties of the dielectric material is the relative permittivity (εr), commonly referred to as dielectric constant (Dk). But in reality, Dk is not constant at all. It varies over frequency as you will see later.

We often assume the value reported in manufacturers’ data sheets is the intrinsic property of the material. But in actual fact, it is the effective dielectric constant (Dkeff) generated by a specific test method. When you compare simulation against measurements, you will often see a discrepancy in Dkeff and IL, due to increased phase delay caused by surface roughness. This has always bothered me. For a long time I was always looking for ways to come up with Dkeff from data sheet numbers alone. Thus the obsession and motivation for my recent research work.

Since phase delay, also known as time delay (TD), is proportional to Dkeff of the material, my theory was that the surface roughness profile decreases the effective separation between parallel plates, thereby increasing the electric field (e-field) strength, resulting in additional capacitance, which accounts for an increase in effective Dk and TD.

The main focus of my paper was to prove the theory and to show a practical method to model Dkeff and TD due to surface roughness. By referencing Gauss’s Law for charged parallel plates, I confirmed mathematically, and through simulation, how the dielectric thickness and permittivity are interrelated to e-field and capacitance. I also revealed how the 10-point mean (Rz) roughness parameter can be applied to finally estimate effective Dkeff due to roughness. Finally I tested the method via case studies.

In his book, “Transmission Line Design Handbook”, Wadell defines Dkeff as the ratio of the actual structure’s capacitance to the capacitance when the dielectric is replaced by air.

Dkeff is highly dependent on the test apparatus and conditions of how it is measured. There are several methods used in the industry. One method that is commonly used by many laminate suppliers is called the clamped stripline resonator test method. It is described by IPC-TM-650, section 2.5.5.5, Rev C.

In short, this method rapidly tests dielectric material for permittivity and loss tangent, over an X-band frequency range of 8-12.4 GHz, in a production environment. It does not guarantee the values are accurate for design applications.

Here’s why:

The measurements are made under stripline conditions, using a carefully designed resonant element pattern card, made out of the same dielectric material to be tested. The card is sandwiched between two sheets of unclad dielectric material under test. The whole structure is then clamped between two large plates, lined with copper foils that are grounded.

Since the resonant element pattern card and material under test are not physically bonded together, there are small air gaps between the various layers affecting measured results. These air gaps are caused in part by:

  • Removing the copper from the material under test, leaving the bare substrate, complete with the micro void imprint of the copper roughness.
  • The air gap between resonant element pattern card and material under test, due to the copper thickness of the etch pattern.
  • The roughness profile of the copper, on the resonant element pattern card and fixture’s grounded foil reference planes, are different than would be in practice, unless the same foil type is used.

If Dkeff and Rz roughness parameters from the manufacturers’ data sheets are known, then the effective Dk due to roughness (Dkeff_rough) of the fabricated core laminate can now be easily estimated by:

Equation 1

image

Where: Hsmooth is the thickness of dielectric from data sheet; Rz is 10-point mean roughness from data sheet; and Dkeff is the Dk from data sheet.

With reference to Figure 1, using Dkeff with rough copper model, as shown on the left, is equivalent to using Dkeff_rough, with smooth copper model, as shown on the right. Therefore all you need to do is use Dkeff_rough for impedance calculations, and any other numerical simulations based on surface roughness, instead of Dk published in data sheets.

It is as simple as that.

image

Figure 1 Effective Dk due to roughness model. Using Dkeff with rough copper model (left) is equivalent to using Dkeff_rough with smooth copper model (right).

For example, one case study I presented used measurements from a CMP28 modeling platform from Wild River Technology. The PCB was fabricated with FR408HR material and reverse treated foil (RTF). Keysight EEsof EDA ADS software was used for modeling and simulation. The results are shown in Figure 2.

The left graph shows results when data sheet values for core and prepreg were used. Dkeff measured (red) was 3.761, compared to simulated Dkeff (blue) of 3.626, at 10 GHz. This gave a delta of ~ 4%. But when the Dkeff_rough was used for core and prepreg the delta was within 1%.

image

Figure 2 Measured vs simulated Dkeff using FR408HR data sheet values for core and prepreg (left) and using Dkeff_rough (right). Modeled and simulated with Keysight EEsof EDA ADS software.

The paper shows in more detail how Equation 1 was derived, based on Gauss’ Law. In addition, I show how IL and phase delay is also improved when Dkeff_rough is used instead of data sheet values. You can download the paper titled, “A Practical Method to Model Effective Permittivity and Phase Delay Due to Conductor Surface Roughness”, and other papers on modeling conductor loss due to roughness from my web site.

Written by Bert Simonovich

February 21, 2017 at 10:48 am

Practical Conductor Roughness Modeling with Cannonballs

leave a comment »

image

In the GB/s regime, accurate modeling of conductor losses is a precursor to successful high-speed 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, close-packing of equal spheres is defined as “a dense arrangement of congruent spheres in an infinite, regular arrangement (or lattice)[8].  The cubic close-packed and hexagonal close-packed are examples of two regular lattices.  The cannonball stack is an example of a cubic close-packing of equal spheres, and is the basis of modeling the surface roughness of a conductor in this design note.

image

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.

Electro-deposited (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

·         Very-low profile (VLP)

·         Ultra-low 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 electro-deposited copper. Tooth profiles are typically reported in terms of 10-point mean roughness (Rz ) for both sides, but sometimes the drum side reports average roughness (Ra ) in manufacturers’ data sheets. Some manufacturers also report RMS roughness (Rq ).

Modeling Roughness

Several modeling methods were developed over the years to determine a roughness correction factor (KSR ). When multiplicatively applied to the smooth conductor attenuation (αsmooth ), the attenuation due to roughness (αrough ) can be determined by:

Equation 1

image

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 (KHJ ), 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

image

Where:

KHJ = 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 skin-effect. The resulting skin-depth (δ ) is the effective thickness where the current flows around the perimeter and is a function of frequency.

Skin-depth at a particular frequency is determined by:

Equation 3

image

Where:

δ = skin-depth in meters;

f = sine-wave frequency in Hz;

μ0= permeability of free space =1.256E-6 Wb/A-m;

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 non-uniform 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.

image

Figure 2 SEM photograph of electrodeposited copper nodules on a matte surface resembling “snowballs” on top of heat treated base foil. Photo credit Oak-Mitsui.

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

image

Where:

KSRH (f ) = roughness correction factor, as a function of frequency, due to surface roughness based on the Huray model;

Aflat= relative area of the matte base compared to a flat surface;

 ai = radius of the copper sphere (snowball) of the ith size, in meters;

 Ni = number of copper spheres of the ith size per unit flat area in sq. meters;

 δ (f ) = skin-depth, as a function of frequency, in meters.

Cannonball Model

Using the concept of cubic close-packing of equal spheres, the radius of the spheres (ai ) and tile area (Aflat ) 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 what-if 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.

image

Figure 3 Cannonball model showing a stack of 14 uniform size spheres (left). Top and front views (right) shows the area (Aflat) of base, height (HRMS) and radius of sphere (r).

Because the Cannonball model assumes the ratio of Amatte/Aflat = 1, and there are 14 spheres, Equation 4 can be simplified to:

Equation 5

image

Where:

KSR (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 ) = skin-depth, as a function of frequency in meters;

Aflat = 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:

image

And the area of the square flat base is:

image

You can approximate the RMS heights of the drum and matte sides by Equation 6 and Equation 7 below:

Equation 6

image

Where: Rz_drum is the 10-point mean roughness in meters. If the data sheet reports average roughness, then Ra_drum is used instead.

Equation 7

image

Where: Rz_matte is the 10-point 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 de-embedded generalized modal S-parameter (GMS) data was computed from 2 inch and 8 inch single-ended stripline traces. They were originally measured from the CMP-28 40 GHz High-Speed Channel Modeling Platform from Wild River Technology [14].

imageThe CMP-28 Channel Modeling Platform, (Figure 4 left -credit Wild River Technology) is a powerful tool for development of high-speed 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® web-based 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 cross-section after etching due to etch factor. Since the tool does not handle trapezoidal cross-sections in the impedance calculation, an equivalent rectangular trace width was determined based on a 2:1 etch-factor (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.

image

Figure 5 Example of Isola’s isoStack® online software used to determine dielectric thicknesses, Dk, Df and characteristic impedance for the CMP-28 board.

The default foil used on FR408HR core laminates is MLS, Grade 3, controlled elongation RT foil. The roughness parameters were easily obtained from Oak-mitsui [11]. Reviewing the data sheet, 1 oz. copper roughness parameters Rz 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 micro-etch treatment is usually applied to the copper surfaces prior to final lamination. This provides enhanced adhesion to the prepreg material. CO-BRA BOND® [12] or MultiBond MP [13] are two examples of oxide alternative micro-etch 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 70-100 μin (1.78-2.54μm) or higher.

The etch treatment creates a surface full of micro-voids 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 micro-etch 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 Oak-mitsui. 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 micro-voids after etch treatment.

image

Figure 6 Example SEM photos of MLS RT foil courtesy of Oak-mitsui. 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 Oak-mitsui data sheet. Rz of the matte side after micro-etch treatment (Rz = 4.443μm) was used to determine KSR_matte .

Table 1 CMP-28 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

Rz Drum side

3.048 μm

Rz Matte side before Micro-etch

5.715 μm

Rz Matte side  after Micro-etch

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.

image

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 much-much 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

image

To accurately model the effect of roughness, the respective roughness correction factor (KSR ) 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 (KSR_drum ) and (KSR_matte ) side to the smooth conductor loss (ILsmooth ), as described above.

The following are the steps to determine KSR_avg (f ) and total IL with roughness:

1. Determine HRMS_drum and HRMS_matte from Equation 6 and Equation 7. 

  image

2. Determine the radius of spheres for drum and matte sides:
image

3. Determine the area of the square flat base for drum and matte sides:
image

4. Determine KSR_drum (f ) and KSR_matte (f ) :
image

5. Determine the average KSR_drum (f ) and KSR_matte (f ):
image

6. Apply Equation 8 to determine total insertion loss of the PCB trace.

image

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!

image

Figure 8 IL (left) for a 6 inch trace in FR408HR RTF using supplier data sheet values for Dk, Df and Rz. Effective Dk is shown right.

image

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.

image

Figure 10 Cannonball Model (left) vs Hammerstad-Jensen model (right).

Conclusions

Using the concept of cubic close-packing 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 CMP-28 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 high-speed 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 Computer-Aided Design,” Microwave symposium Digest, 1980 IEEE MTT-S International , vol., no., pp.407,409, 28-30 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 High-Speed 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. 12-28. URL: http://iconnect007.uberflip.com/i/258943-pcbd-feb2014/12

[6]   Y. Shlepnev, “Sink or swim at 28 Gbps”, The PCB Design Magazine, October 2014, p. 12-23. URL: http://www.magazines007.com/pdf/PCBD-Oct2014.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, “Close-packing of equal spheres”. URL: http://en.wikipedia.org/wiki/Close-packing_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.isola-group.com/

[11]    Oak-mitsui 80 First St, Hoosick Falls, NY, 12090. URL: http://www.oakmitsui.com/pages/company/company.asp

[12]    Electrochemicals Inc. CO-BRA BOND®. URL: http://www.electrochemicals.com/ecframe.html

[13]    Macdermid Inc., Multibond. URL: http://electronics.macdermid.com/cms/products-services/printed-circuit-board/surface-treatments/innerlayer-bonding/index.shtml

[14]    Keysight Technologies, EEsof EDA, Advanced Design System, 2015.01 software. URL: http://www.keysight.com/en/pc-1297113/advanced-design-system-ads?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

Are Guard Traces Worth It?

leave a comment »

Originally  published in, The PCB Design Magazine, April 2013 issue.

clip_image002By 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 high-speed 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 end-termination resistors, on the guard trace, could be deactivated, and/or shorted, as required. The line-width space geometry was set at 5-5-5 mils, and the spacing for the non-guarded topologies was set to three times the line width.

image

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 end-termination 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 two-line 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 three-line 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 far-end 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.

image

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.

image

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.

image

Figure 4 Minimum track to track spacing to fit an 8 mil drilled via and pad in through-hole 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.

image

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 pad-track 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 S-parameter 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 well-known 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.

image

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 peak-peak amplitude of the noise just about equals the peak magnitude of the no guard case.

image

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.

image

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

  1. Eric Bogatin, Bert Simonovich,Dramatic Noise Reduction using Guard Traces with Optimized Shorting Vias, DesignCon2013, Santa Clara, CA, USA, Jan 28-31, 2013.

Written by Bert Simonovich

April 12, 2013 at 2:36 pm

PCB Vias Are Capacitive But Not Necessarily Capacitors

with 3 comments

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 high-speed 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 multi-layer PCBs are capacitive because of the distributed capacitance between the via barrel and anti-pads. 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.

image

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.

image

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.

image

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 S-parameter 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.

image

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 one-half 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 S-parameters 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 bit-rates up to 3.6GB/s.

Equation 1 is a commonly used to convert 3dB bandwidth to equivalent 10-90 rise time. Substituting 1.83 GHz for the 3dB bandwidth, the rise time equals approximately 185 ps.

Equation 1

image

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 bit-rate 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.

image

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:

image

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 high-speed design challenge, email us at: info@lamsimenterprises.com.

Written by Bert Simonovich

May 15, 2011 at 8:44 pm

%d bloggers like this: