Archive for the ‘Printed Circuit Boards’ Category
Practical Modeling of Highspeed Channels
As Dave Dunham from Molex Corp. likes to say, “When designing highspeed 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.
Although many EDA tools include the latest and greatest models for conductor surface roughness and wideband 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 highspeed 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 Highspeed Digital Symposium session, you would have heard me speak on a “Practical Modeling of Highspeed 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:
Via Stubs Demystified
We worry about via stubs in highspeed 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 bitrate), the received eye will be devastated, resulting in a high biterrorratio (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, nonreturntozero (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.
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 ( f_{o}) and at every odd harmonic. If you know the length of the stub (in inches) and the effective dielectric constant (Dk_{eff}), surrounding the via hole structure, the resonant frequency can be predicted by:
Equation 1
Where: f_{o} 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 Dk_{eff} is not the same as the bulk Dk published in laminate manufacturers’ data sheets. It is typically higher. A higher Dk_{eff} 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 antipads) 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 Dk_{eff} of 6.16, which is considerably higher than the published bulk Dk of 3.65. When you model a via in an electromagnetic (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 (xy) vs perpendicular (z) measured values for dielectric constant. Dielectric constant and loss tangent, as published in manufacturers’ data sheets, report perpendicular measured values. For FR4 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, Dk_{eff} can be roughly estimated by:
Equation 2
Where: Dk_{xy} is the dielectric constant adjusted for anisotropy (15%25% higher); Dk_{z} is the bulk dielectric constant from data sheets; s is viavia spacing; drillØ is drill diameter; H and W are antipad shape dimensions as shown in Figure 3 .
Figure 3 Antipad parameters for Equation 2.
The effects of via stubs can be mitigated by: using blind or buried vias; backdrilling; or by using thru vias only (i.e. from top layer to bottom layer). Practically, the shortest stub that can be achieved by backdrilling 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 bitrate. Since a ¼wave resonant null behaves somewhat like a notch filter, depending on the highfrequency rolloff due to Qfactor, 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 7^{th} harmonic, or higher, of the Nyquist frequency to maintain the integrity of the 5^{th} harmonic frequency component that makes up the risetime of a signal.
With this in mind, for a given baudrate (Baud) in GBd/s, the maximum stub length (l_{max}), in inches can be estimated by:
Equation 3
For NRZ signaling, the baudrate is equal to the bit rate. But for pulseamplitude modulation (PAM4) signaling, which has 2 symbols per bit time, the baudrate is ½ of that. Thus a 56 GB/s PAM4 signal has a baudrate 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 baudrate based on Equation 3, using a Dk_{eff} = 6.16 (blue) vs 3.65 (red). It shows us the higher the baudrate, 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 Dk_{eff }. Even though there is ~ 70% difference in Dk_{eff}, there is only ~ 30% delta in stub lengths for the same baudrate. 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.
Figure 4 Chart showing estimated maximum stub length vs baudrate with Dk_{eff} 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 Dk_{eff} 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.
Figure 5 Eye diagrams comparison with BER at 10E12 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 PAM4 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 10E12 across all three eyes.
Figure 6 PAM4, 28 GBd/s (56 GB/s) eye height and width comparison at BER of 10E12 for 5 mil vs 12 mil stub lengths. Modeled and simulated with Keysight ADS.
Because PAM4 signalling has three smaller eyes, that are onethird 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 PAM4. Similarly there was no increase in jitter for NRZ compared to 2% increase for PAM4 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 PAM4 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 highspeed 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 3D 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 PAM4. But you now have a practical way to quickly quantify the answer if you know the stub length, baudrate and delay through the via.
Obsessions with Conductor Surface Roughness – What’s the Dk Because of it?
You 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 (ε_{r}), commonly referred to as dielectric constant (D_{k}). But in reality, D_{k} 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 (D_{keff}) 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 (efield) strength, resulting in additional capacitance, which accounts for an increase in effective D_{k} 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 efield and capacitance. I also revealed how the 10point mean (R_{z}) 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 D_{keff} as the ratio of the actual structure’s capacitance to the capacitance when the dielectric is replaced by air.
D_{keff} 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 IPCTM650, section 2.5.5.5, Rev C.
In short, this method rapidly tests dielectric material for permittivity and loss tangent, over an Xband frequency range of 812.4 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 D_{keff} and R_{z} roughness parameters from the manufacturers’ data sheets are known, then the effective D_{k} due to roughness (D_{keff}_{_rough}) of the fabricated core laminate can now be easily estimated by:
Where: H_{smooth} is the thickness of dielectric from data sheet; R_{z} is 10point mean roughness from data sheet; and D_{keff} is the D_{k} from data sheet.
With reference to Figure 1, using D_{keff} with rough copper model, as shown on the left, is equivalent to using D_{keff}_{_rough}, with smooth copper model, as shown on the right. Therefore all you need to do is use D_{keff}_{_rough} for impedance calculations, and any other numerical simulations based on surface roughness, instead of D_{k} published in data sheets.
It is as simple as that.
Figure 1 Effective D_{k }due to roughness model. Using D_{keff} with rough copper model (left) is equivalent to using D_{keff}_{_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. D_{keff} measured (red) was 3.761, compared to simulated D_{keff} (blue) of 3.626, at 10 GHz. This gave a delta of ~ 4%. But when the D_{keff_rough} was used for core and prepreg the delta was within 1%.
Figure 2 Measured vs simulated D_{keff} using FR408HR data sheet values for core and prepreg (left) and using D_{keff_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 D_{keff_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.
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.
PCB Vias – An Overview
Vias make electrical connections between layers on a printed circuit board. They can carry signals or power between layers. For backplane designs, the most common form of vias use plated through hole (PTH) technology. They connect the pins of connectors to inner signal layers. A PTH via is formed by drilling a hole through the layers to be connected and then copper plating it.
High Density Interconnects (HDI) is another via technology used to form very small vias where drilling holes, using a conventional drill bit, is impractical. Also known as microvias, this technology creates the hole with a laser before plating.
Via Aspect Ratio
Via aspect ratio is defined as the ratio of the circuit board thickness to the smallest unplated drilled hole diameter. It is an important metric you need to be aware of when specifying the minimum via hole size for your design, and designing your stackup. For example, an unplated via with a drill diameter of 0.020 inches and a board thickness of 0.200, would have an aspect ratio of 10:1. The smaller the aspect ratio, the more consistent the plating is throughout the length of the via. It is desirable to have 2 mil plating thickness for the via walls. Large aspect ratio vias tend to have more plating at each end compared to the middle. This increases the chance of cracked via barrels due to zaxis expansion while soldering.
An aspect ratio of 6:1 pretty much ensures your board can be fabricated anywhere. Most highend board shops have the capability of fabricating boards with 10:1 aspect ratio; for drill diameters of less than 0.020 inches. Practically, the smallest drill diameter used for a through holed via is 0.013 inches. At 10:1, the maximum board thickness would be 0.130 inches.
For drill diameters larger than 0.020 inches, the max aspect ratio can be anywhere from 15:1 to over 20:1; depending on the board shop. Since backplane via hole size is driven by the compliant pins of the connector, it is best to work with your board shop to determine the maximum board thickness they can fabricate with the minimum finished hole size (FHS) specified in the design.
Via Configurations
The following lists the various via configurations you might expect to find on any multilayer PCB design:

Stub Via

Through Via
 Blind or Microvia

Buried Via

Backdrilled Via
Stub Via
The Stub Via is the most common via configuration found in PCBs today. As illustrated, there are two variations; Stub Via A and Stub Via B.
For the Stub Via A example, it shows the through portion starting from the top layer and ending at some inner layer. The stub portion is the remaining portion continuing from the inner layer junction to the bottom layer.
The Stub Via B example shows the through portion originating from one internal signal layer and terminating on another internal signal layer. In this scenario, there are two stubs. The first stub is from the first internal layer junction to the top layer; the second stub is from the second internal layer junction to the bottom layer.
Through Via
Through vias are the oldest and simplest via configurations originally used in 24 layer PCB designs. Since the signals originate and terminate from the outer layers of the PCB, there are no stubs. In multilayer PCB applications, they are an inexpensive way to eliminate the resonance effects caused by stubs where other mitigation techniques are not practical or are too expensive.
Blind/Buried Via
Blind and buried vias are just like any other via, except they do not go all the way through the PCB. A Blind Via connects one or more internal layers to only one external layer. Controlleddepth drilling is used to form the holes prior to plating.
A buried via, on the other hand, is a plated hole which is completely buried within the board. It connects one or more internal layers and does not connect to an external layer. Using buried via technology is costly because the inner layers being interconnected need to be fully fabricated and plated before final lamination of the entire PCB.
A microvia is a form of blind via. Because the holes are so small (0.006 inches or less), they are formed using lasers, and cannot penetrate more than one or two layers at a time. They are most commonly used in highdensity PCB designs like cell phones, or in FPGA and custom ASIC chip packaging.
Backdrilled Via
High speed pointpoint serial link based backplanes are often thick structures; due to the system architecture and cardcard interconnect requirements. Backdrilling the via stub is common practice on thick PCBs to minimize stub length for bitrates greater than 3Gb/s.
Backdrilling is a process to remove the stub portion of a PTH via. It is a postfabrication drilling process where the backdrilled hole is of larger diameter than the original PTH. This technology is often used instead of blindvia technology to remove the stubs of connector vias in very thick highspeed backplane designs. State of the art board fabrication shops are able to backdrill to within 8 mils of the signal layer to keep, so there will always be a small stub portion attached to the via.
Backdrilling is not without limitations. Smaller vias and tighter pitch driven by large pin count BGA packages makes backdrilling impractical in these applications; due to drill bit size and tolerance issues. Fortunately, smaller via diameters limit the maximum PCB thickness due to aspect ratio; thereby limiting the length of the stub to the board thickness. Careful planning the highspeed layers within the stackup is one way to control stub length.
We worry about stubs in highspeed designs because they cause unwanted resonant frequency nulls which appear in the insertion loss plot of the channel. If one of these frequency nulls happen to line up at or near the Nyquist frequency of the bit rate, the received eye will be devastated resulting in a high biterrorrate; even link failure. A shorter stub length means these resonances will be pushed out further in frequency; ideally past the 5th harmonic of the Nyquist frequency as a rule of thumb.
Rules of thumb, in general, are no substitute for actual modeling and simulation. You should never depend on them to signoff the final design; but you can use them to gain some intuition before hand. With that in mind, you can estimate the maximum stub length in inches using the following equation:
Where:
L _{Stub_max }= maximum stub length in inches.
Dkeff = effective dielectric constant of the material surrounding the via hole structure.
BR = Bit rate in GB/s.
For example, the maximum stub length at 5GB/s should be less than 0.120 inches in FR4 material with a Dkeff of 4.0 to ensure the first resonant frequency null is greater than 5 times the Nyquist frequency of the bit rate. If the stub length is greater than this, it does not mean the design will not work at 5GB/s. Depending on just how much longer it is means there will be less than optimum eye opening at the receiver.
If you know the length of the stub, you can predict the fundamental resonant frequency, using the following equation:
Where:
Stub_len = stub length in inches.
f_{o} = fundamental resonant frequency in GHz
So, using the same Dkeff of 4.0, and stub length of 0.120 inches, we calculated in the above example, the first resonant frequency null would occur at approximately 12.3 GHz. If we assume this is the 5th harmonic, then the Nyquist frequency is approximately 2.5GHz and the bit rate is 5Gb/s; which is where we started.
PCB Crosssectional Geometries
PCB crosssectional geometries describe the details of the dielectric substrates, traces and reference planes within a PCB stackup. Their physical relationship with one another can then be used to predict the characteristic impedance of the respective traces. There are only three generic crosssectional geometries with variations within each. They are:

Coplanar

Microstripline

Stripline
Coplanar:
Coplanar geometry, or sometimes called coplanar waveguide (CPW), is a signal conductor sandwiched between two coplanar reference conductors or planes. These reference planes are usually ground. The characteristic impedance is controlled by the signal trace width and the gap between it and reference planes. This is a common transmission line structure for RF and microwave designs using singlesided printed circuit board technology. As a rule of thumb, the width of the reference plane on each side of the signal trace should be at least five times the distance between the left and right plane.
Microstrip line:
The microstrip line is the most popular transmission line geometry used in two or four layer printed circuit boards. The characteristic impedance is controlled by the signal trace width, on one side of the substrate, and the thickness of the substrate to the reference plane below it. The embedded microstrip line has the signal trace covered with prepreg or other dielectric material.
Cross section views below showing Microstrip line (left) and embedded microstrip line (right).
Stripline:
Cross section views below shows an example of single stripline (left) and dual stripline (right) geometries. These are geometries are typically found in multilayer PCBs of 6 layers or more. The characteristic impedance is controlled by the trace width, thickness and its proximity to the reference planes above and below.
Single stripline has one signal layer sandwiched between two reference planes. If the signal layer is exactly spaced between the two reference planes, the geometry is called a symmetrical stripline; as opposed to an asymmetrical stripline, where the signal trace is offset from the center of the crosssection.
Dual stripline geometries have two signal layers sandwiched between reference planes, and are mainly used to save layers; caveat is a trace on one layer is routed orthogonal to the trace on the other to mitigate crosstalk.
Differential Pair Geometry:
Differential signaling is when a signal and its complement are transmitted on two separate conductors. These conductors are called a differential pair. In a PCB, both traces are routed together with a constant space between them as edgecoupled or broadsidecoupled.
Edgecoupled routes the traces sidebyside on the same layer as microstrip or stripline. The advantage is that any noise on the reference plane(s) is common to both traces and thus cancelled at the receiver. Most differential pairs are routed this way.
Broadsidecoupled routes one trace exactly over the other on 2 separate layers as dual stripline. Since each trace is more tightly coupled to its adjacent reference plane than the opposite reference plane, any noise on the planes will not be common to both traces and thus, will not be cancelled at the receiver. Because of this, and the fact that it usually results in a thicker PCB, this geometry is rarely used.
OddMode Impedance:
Consider a pair of equal width microstrip line traces, labeled 1 and 2, with a constant spacing between them. Each individual trace, when driven in isolation, will have a characteristic impedance Zo, defined by the selfloop inductance and selfcapacitance of the trace with respect to the reference plane.
When a pair of traces are driven differentially, the mode of propagation is odd. If the spacing between the transmission lines is close, there will be electromagnetic coupling between the two traces. This coupling is defined by the mutual inductance and capacitance.
The proximity of the traces to a reference plane(s) influences the amount of electromagnetic coupling between traces. The closer the traces are to the reference plane(s), the lower the selfloop inductance and stronger selfcapacitance to the plane(s); resulting in a lower mutual inductance, and weaker mutual capacitance between traces. The result is a lower differential impedance.
A 2D field solver is usually used to extract the parameters for a given geometry. Once the RLGC parameters are extracted, an L C matrix can be set up as follows:
The selfloop inductance and selfcapacitance for trace 1 and 2 are L11, C11, L22, C22 respectively. The off diagonal terms in each matrix, L12, L21, C12, C21, are the mutual inductance and mutual capacitance. We use the LC matrix to determine the oddmode impedance.
The oddmode impedance is the impedance of one trace, of a differential pair, when driven differentially. It can be calculated by the following equation:
Where:
Zodd = odd mode impedance
Lo = selfloop inductance = L_{11} = L_{22}
Co = selfcapacitance = C_{11} = C_{22 }
Lm = mutual inductance = L_{12} = L_{21}
Cm = mutual capacitance = C_{12} =C_{21}
Even Mode Impedance:
When current flows down both traces, of the same polarity, the mode of propagation is even and the coupling is positive. The even mode impedance can be calculated using the following equation:
Differential Impedance:
The differential impedance is twice the oddmode impedance:
Average Impedance:
When current flows down two traces randomly, as if they were singleended, the mode of propagation is a combination of odd and even. The average impedance of each trace is affected by its proximity to the adjacent trace(s); calculated by the following equation:
Coupling Coefficient:
The coupling coefficient, Kcc, is a number that conveys the amount of electromagnetic coupling between two traces. Knowing the odd and even mode impedance, Kcc can be calculated by the following equation:
Backward Crosstalk Coefficient:
Two traces near one another will couple a portion of its own signal to the other. If we consider one trace as the aggressor, and the other as the victim, the amount of coupled noise travelling backwards on the victim’s trace, opposite to the aggressor’s direction, is called NearEnd crosstalk (NEXT) or backwards crosstalk. The amount of coupled noise, travelling in the same direction as the aggressor’s direction, is called FarEnd crosstalk (FEXT).
In stripline, there is little to no FEXT, but backwards crosstalk will saturate to a fraction of the amplitude of the aggressor’s voltage for the length of time the traces are coupled. This fraction of the aggressor’s voltage is called the backward crosstalk coupling coefficient Kb. It is equal to one half of the coupling coefficient Kcc :
Example:
A 898 mil differential pair; with 12mil core; 12 mil prepreg; Dk=4; stripline geometry; 1/2 oz copper; has the following R L G C matrix extracted from a 2D field solver:
If the two traces are driven differentially, then the differential impedance is 100 Ohms and there is 13% coupling of the two traces. On the other hand, if the traces are driven singleended then the characteristic impedance of each trace is 53 Ohms. With 9 mils of space between them, the backward crosstalk is 7%.
If you increase the spacing between traces until Zodd equals approximately Zeven, the coupling will reduce to near zero, and there will be little backward crosstalk. Depending on your design and your noise budget, you may be able to live with a certain amount of backwards crosstalk. The only way to know the spacing between traces to achieve the budget is to plug in the numbers.
Acknowledgment:
I would like to thank my old Nortel colleague, the late Dick Goulette, for sharing these equations many years ago. They have served me well over the years.
Via Stub Termination Brought to You by “The Stubinator”
Thick backplanes with long via stubs will cause unwanted resonances in the channel insertion loss compared to vias with little or no stub length as shown by the red and green traces in the plot of Figure 1. If these resonances occur at or near the Nyquist frequency of the bit rate, there will be little or no eyeopening left at the receiver.
Figure 1 Topology circuit model of 2 differential vias with 30 inches of PCB etch. Insertion loss plot of Long viano stub (green); short vialong stub (red); stub terminated (blue). Received eye diagrams after optimized FFE receive equalization at 10GB/s. Modeled and simulated using Agilent ADS.
In a typical backplane application, the signal entering the via structure from the top will travel along the through portion until it reaches the junction of the internal track and stub. At that point, the signal splits with some of the signal continuing along the trace, and the rest continuing along the stub. If the signal was Arnold Schwarzenegger, he would say, “I’ll be back!”. Having done this gig before, he knows that when he reaches the end of the stub it’s like hitting a brick wall; there’s no where to go but back up the stub. Like Arnold, when the signal reaches the end of the stub, it reflects back up the stub. When it arrives at the same junction, a portion combines with the original signal and the rest continues back toward the source. If the round trip delay is half a cycle, the two waves are completely 180 degrees out of phase and there is cancellation of the original signal. The frequency where maximum cancellation occurs is called the ¼ wave resonant frequency, fo. Resonance nulls due to stubs in an insertion loss plot, like the one shown in Figure 1, 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, the resonant frequency can be predicted with the following formula:
(1)
It is common practice to reduce stub lengths in highspeed backplane designs by backdrilling the stubs as close as possible to the active internal signal layer. This is a complex and costly process involving setting individual drill depths on a per board basis. Special design features must be designed into the artwork to set correct backdrill depth. Furthermore, it is difficult to verify ALL backdrilled holes were drilled correctly. I know of a case where a backplane came back and one via (that they knew of) had a significantly longer stub than was specified. The problem showed up by accident when they were characterizing the channel using a VNA and saw an unexpected resonant null in the SDD21 insertion loss plot. When all was said and done, it turned out there was a glitch in the fabricator’s software controlling the backdrilling process. There is no practical way to find these faults; short of doing VNA measurements on 100% of the backdrilled holes. With hundreds of them in a typical highspeed backplane, the cost would be prohibitive. Thus we have to trust the fabrication process of the vendor(s).
If only there was a way to terminate the stub and get rid of all this backdrilling. Well there just might be a solution. After returning from last year’s DesignCon2010, I was intrigued by a paper presented by Dr. Nicholas Biunno on a new matched terminated stub technology developed by SanminaSCI Corporation. They call this technology MTSvia^{TM}^{ }and it allows the embedding of metal thinfilm or polymer thick film resistors within a PCB stackup during its fabrication. I like to call it “The Stubinator”. They developed this technology as an alternative to backdrilling. The beauty of this is you can terminate all the highspeed via stubs on just one resistive layer at the bottom of the PCB.
Of course, for this to work, we need to terminate the vias with a resistance equal to the differential via impedance to be most effective. But how do we determine the via differential impedance without going through a bunch of trial and error builds? In a DesignCon2009 paper titled, “Practical Analysis of Backplane Vias” I coauthored with Eric Bogatin from Bogatin Enterprises L.L.C., Sanjeev Gupta and Mike Resso from Agilent Technologies, we showed how you can model and simulate differential vias as simple twinrod transmission line structures using simple transmission line circuit models as shown in Figure 1. You can download a copy of this awardwinning paper from my web site at: Lamsimenterprises.com .
After determining fo (either by measurement of a real structure or through 3D modeling) and solving for Dkeff by rearranging equation (1), the differential via impedance calculated using the following equation:
(2)
Where:
s = the center to center spacing of the vias
D = Drill diameter.
Example:
The differential vias used in the model of Figure 1 has the following parameters:
s = 0.059 in.
D = 0.028 in.
stub_length = 0.269 in.
Dkeff = 6.14 by Equation (1) and fo=4.4GHz ;
Zdiff = 66 Ohms by Equation (2).
By adding a 66 Ohm resistor across the bottom of each via stub in the model, the blue trace in the plot shows the stub resonance has completely disappeared at the expense of an additional flat loss of about 10dB. The eye has opened up nicely.
This “Stubinator” technology looks like it could be a promising alternative to backdrilling. It resolves many of the issues and limitations highlighted above. Combined with silicon that can accommodate the additional signal loading, it may extend the life of traditional copper interconnections for next generation of Ethernet standards beyond 10GB/s.
Fiber Weave Effect Timing Skew
Fiber weave effect timing skew is becoming more of an issue as bit rates continue to soar upwards. For signaling rates of 5GB/s and beyond, it can actually ruin your day. For example, the figure on the left shows a 5GB/s received eye is totally closed due to 12.7 inches of fiber weave effect. It was modeled and simulated using Agilent ADS software.
So what is fiber weave effect anyways and why should we be concerned about it? Well, it’s the term commonly used when we want to describe the situation where a fiberglass reinforced dielectric substrate causes timing skew between two or more transmission lines of the same length. Since the dielectric material used in the PCB fabrication process is made up of fiberglass yarns woven into cloth and impregnated with epoxy resin, it becomes nonhomogeneous.
The speed at which a signal propagates along a transmission line depends on the surrounding material’s relative permittivity (e_{r}), or dielectric constant (Dk). The higher the Dk, the slower the signal propagates along the transmission line. When one trace happens to line up over a bundle of glass yarns for a portion of its length, as illustrated by the top trace in the figure on the left, the propagation delay is different compared to another trace of the same length which lines up over mostly resin. This is known as timing or phase skew and is due to the delta Dk surrounding the respective traces.
Fiber weave effect is a statistical problem. It is not uncommon for PCB designs to have long parallel lengths of track routing without any bends or jogs. This is particularly true in large passive backplane designs. Because the fiber weave pattern tends to run parallel to the xy axis, any traces running the same way will eventually encounter a situation of worst case timing skew if you build enough boards. This was demonstrated by Intel after compiling more than 58,000 TDR and TDT measurements over two years. In 2007, Jeff Loyer et al presented a DesignCon paper “Fiber Weave Effect: Practical Impact Analysis and Mitigation Strategies” where they published the data and proposed techniques to mitigate the effect of fiber weave skew. They showed statistically it is possible to have a worst case timing skew of approximately 16ps per inch representing a delta Dk of approximately 0.8.
In high speed differential signalling this is an issue because any timing skew between the positive (D+) and negative (D) data converts some of the differential signal into a common signal component. Ultimately this results in eye closure at the receiver and contributes to EMI radiation.
You can calculate the timing skew using the following equation:
Where:
t_{skew} = total timing skew due to fiber weave effect length (sec)
Dk_{max}= dielectric constant of material predominated by fiberglass.
Dk_{min}= dielectric constant of material predominated by resin.
c = speed of light = 2.998E+8 m/s (1.18E+10 in/s)
A practical methodology you can use to estimate the minimum and maximum values of Dk is by studying the material properties available from PCB laminate suppliers. Consider two extreme styles of fiberglass cloths used in modern PCB laminate construction as illustrated by the figure on the left. The loose weave pattern of 106 has the highest resin content of all the most popular weaves, while the tight weave pattern of 7628 has the lowest. Therefore, you could use the specified values of Dk for cloth styles 106 and 7628 to get Dk_{min} and Dk_{max }respectively. Once you have these and apply a tolerance, you can estimate the t_{skew }.
Example:
Assume Fr4 material; one inch of fiber weave effect; Dk_{106}= 3.34(+/0.05) and Dk_{7628}= 3.97(+/0.05), then timing skew is calculated as follows:
Modern serial link interfaces use differential signalling on a pair of transmission lines of equal length for interconnect between two points. In a DesignCon 2007 paper, “Losses Induced by Asymmetry in Differential Transmission Lines” by Gustavo Blando et al, they showed how intrapair timing skew between the positive (D+) and negative (D) data caused an increase in the differential insertion loss profile due to timing induced resonances. These resonances appear as dips in the differential insertion loss profiles of the channel as shown in the following figure:
This figure presents the results from an ADS simulation I did recently of a PCIe Gen2 channel running at 5GT/s. The eye diagrams are at the receiver after approximately 30” of track length chip to chip. The channel model was parameterized to allow for adjusting the fiber weave effect length as required.
As you can see, when the length of the fiber weave effect induced skew increases from 0 to 12.7 inches, the fundamental frequency nulls in the differential insertion loss plots decrease. These nulls occur at the fundamental frequency (fo) and every odd harmonic.
Also, the eye shows some degradation at 5.6 inches of fiber weave effect and starts to distort significantly after 7.8 inches. At 12.7 inches, fo equals the Nyquist frequency of the data rate (in this case 2.5GHz) and the eye is totally closed.
You can predict the resonant frequency ahead of time and use it to gain some intuition before you simulate and validate the results. If you know the total intrapair timing skew, fo is calculated using the following equation:
Where:
f_{o }= resonant frequency
t_{skew} = total intrapair timing skew
Example:
Using t_{skew} = 16 ps/in we calculated above and using 12.7 inches from the last simulation results in the figure above, the fundamental resonant frequency null is:
You can find more details of this phenomena plus a novel way to model and simulate it from a recent White Paper I published titled, “Practical Fiber Weave Effect Modeling”. It, along with other papers, is found on my website at LamsimEnterprises.com.
PCB Laminate Construction
Present day FR4style laminates used for PCB fabrication rely on woven glass fiber yarns to maintain the structural integrity of the finished product. These yarns are made up of electronic or EGlass material. Because it is the same glass used in everything from Corvette bodies to boat hulls, it is a very inexpensive reinforcement material. NEGlass has improved electrical and mechanical performance over EGlass. It is used for higher performance laminate products such as Park Nelco 400013SI.
The table on the left shows five of the most common fiberglass styles used for laminate construction today. When glass fiber yarns are woven into fabric, the “Warp” yarns run the length of the roll, while the “Fill or Weft” yarns run the width. Yarn count refers to the number of warp threads per inch by the number of fill threads per inch.
Prepreg is the term we commonly use for a weave of glass fiber yarns preimpregnated with resin which is only partially cured. The glass to resin thickness ratio defines the overall thickness of a prepreg mat. You can see from the table above, the typical resin content is a function of the thread count and yarn diameter. For example, the figure on the far left illustrates styles like 106 and 1080 having smaller diameter yarns and higher resin content. The right hand figure is indicative of yarns with larger diameter and lower resin content like style like 2116 or 7628.
When copper foil is attached to one or both sides of fully cured prepreg mats, the finished laminated panel is called a core. Both cores and prepreg mats are available in various panel sizes and thicknesses.
There are several different kinds of resin systems in use today to form prepreg and cores. The general specification FR4 is the most common. It refers to a specific fireretardant level rather than specific resin chemistry. Since you have a choice of many laminates that meets the FR4 fire specification, there is no such thing as “standard FR4”. That being said, most of us consider “standard FR4” to mean a laminate having a typical dielectric constant (Dk) of about 4.3 and dissipation factor (Df) of 0.020 – 0.025 at 1MHZ and 50% resin content.
Each family of resin systems have their unique electrical and mechanical characteristics depending on the fiberglass style and resin chemistry. For example, Nelco 40006 at 50% resin content has a typical Dk of 4.0 and Df of 0.023 at 2.5GHz. A higher performance resin system like Nelco N400013 on the other hand, has a Dk of 3.7 and Df of 0.009 for the same resin content and frequency. This tells us two things:

A lower Dk means we can ultimately achieve an overall thinner board for the same characteristic impedance.

A lower DF means less high frequency attenuation allowing us to run at a higher bit rate or have longer traces.
When designing your board stackup, it is best to refer the manufactures data sheet for exact values. The Park Electrochemical Corp. (Nelco) website is an excellent resource to explore when trying to decide on the best dielectric material to use for your next highspeed design.