Archive for the ‘Modeling’ Category
Differential Impedance and Why We Care
Originally published in Signal Integrity Journal April 14,2020
What is Differential Impedance and Why do We Care?
Simply put, differential impedance is the instantaneous impedance of a pair of transmission lines when two complimentary signals are transmitted with opposite polarity. For a printed circuit board (PCB) this is a pair of traces, also known as a differential pair. We care about maintaining the same differential impedance for the same reason we care about maintaining the same instantaneous impedance of a singleended (SE) transmission line: to avoid reflections.
There is really nothing special about differential pairs, other than maintaining the correct differential impedance. But you must understand the implications of the spacing between the traces in a pair.
The differential impedance is simply twice the oddmode impedance of each trace. SE impedance is the impedance of a single trace and only equals the oddmode impedance when there is little or no intrapair coupling between them. When the traces are brought closer together, the differential impedance is reduced, unless the line widths are adjusted to compensate. (More about this later.)
Figure 1 shows the effect on intrapair coupling of a pair of edgecoupled stripline traces driven differentially. The top figure shows electromagnetic fields surrounding a loosely coupled pair of traces 3.5 linewidths apart. The bottom figure shows a closely coupled pair at 1.5 linewidths apart. The red plus trace is current flowing into the page while the minus blue trace is current flowing out of the page.
The circular lines surrounding each trace are the magnetic fields representing loop inductance. The direction of rotation is based on current direction, using the righthand rule. The electric field (efield) lines are perpendicular to the magnetic field lines. They are a measure of capacitance.
Figure 1. Effect on intrapair coupling of a pair of edgecoupled stripline traces driven differentially. Top figure shows electromagnetic fields surrounding a loosely coupled pair of traces 3.5 linewidths apart. Bottom figure shows a closely coupled pair at 1.5 linewidths apart.
When the traces are loosely coupled, the electric and magnetic field lines are fairly symmetrical around each trace, and are mirror images of one another about the center line between them. Most of the respective efield coupling is to the reference ground planes. As the traces are moved closer to one another, the counterrotating rings compress about the centerline, lowering the inductance. At the same time, more of the efield lines along the inside edge of each trace tend to couple to one another, increasing the capacitance.
Because of the way the EMfields interact along the centerline, we can think of it as a virtual ground (VGND) reference plane. They behave exactly the same way as if there is a solid reference plane between them.
OddMode Impedance
Consider a pair of equal width microstrip line traces, labeled 1 and 2, with a constant spacing between them as shown in Figure 2. Assuming lossless transmission lines, each individual trace, when driven in isolation, will have a SE characteristic impedance Zo, defined by the selfloop inductance (L11, L22) and selfcapacitance (C11, C22) with respect to the GND reference plane.
When the pair of traces are driven differentially, the mode of propagation is odd. The electromagnetic field interaction is shown in Figure 1. When the intrapair spacing is close, there will be electromagnetic coupling defined by the mutual inductance (Lm) and mutual capacitance (Cm).
The proximity of the traces to a reference plane influences the amount of electromagnetic coupling between traces. The closer the traces are to the reference plane, the lower the selfloop inductance and stronger selfcapacitance; resulting in a lower mutual inductance, and weaker mutual capacitance between traces. The end result is a lower differential impedance.
Figure 2. Pair of microstrip traces showing selfloop inductance (L11, L22), selfcapacitance (C11, C22), mutual capacitance (Cm) and mutual inductance (Lm) when line 1 and line 2 are driven differentially.
A 2D field solver is usually used to extract the parameters for a given geometry. Once the resistance, inductance, conductance, and capacitance (RLGC) parameters are extracted, an L C matrix can be set up as follows:
L11 L12 C11 C12
L21 L22 C21 C22
The selfloop inductance and selfcapacitance for trace 1 and 2 are L11, C11, L22, C22 respectively. In a perfectly symmetrical differential pair, the offdiagonal (12, 21) terms in each matrix are the mutual inductance and mutual capacitance respectively. The LC matrix can be used to determine the oddmode impedance. It can be calculated by the following equation [1]:
Equation 1
Where:
Zodd = odd mode impedance
Ls = selfloop inductance = L11 = L22
Cs = selfcapacitance = C11 = C22
Lm = mutual inductance = L12 = L21
Cm = mutual capacitance = C12 =C21
Example
A Polar SI9000 field solver is used to compare a loosely coupled pair, with 4 mil traces, separated by 20 mil space, vs. a SE transmission line with the same dielectric thickness (see Figure 3). The LC matrix was extracted at 10GHz. As can be seen, the oddmode impedance of the loosely coupled pair equals the characteristic impedance of the SE trace, and thus differential impedance would be the same.
Figure 3. Comparison of a loosely coupled pair (left), with 4 mil traces, separated by 20 mil space, vs. a SE transmission line (right) with the same dielectric thickness. Oddmode impedance of the loosely coupled pair equals the characteristic impedance of the SE trace.
But if you route a pair of traces with close coupling, the oddmode impedance is less than the SE impedance for the same trace width (unless you adjust the line width). For example, on the left side of Figure 4, a 444 mil geometry has a differential impedance of 91 Ohms. In order to get 100 Ohms differential, the line width must be reduced to 3.35 mils and space adjusted to 4.65 mils to keep the same 12 mil centercenter pitch, shown on right.
Figure 4. Comparison of 444 mil geometry (left) vs. 3.354.653.35 geometry (right) to achieve 100 Ohm differential impedance for the same centercenter pitch.
But it doesn’t end there.
For some industry standards, there is usually a very short reach (VSR) spec which has a maximum channel loss defined. For example, the IEEE 802.3 CAUI4 chipmodule (C2M) spec budgets 7.5 dB at 12.89 GHz Nyquist frequency from the chip’s pins to a faceplate module’s pins, e.g. small formfactor pluggable (SFP) module. Because of modern topofrack routers and switches, it is not unusual to have 10 or more inches between the main switch chip and SFP module, the differential pair geometry design becomes important to satisfy both differential impedance and insertion loss (IL).
Reduced line width and tighter coupling results in higher loss over the length of the channel. Using the above examples, differential IL is plotted in Figure 5 for all three differential pairs. Loose coupling is shown in green; tight coupling without line width adjustment (Tight1) is shown in red, while tight coupling with line width adjustment (Tight2) is shown in blue.
As you can see, there is about a half dB difference at 12.89 GHz between loose coupling and both tight coupling examples over 10.6 inches. Tight coupling lowers IL, regardless if line width is adjusted to meet differential impedance. In this example, there is only 0.1 dB delta between Tight1 and Tight2, which suggests most of the higher loss is due to tighter coupling.
Figure 5. Differential IL comparison of loose coupling (green); Tight1 coupling without line width adjustments (red) and Tight2 coupling with line width adjustment (blue).
This can be explained by reviewing SE to differential mixedmode conversion. Given a 4port Sparameter, with SE port order as shown in Figure 6, the differential IL is determined by;
Equation 2
Where:
SDD21 = the differential IL defined by the ratio of the differential signaling coming out of port 2 to the differential signal going into port 1
S21 = the SE IL defined by the ratio of the SE signaling coming out of port 2 to the SE signal going into port 1
S43 = the SE IL defined by the ratio of the SE signaling coming out of port 4 to the SE signal going into port 3
S23 = farend crosstalk coupling from port 3 to port 2
S43 = farend crosstalk coupling from port 4 to port 3
As you can see from Equation 2, when the traces get closer together, and the coupling terms get larger, differential IL increases.
Figure 6. SE 4port Sparameter port labeling.
Figure 7 plots differential TDR of all three examples. The steeper monotonic rise of the blue trace is due to higher resistive loss of 3.35 mil traces, as compared to the 4 mil traces in the other two examples.
Figure 7. Differential TDR comparison of loose coupling (green); Tight1 coupling without line width adjustments (red) and Tight2 coupling with line width adjustment (blue).
To summarize then, it doesn’t matter if a differential pair is tightly coupled or loosely coupled. Properly engineered, both can be designed to properly match the output driver impedance. But as we have seen, each will have advantages and disadvantages.
Tighter coupling gives you better routing density at the expense of higher loss. Loose coupling allows for easier routing around obstacles and less loss. But in either case, they must be designed and measured for differential impedance.
So why is this important?
PCB fabrication shops use impedance as a metric to determine if the board has been fabricated to specification. Because the oddmode impedance of a tightly spaced pair of traces depends on driving both traces differentially, you will not be able to determine the differential impedance by just measuring SE impedance of a tightly coupled pair like you could with two uncoupled traces.
References:

E. Bogatin, “Signal Integrity Simplified”, 3rd edition, Prentice Hall PTR, 2018

Keysight Advanced Design System (ADS) [computer software], (Version 2020)

Polar Instruments Si9000e [computer software] Version 2017
CannonballHuray Model Demystified
Recently on the SIList there was great debate on whether or not my Cannonball model can be used to determine surface ratio and radius of sphere parameters needed for Huray roughness model from data sheets alone.
The author of this paper, “Conductor surface roughness modeling: From “snowballs” to “cannonballs”, [1] argues it is impossible to accurately model transmission lines from data sheets alone and seems to imply that because I had measured data in advance that I had magically “adjusted” R_{z} parameter to get such good correlation to measurements in my EDICon 2016 paper, “Practical Model of Conductor Surface Roughness Using Cubic Closepacking of Equal Spheres” [5].
Unfortunately his paper has created more confusion than clarity. To be clear, there is only ONE “Cannonball” model, and it is based on the cubic close packing of equal spheres, also known as facecentered cubic (FCC) packing.
The author of [1] also advocates using a material model identification methodology, similar to what I like to call the Design Feedback Method, shown in Figure 1. The author believes it is the only “accurate” way of determining printed circuit board (PCB) material properties for modeling.
Figure 1 Design Feed Back Method flow chart
This involves designing, building and measuring a test coupon with the intended PCB trace geometry to be used in final design. After modeling and tuning various parameters to best fit measured data, material parameters are extracted and then used in channel modeling software to design the final product.
The problem with this approach for many small companies is: TIME, RESOURCES, and MONEY.

Time to define stackup and test structures.

Time to actually design a test coupon.

Time to procure raw material – can take weeks, depending on scarcity of core/prepreg material.

Time to fabricate the bare PCB.

Time to assemble and measure.

Time to crosssection and measure parameters.

Time to model and fit parameters to measurements.
Then there is the issue of resources, which include having the right test equipment and trained personnel to get trusted measurements.
In the end this process ultimately costs more money, and material properties are only accurate for the sample from which they were extracted for the software and roughness model used. There is no guarantee extracted parameters reflect the true material properties.
There will be variation from sample to sample built from the same fab shop and more so from different fab shops because they have a different etch line and oxide alternative process.
For example Figure 2 shows measurements from two boards of the same design. As you can see there are differences in both insertion loss and TDR plots. Which curve do we use to fit parameters for material extraction to use in simulations? How many do we have to build and test to get a statistical sample of reality? How much time will this take? And how much money will it cost, especially if several PCB stackup geometries are required?
Figure 2 Comparison of insertion loss and TDR measurements of two boards of the same design
But, as Eric Bogatin often likes to say, “Sometimes an OK answer NOW is better than a good answer late”. For many signal integrity engineers, and design consultants, like myself, have to come up with an answer sooner, rather than later for many reasons. And depending on the issue at hand, those answers may be good enough. This was the initial motivation for my research.
So where do we get these parameters? Often the only sources are from manufacturers’ data sheets alone. But in most cases, the numbers do not translate directly into parameters needed for the EDA tools.
This paper will revisit the Cannonball model as it applies to the CMP28 reference platform from Wildriver Technology [14], and as part of it I will show:

How to determine effective dielectric constant (D_{keff}) due to roughness from data sheets alone.

How to apply my simple Cannonball stack model to determine roughness parameters needed for Huray model from data sheets alone.

How to apply these parameters using Simbeor software [10].

How to pull it all together with a simple case study.
But before we get into it, it is important to give a bit of background on material properties and PCB fabrication process.
Electrodeposited Copper
Electrodeposited (ED) copper is widely used in the PCB industry due to its low cost. A finished sheet of ED foil has a matte side and drum side. The matte side is usually treated with tiny nodules and is the side bonded to the core laminate. The drum side is always smoother than the matte side. For high frequency boards, sometimes the drum side of the foil is treated instead and bonded to the core. In this case it is known as reversed treated foil (RTF).
IPCTM6502.2.17A defines the procedure for determining the roughness or profile of metallic foils used on PCBs. Profilometers are often used to quantify the roughness tooth profile of electrodeposited copper.
Nodule treated tooth profiles are typically reported in terms of 10point mean roughness (R_{z}). Some manufacturers may also report root mean square (RMS) roughness (R_{q}). For standard foil this is the matte side. For RTF it is the drum side. Most often the untreated, or prepreg side, reports average roughness (R_{a}) in manufacturers’ data sheets.
With the realization of roughness having a detrimental effect on insertion loss (IL), copper suppliers began providing very low profile (VLP) and ultralow profile (ULP) class of foils. VLP foils have treated roughness profiles less than 4 μm while ULP foils are less than 2 μm. Other names for ULP class are HVLP or eVLP, depending on the foil manufacturer.
It is important to obtain the actual vendor’s copper foil data sheet used by the respective laminate supplier for accurate modeling.
Oxide/Oxide Alternative Treatment
In order to promote good adhesion of copper to the prepreg material during the PCB lamination process, the copper surface is treated with chemicals to form a thin, nonconductive film of black or brown oxide. The controlled oxidation process increases the surface area, which provides a better bond between the prepreg and the copper surface. It also passivates the copper surface to protect it from contamination.
Although oxide treatment has been used for many years, eventually the industry learned that the lack of chemical resistance resulted in pink ring, which is indicative of poor adhesion between copper and prepreg. This weakness has led to oxide alternative (OA) treatments which rely on some sort of etching process, but no oxide layer is formed.
With the push for smoother copper to reduce conductor loss, newer chemical bond enhancement treatments, working at the molecular level, were developed to maintain copper smoothness, yet still provide good bonding to the prepreg.
Since OA treatment is applied to the drum side of the foil during the PCB Fabrication process, the OA roughness numbers should be used instead of R_{a} specified in foil manufacturer’s data sheets. RTF foil is modeled differently and discussed later in the case study.
Tale of Two Data Sheets
Everyone involved in the design and manufacture of PCBs knows the most important properties of the dielectric material are the dielectric constant (D_{k}) and dissipation factor (D_{f }).
Using D_{k} / D_{f }numbers for stackup design and channel modeling from “Marketing” data sheets, like the example shown in Figure 3, will give inaccurate results. These data sheets are easily obtained when searching laminate supplier’s web sites.
Figure 3 Example of a “Marketing” data sheet easily obtained from laminate supplier’s web site. Source Isola Group.
Instead, real or “Engineering” data sheets, which are used by PCB fabricators to design stackups, should be used for PCB interconnect modeling. These data sheets define the actual thickness, resin content and glass style for different cores and prepregs. They include D_{k }/ D_{f }over a wide frequency range; usually from 100 MHz10GHz.
Figure 4 Example of an “Engineering” data sheet showing D_{k}/D_{f} for different glass styles and resin content over frequency. Source Isola Group.
Effective D_{k} Due to Roughness
Many engineers assume D_{k }published 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 simulations are compared against measurements, there is often a discrepancy in D_{keff}, due to increased phase delay caused by surface roughness.
D_{keff} is highly dependent on the test apparatus and conditions of how it is measured. One method commonly used by many laminate suppliers is the clamped stripline resonator test method, as described by IPCTM650, 2.5.5.5, Rev C, Test Methods Manual.
The measurements are done under stripline conditions using a carefully designed resonant element pattern card made with the same dielectric material to be tested. As shown in Figure 5, the card is sandwiched between two sheets of unclad dielectric material under test. Then the whole structure is clamped between two large plates; each lined with copper foil and are grounded. They act as reference planes for the stripline.
Figure 5 Illustration of clamped stripline resonator test method, as described by IPCTM650, 2.5.5.5, Rev C, Test Methods Manual
This method assures consistency of product when used in fabricated boards. It does not guarantee the values directly correspond to design applications.
This is a key point to keep in mind, and here is why.
Since the resonant element pattern card and material under test are not physically bonded together, there are small air gaps between the various layers that affect measured results. The small air gaps result in a lower D_{keff} than what is measured in real applications using foil with different roughness bonded to the same core laminate. This is the primary reason for phase delay discrepancy between simulation and measurements.
If D_{k} 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 be estimated by [2]:
Equation 1
where: H_{smooth} is the thickness of dielectric from data sheet; R_{z} is 10point mean roughness from data sheet; D_{k} is dielectric constant from data sheet
Most EDA tools include a wideband causal dielectric model. To use it, you must enter D_{k }and D_{f} at a particular frequency. I found it is usually best to use the values near the Nyquist frequency of the baud rate.
Modeling Copper Roughness
“All models are wrong but some are useful”– a famous quote by George E. P. Box, who was a British statistician in the mid20^{th} century. The same can be said when using various roughness models.
For example many roughness models require RMS roughness numbers, but often R_{z} is the only number available in data sheets, and vice versa. If R_{z} is defined as the sum of the average of the five highest peaks and the five lowest valleys of the roughness profile over a sample length, and R_{q} is the RMS value of that profile, then the roughness can be modeled as a triangular profile with a peak to valley height equal to R_{z}, as illustrated in Figure 6.
Figure 6 Triangular roughness profile model with peak to valley height equal to 10point mean roughness R_{z}.
If we define the RMS height of the triangular roughness profile is equal to ∆, then:
Equation 2
And likewise, if we assume ∆ ~ R_{q}, then:
Equation 3
Several modeling methods were developed over the years to determine a roughness correction factor (K_{SR}). When multiplicatively applied to the smooth conductor attenuation (α_{smooth}), the attenuation due to roughness (α_{rough}) can be determined by:
Equation 4
Huray Model
In recent years, the Huray model has found its way into popular EDA software due to the continually increasing need for better modeling accuracy. The model is based on a nonuniform distribution of spherical shapes resembling “snowballs” and stacked together forming a pyramidal geometry.
By applying electromagnetic wave analysis, the superposition of the sphere losses can be used to determine 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 (K_{SRH}) can be analytically solved by [4]:
Equation 5
Although it has been proven to be a pretty accurate model, it relied on analysis of scanning electron microscopy (SEM) pictures of the treated surface and tuning of parameters for best fit to measured data. This is not a practical solution if all you have is roughness parameters from manufacturers’ data sheets.
CannonballHuray Model
Building upon the work already done by Huray, and using the Cannonball stack principle, the sphere radius and flat base area parameters are easily estimated solely from roughness parameters published in manufacturers’ data sheets.
As illustrated in Figure 7 there are three rows of equal sized 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. This stacking arrangement is known as closepacking of equal spheres, but more commonly known as the “Cannonball” stack due to the method used by sailors to stack actual cannonballs aboard ships.
Figure 7 CannonballHuray physical model. The height of the stack is the RMS height of the peak to valley profile equal to R_{z} from data sheets.
If we could peer into the stack and imagine a pyramid lattice structure connecting to the center of all the spheres, then the total height is equal the height of two pyramids plus the diameter of one sphere.
Given the height of the Cannonball stack (∆) is equal to the RMS value of the peak to valley roughness profile; then from method described in my earlier papers, determining the sphere radius (r ), from R_{z} found in data sheets, can be further simplified and approximated as [13]:
and base area (A_{flat}) as:
Equation 7
Because the model assumes the ratio of A_{matte}/A_{flat} = 1, and there are only 14 spheres, the original CannonballHuray model can be further simplified to:
Equation 8
where: K_{CH} (f) = CannonballHuray roughness correction factor, as a function of frequency; δ (f) = skindepth, as a function of frequency in meters; r = the radius of spheres in meters (Equation 6)
CMP28 Case Study Revisited
To test the accuracy of the model, stackup details and measured data from a CMP28 test platform, design kit, courtesy of Wildriver Technology, shown in Figure 8, was used for model validation. The PCB stackup is shown in Figure 9
Two different sets of Sparameter (s2p) files from a 2 inch and 8 inch singleended (SE) stripline traces shown were used in this study. The original set of measurements, from my previous papers, and a second set provided as part of CMP28 design kit from another PCB were used for model correlation.
The 6 inch transmission line segment Sparameter data was deembedded using Ataitec ISD software [8] for both sets of data.
Figure 8 Photo of a portion of CMP28 test platform courtesy of Wildriver Technology used for model validation.
Figure 9 CMP28 PCB Stackup
The PCB was fabricated with Isola FR408HR 3313 core and prepreg, with 1 oz. RTF. D_{k} and D_{f} at 10GHz were obtained from the FR408HR data sheet found on their web site and shown in Figure 10 & Figure 11.
Figure 10 Isola FR408HR data sheet used for core dielectric properties.
Figure 11 Isola FR408HR data sheet used for prepreg dielectric properties.
The foil used on FR408HR core laminates is MLS, Grade 3, controlled elongation RTF from Oakmatsui. Roughness Rz parameters for drum and matte sides are 120μin (3.048 μm) and 225μin (5.715μm) respectively for 1 oz. copper foil.
Figure 12 MLS RTF foil data sheet used on FR408HR laminate.
An oxide or oxide alternative (OA) treatment is usually applied to the copper surfaces prior to final PCB lamination. When it is applied to the matte side of RTF, it tends to smoothen the macroroughness slightly. At the same time, it creates a surface full of microvoids which follows the underlying rough profile and allows the resin to fill in the cavities, providing a good anchor.
MultiBond MP from Macdermid Enthone is an example of an oxide alternative microetch treatment commonly used in the industry. Typically 50 μin (1.27μm) of copper is removed when the treatment is completed, depending on the board shop’s process control, as per Figure 13.
In a subsequent paper by J.A. Marshall, presented at IPC APEX 2015 titled, “Measuring Copper Surface Roughness for High Speed Applications” [11], there is data supporting the hypothesis that RTF roughness gets smoother after OA application.
Figure 13 Macdermid Enthone MultiBond MP data sheet reference from their web site.
Table 1 summarizes the PCB design parameters, dielectric material properties and copper roughness parameters obtained from respective manufactures’ data sheets.
Table 1 CMP28 Test Board and Data Sheet Parameters
Parameter  FR408HR/RTF 
Dk Core/Prepreg  3.65/3.59 @10GHz 
Df Core/Prepreg  0.0094/0.0095 @ 10GHz 
R_{z} Drum side  3.048 μm 
R_{z} Matte side before Microetch  5.715 μm 
R_{z }Matte side after Microetch  4.445 μm 
Trace Thickness, t  1.25 mil (31.7μm ) 
Trace Etch Factor  60 deg 
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) 
From Table 1 and by applying Equation 1, D_{keff} of core and prepreg due to roughness were determined to be:
Next, the Cannonball model’s sphere radiuses, for matte and drum side of the foil, were determined to be:
Because most EDA tools only allow a single value for the radius parameter, the average radius (r_{avg}) was determined to be:
Equation 9
Simbeor electromagnetic software from Simberian Inc. [10] was used for modeling the transmission lines. It includes the latest and greatest dielectric and conductor roughness models, including the HurayBracken causal metal model.
Solution explorer pane and solution tree, as shown in Figure 14, allows you to edit and view solution data as a tree structure. All parameters from Table 1 were entered here.
Simbeor requires two parameters; roughness factor (RF1) and sphere radius (SR1). Because the Cannonball model always has N=14 spheres and base area (A_{flat}) is always 36r^{2}, r^{2} cancels out and RF1 can be simplified to:
Equation 10
Sphere radius (SR1) is r_{avg} = 0.225 as calculated from Equation 9.
Figure 14 Simbeor Solution Explorer Pane and Solution Tree
The wideband causal dielectric model option was used to model dielectric properties over frequency. Effective D_{k} due to roughness for core and prepreg, calculated above, were substituted instead of data sheet values. Standard copper resistivity of 1.724e8 ohmmeter was used.
After the transmission lines were modeled and simulated, the Sparameter results were saved in touchstone format. Keysight ADS [5] was used for further simulation analysis and comparison.
D_{keff} can be derived from phase delay. This is also known as time delay (TD) and is often used as a metric for simulation correlation accuracy for phase. TD, as a function of frequency, in seconds, is calculated from the unwrapped measured transmission phase angle, and is given by:
Equation 11
and:
D_{keff }, as a function of frequency, is then given by:
Equation 12
where:c = speed of light (m/s); Length = length of conductor (m)
Figure 15 compares the simulated results vs measurement of a 6inch, deembedded stripline trace. The red plots are measured from CMP28 design kit data. The data was bandwidth limited to 35 GHz. The blue plots are the original measured data used in my previous paper [5]. The green plots are modeled with data sheet values only with oxide alternative treatment applied. SE IL is shown on the left and D_{keff} is shown on the right. As can be seen, there is excellent correlation.
Figure 15 Measured vs simulated insertion loss (left) and D_{keff }(right) with OA etch treatment applied.
The author of [1] suggests is that because I had the measured data, R_{z} was “adjusted” to show excellent results. What he is implying is my “adjusting” the roughness, due to the oxide treatment, was the reason for such good results, in spite of the fact Macdermid’s OA data sheet reports typical 50 μin of copper removal after treatment and data from [11] showing RTF gets slightly smoother after OA treatment.
So ok, let’s see what happens if I didn’t adjust the roughness due to OA treatment. Instead of using R_{z }matte side after microetch (4.445 μm ) roughness, we will use 5.715 μm from data sheet.
This will affect D_{keff }of prepreg and average sphere radius r_{avg}_{ , }so we will recalculate them:
And average radius is:
Figure 16 compares the simulated results vs measurement. The red plots are measured from CMP28 design kit data. The blue plots are the original measured data used in my previous paper [5]. The green plots are modeled with data sheet values only without oxide alternative treatment applied. SE IL is shown on the left and D_{keff} is shown on the right.
As can be seen, there is still excellent correlation with insertion loss even though OA was not considered. As expected using the rougher number would increase effective Dk. But in the end the TDR plots in Figure 17shows impedance change is negligible.
Figure 16 Measured vs simulated insertion loss (left) and phase delay (right) without OA etch treatment applied.
Figure 17 Measured vs simulated TDR plots with OA etch treatment (left) and without (right).
Summary and Conclusions
By using CannonballHuray model, with copper foil roughness and dielectric material properties obtained solely from respective manufacturers’ data sheets, practical PCB interconnect modeling for highspeed design is now achievable using commercial fieldsolving software employing Huray model.
Measured results from two different boards confirmed there are variations due to manufacturing that would affect material model extraction method accuracy.
When oxide alternative treatment was not considered, even though the matte side roughness of RTF gets smoothened during the PCB fabrication process, the simulated results still show excellent correlation to the original measured data from previous paper [5].
References
[1] Y. Slepnev, “Conductor surface roughness modeling: From “snowballs” to “cannonballs”.
[2] B. Simonovich, “A Practical Method to Model Effective Permittivity and Phase Delay Due to Conductor Surface Roughness”. DesignCon 2017, Proceedings, Santa Clara, CA, 2017
[3] L. Simonovich, “Practical method for modeling conductor roughness using cubic closepacking of equal spheres,” 2016 IEEE International Symposium on Electromagnetic Compatibility (EMC), Ottawa, ON, 2016, pp. 917920. doi: 10.1109/ISEMC.2016.7571773.
[4] Huray, P. G. (2009) “The Foundations of Signal Integrity”, John Wiley & Sons, Inc., Hoboken, NJ, USA., 2009
[5] L.Simonovich, “Practical Model of Conductor Surface Roughness Using Cubic Closepacking of Equal Spheres”, EDICon 2016, Boston, MA
[6] Keysight Advanced Design System (ADS) [computer software], (Version 2017). URL: http://www.keysight.com/en/pc1297113/advanceddesignsystemads?cc=US&lc=eng.
[7] Isola Group S.a.r.l., 3100 West Ray Road, Suite 301, Chandler, AZ 85226. URL: http://www.isolagroup.com/
[8] Ataitec, URL: http://ataitec.com/products/isd/
[9] V. DmitrievZdorov, B. Simonovich, I. Kochikov, “A Causal Conductor Roughness Model and its Effect on Transmission Line Characteristics”, DesignCon 2018 Proceedings, Santa Clara, CA, 2018
[10] Simberian Inc., 2629 Townsgate Rd., Suite 235, Westlake Village, CA 91361, USA, URL: http://www.simberian.com/
[11] John A. Marshall, “Measuring Copper Surface Roughness for High Speed Applications”, IPC APEX Expo 2015.
[12] Macdermid Enthone, Multibond MP, Inner Layer Oxide Alternative Bonding. URL: https://electronics.macdermidenthone.com/productsandapplications/printedcircuitboard/surfacetreatments/innerlayerbonding
[13] B. Simonovich, “PCB Interconnect Modeling Demystified”. DesignCon 2019, Proceedings, Santa Clara, CA, 2019.
[14] Wild River Technology LLC 8311 SW Charlotte Drive Beaverton, OR 97007. URL: https://wildrivertech.com/
Perils of Crossing Split Planes
I 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 Sparameter 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.
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; nearend/farend 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.
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 highspeed 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.
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.
Practical Conductor Roughness Modeling with Cannonballs
In the GB/s regime, accurate modeling of conductor losses is a precursor to successful highspeed serial link designs. Failure to model roughness effects can ruin you day. For example, Figure 1 shows the simulated total loss of a 40 inch printed circuit board (PCB) trace without roughness compared to measured data. Total loss is the sum of dielectric and conductor losses. With just 3dB delta in insertion loss between simulated and measured data at 12.5 GHz, there is half the eye height opening with rough copper at 25GB/s.
So what do cannon balls have to do with modeling copper roughness anyway? Well, other than sharing the principle of close packing of equal spheres, and having a cool name, not very much.
According to Wikipedia, closepacking of equal spheres is defined as “a dense arrangement of congruent spheres in an infinite, regular arrangement (or lattice)” [8]. The cubic closepacked and hexagonal closepacked are examples of two regular lattices. The cannonball stack is an example of a cubic closepacking of equal spheres, and is the basis of modeling the surface roughness of a conductor in this design note.
Figure 1 Comparisons of measured insertion loss of a 40 inch trace vs simulation. Eye diagrams show that with 3dB delta in insertion loss at 12.5GHz there is half the eye opening at 25GB/s. Modeled and simulated with Keysight EEsof EDA ADS software [14].
Background
In printed circuit (PCB) construction there is no such thing as a perfectly smooth conductor surface. There is always some degree of roughness that promotes adhesion to the dielectric material. Unfortunately this roughness also contributes to additional conductor loss.
Electrodeposited (ED) copper is widely used in the PCB industry. A finished sheet of ED copper foil has a matte side and drum side. The drum side is always smoother than the matte side.
The matte side is usually attached to the core laminate. For high frequency boards, sometimes the drum side of the foil is laminated to the core. In this case it is referred to as reversed treated (RT) foil.
Various foil manufacturers offer ED copper foils with varying degrees of roughness. Each supplier tends to market their product with their own brand name. Presently, there seems to be three distinct classes of copper foil roughness:
· Standard
· Verylow profile (VLP)
· Ultralow profile (ULP) or profile free (PF)
Some other common names referring to ULP class are HVLP or eVLP.
Profilometers are often used to quantify the roughness tooth profile of electrodeposited copper. Tooth profiles are typically reported in terms of 10point mean roughness (R_{z }) for both sides, but sometimes the drum side reports average roughness (R_{a }) in manufacturers’ data sheets. Some manufacturers also report RMS roughness (R_{q }).
Modeling Roughness
Several modeling methods were developed over the years to determine a roughness correction factor (K_{SR }). When multiplicatively applied to the smooth conductor attenuation (α_{smooth }), the attenuation due to roughness (α_{rough }) can be determined by:
Equation 1
The most popular method, for years, has been the Hammerstad and Jensen (H&J) model, based on work done in 1949 by S. P. Morgan. The H&J roughness correction factor (K_{HJ }), at a particular frequency, is solely based on a mathematical fit to S. P. Morgan’s power loss data and is determined by [2]:
Equation 2
Where:
K_{HJ} = H&J roughness correction factor;
∆ = RMS tooth height in meters;
δ = skin depth in meters.
Alternating current (AC) causes conductor loss to increase in proportion to the square root of frequency. This is due to the redistribution of current towards the outer edges caused by skineffect. The resulting skindepth (δ ) is the effective thickness where the current flows around the perimeter and is a function of frequency.
Skindepth at a particular frequency is determined by:
Equation 3
Where:
δ = skindepth in meters;
f = sinewave frequency in Hz;
μ_{0}= permeability of free space =1.256E6 Wb/Am;
σ = conductivity in S/m. For annealed copper σ = 5.80E7 S/m.
The model has correlated well for microstrip geometries up to about 15 GHz, for surface roughness of less than 2 RMS. However, it proved less accurate for frequencies above about 5GHz for very rough copper [3] .
In recent years, the Huray model [4] has gained popularity due to the continually increasing data rate’s need for better modeling accuracy. It takes a real world physics approach to explain losses due to surface roughness. The model is based on a nonuniform distribution of spherical shapes resembling “snowballs” and stacked together forming a pyramidal geometry, as shown by the scanning electron microscope (SEM) photo in Figure 2.
Figure 2 SEM photograph of electrodeposited copper nodules on a matte surface resembling “snowballs” on top of heat treated base foil. Photo credit OakMitsui.
By applying electromagnetic wave analysis, the superposition of the sphere losses can be used to calculate the total loss of the structure. Since the losses are proportional to the surface area of the roughness profile, an accurate estimation of a roughness correction factor (KSRH) can be analytically solved by [1]:
Equation 4
Where:
K_{SRH} (f ) = roughness correction factor, as a function of frequency, due to surface roughness based on the Huray model;
A_{flat}= relative area of the matte base compared to a flat surface;
a_{i} = radius of the copper sphere (snowball) of the i^{th} size, in meters;
Ni = number of copper spheres of the i^{th} size per unit flat area in sq. meters;
δ (f ) = skindepth, as a function of frequency, in meters.
Cannonball Model
Using the concept of cubic closepacking of equal spheres, the radius of the spheres (a_{i }) and tile area (A_{flat }) parameters for the Huray model can now be determined solely by the roughness parameters published in manufacturers’ data sheets.
Why is this important? Well, as my friend Eric Bogatin often says, “Sometimes an OK answer NOW! is more important than a good answer late”. For example, often during the architectural phase of a backplane design, you are going through some whatif scenarios to decide on a final physical configuration. Having a method to accurately predict loss from data sheets alone rather than go through a design feedback method, described in [7] can save an enormous amount of time and money.
Another reason is that it gives you a sense of intuition on what to expect with measurements to help determine root cause of differences; or sanitize simulation results from commercial modeling tools. If you are like me, I always like to have alternate ways to verify that I have used the tool properly.
Recalling that losses are proportional to the surface area of the roughness profile, the Cannonball model can be used to optimally represent the surface roughness. As illustrated in Figure 3, there are three rows of spheres stacked on a square tile base. Nine spheres are on the first row, four spheres in the middle row, and one sphere on top.
Figure 3 Cannonball model showing a stack of 14 uniform size spheres (left). Top and front views (right) shows the area (A_{flat}) of base, height (H_{RMS}) and radius of sphere (r).
Because the Cannonball model assumes the ratio of A_{matte}/A_{flat} = 1, and there are 14 spheres, Equation 4 can be simplified to:
Equation 5
Where:
K_{SR} (f ) = roughness correction factor, as a function of frequency, due to surface roughness based on the Cannonball model;
r = sphere radius in meters; δ (f ) = skindepth, as a function of frequency in meters;
A_{flat} = area of square tile base surrounding the 9 base spheres in sq. meters.
In my white paper [16] the radius of a single sphere is:
And the area of the square flat base is:
You can approximate the RMS heights of the drum and matte sides by Equation 6 and Equation 7 below:
Equation 6
Where: R_{z_drum} is the 10point mean roughness in meters. If the data sheet reports average roughness, then R_{a_drum} is used instead.
Equation 7
Where: R_{z_matte} is the 10point mean roughness in meters.
Practical Example
To test the accuracy of the model, board parameters from a PCBDesign007 February 2014 article, by Yuriy Shlepnev [5] was used. Measured data was obtained from Simbeor software design examples courtesy of Simberian Inc. [9]. The extracted deembedded generalized modal Sparameter (GMS) data was computed from 2 inch and 8 inch singleended stripline traces. They were originally measured from the CMP28 40 GHz HighSpeed Channel Modeling Platform from Wild River Technology [14].
The CMP28 Channel Modeling Platform, (Figure 4 left credit Wild River Technology) is a powerful tool for development of highspeed systems up to 40 GHz, and is an excellent platform for model development and analysis. It contains a total of 27 microstrip and stripline interconnect structures. All are equipped with 2.92mm connectors to facilitate accurate measurements with a vector network analyzer (VNA).
The PCB was fabricated with Isola FR408HR material and reverse treated (RT) 1oz. foil. The dielectric constant (Dk) and dissipation factor (Df), at 10GHz for FR408HR 3313 material, was obtained from Isola’s isoStack® webbased online design tool [10]. This tool is a free, but you need to register to use it. An example is shown in Figure 5.
Typical traces usually have a trapezoidal crosssection after etching due to etch factor. Since the tool does not handle trapezoidal crosssections in the impedance calculation, an equivalent rectangular trace width was determined based on a 2:1 etchfactor (60^{ }deg taper). The as designed nominal trace width of 11 mils, and a 1oz trace thickness of 1.25 mils per isoStack® was used in the analysis.
Figure 5 Example of Isola’s isoStack® online software used to determine dielectric thicknesses, Dk, Df and characteristic impedance for the CMP28 board.
The default foil used on FR408HR core laminates is MLS, Grade 3, controlled elongation RT foil. The roughness parameters were easily obtained from Oakmitsui [11]. Reviewing the data sheet, 1 oz. copper roughness parameters R_{z} for drum and matte sides are 120μin (3.175 μm) and 225μin (5.715μm) respectively. Because this is RT foil, the drum side is the treated side and bonded to the core laminate.
An oxide or microetch treatment is usually applied to the copper surfaces prior to final lamination. This provides enhanced adhesion to the prepreg material. COBRA BOND® [12] or MultiBond MP [13] are two examples of oxide alternative microetch treatments commonly used in the industry. Typically 50 μin (1.27μm) of copper is removed when the treatment is completed. But depending on the board shop’s process control, this can be 70100 μin (1.782.54μm) or higher.
The etch treatment creates a surface full of microvoids which follows the underlying rough profile and allows the resin to squish in and fill the voids providing a good anchor. Because some of the copper is removed during the microetch treatment, we need to reduce the published roughness parameter of the matte side by nominal 50 μin (1.27 μm) for a new thickness of 175μin (4.443μm).
Figure 6 shows SEM photos of typical surfaces for MLS RT foil courtesy of Oakmitsui. The left and center photos are the treated drum side and untreated matte side respectively. The right photo is a 5000x SEM photo of the matte side showing microvoids after etch treatment.
Figure 6 Example SEM photos of MLS RT foil courtesy of Oakmitsui. Left is the treated drum side and center is untreated matte side. SEM photo on the right is the matte side after etch treatment.
The data sheet and design parameters are summarized in Table 1. Respective Dk, Df, core, prepreg and trace thickness were obtained from the isoStack® software, shown in Figure 5. Roughness parameters were obtained from Oakmitsui data sheet. R_{z} of the matte side after microetch treatment (R_{z} = 4.443μm) was used to determine K_{SR_matte }.
Table 1 CMP28 test board parameters obtained from manufacturers’ data sheets and design objective.
Parameter 
FR408HR 
Dk Core/Prepreg 
3.65/3.59 @10GHz 
Df Core/Prepreg 
0.0094/0.0095 @ 10GHz 
R_{z} Drum side 
3.048 μm 
R_{z} Matte side before Microetch 
5.715 μm 
R_{z }Matte side after Microetch 
4.443 μm 
Trace Thickness, t 
31.730 μm 
Trace Etch Factor 
2:1 (60 deg taper) 
Trace Width, w 
11 mils (279.20 μm) 
Core thickness, H1 
12 mils (304.60 μm) 
Prepreg thickness, H2 
10.6 mils (269.00 μm) 
GMS trace length 
6 in (15.23 cm) 
Keysight EEsof EDA ADS software [14] was used for modeling and simulation analysis. A new controlled impedance line (CIL) designer enhancement, in version 2015.01, makes modeling the transmission line substrate easy. Unlike earlier substrate models, the CIL model allows you to model trapezoidal traces.
Figure 7 is the general schematic used for analysis. There are three transmission line substrates; one for dielectric loss; one for conductor loss and the other for total loss without roughness.
Figure 7 Keysight EEsof EDA ADS generic schematic of controlled impedance line designer used in the modeling and simulation analysis.
Dielectric loss was modeled using the Svensson/Djordjevic wideband Debye model to ensure causality. By setting the conductivity parameter to a value muchmuch greater than the normal conductivity of copper ensures the conductor is lossless for the simulation. Similarly the conductor loss model sets the Df to zero to ensure lossless dielectric.
Total insertion loss (IL) of the PCB trace, as a function of frequency, is the sum of dielectric and rough conductor insertion losses.
Equation 8
To accurately model the effect of roughness, the respective roughness correction factor (K_{SR} ) must be multiplicatively applied to the AC resistance of the drum and matte sides of the traces separately. Unfortunately ADS, and many other commercial simulators, do not allow access to these surfaces to apply the correction properly. The best you can do is to apply the average of (K_{SR_drum }) and (K_{SR_matte }) side to the smooth conductor loss (IL_{smooth }), as described above.
The following are the steps to determine K_{SR_avg} (f ) and total IL with roughness:
1. Determine H_{RMS_drum }and H_{RMS_matte }from Equation 6 and Equation 7.
2. Determine the radius of spheres for drum and matte sides:
3. Determine the area of the square flat base for drum and matte sides:
4. Determine K_{SR_drum} (f ) and K_{SR_matte} (f ) :
5. Determine the average K_{SR_drum} (f ) and K_{SR_matte} (f ):
6. Apply Equation 8 to determine total insertion loss of the PCB trace.
Summary and Results
The results are plotted in Figure 8. The left plot compares the simulated vs measured insertion loss for data sheet values and design parameters. Also plotted is the total smooth insertion loss (crosses) which is the sum of conductor loss (circles) and dielectric loss (squares). Remarkably there is excellent agreement up to about 30GHz by just using algebraic equations and published data sheet values for Dk, Df and roughness.
The plot shown on the right is the simulated (blue) vs measured (red) effective dielectric constant (Dkeff ), and is determined by the equations shown. As can be seen, the measured curve has a slightly higher Dkeff (3.76 vs 3.63 @ 10GHz) than published. According to [6], the small increase in the Dk is due to the anisotropy of the material.
When the measured Dkeff (3.76) was used in the model, for core and prepreg, the IL results shown in Figure 9 (left) are even more remarkable up to 50 GHz!
Figure 8 IL (left) for a 6 inch trace in FR408HR RTF using supplier data sheet values for Dk, Df and R_{z}. Effective Dk is shown right.
Figure 9 IL (left) for a 6 inch trace in FR408HR RTF and effective Dk (right).
Figure 10 compares the Cannonball model against the H&J model. The results show that the H&J is only accurate up to approximately 15 GHz compared to the Cannonball model’s accuracy to 50GHz.
Figure 10 Cannonball Model (left) vs HammerstadJensen model (right).
Conclusions
Using the concept of cubic closepacking of equal spheres to model copper roughness, a practical method to accurately calculate sphere size and tile area was devised for use in the Huray model. By using published roughness parameters and dielectric properties from manufacturers’ data sheets, it has been demonstrated that the need for further SEM analysis or experimental curve fitting, may no longer be required for preliminary design and analysis.
When measurements from CMP28 modeling platform, fabricated with FR408HR and RT foil, was compared to this method, there was excellent correlation up to 50GHz compared to the H&J model accuracy to 15GHz.
The Cannonball model looks promising for a practical alternative to building a test board and extracting fitting parameters from measured results to predict insertion loss due to surface roughness.
For More Information
If you liked this design note and want to learn more, or get more details on this innovative roughness modeling methodology, you can visit my web site, LAMSIM Enterprises.com , and download a copy of the white paper [16], or my award winning DesignCon 2015 paper, [1]. And while you are there, feel free to investigate my other white papers and publications.
If you would like more information on our signal integrity and backplane services, or how we can help you achieve your next highspeed design challenge, email us at: info@lamsimenterprises.com
References
[1] Simonovich, Bert, “Practical Method for Modeling Conductor Surface Roughness Using Close Packing of Equal Spheres”, DesignCon 2015 Proceedings, Santa Clara, CA, 2015, URL: http://lamsimenterprises.com/Copyright2.html
[2] Hammerstad, E.; Jensen, O., “Accurate Models for Microstrip ComputerAided Design,” Microwave symposium Digest, 1980 IEEE MTTS International , vol., no., pp.407,409, 2830 May 1980 doi: 10.1109/MWSYM.1980.1124303 URL: http://ieeexplore.ieee.org/stamp/stamp.jsp?tp=&arnumber=1124303&isnumber=24840
[3] S. Hall, H. Heck, “Advanced Signal Integrity for HighSpeed Digital Design”, John Wiley & Sons, Inc., Hoboken, NJ, USA., 2009
[4] Huray, P. G. (2009) “The Foundations of Signal Integrity”, John Wiley & Sons, Inc., Hoboken, NJ, USA., 2009
[5] Y. Shlepnev, “PCB and package design up to 50 GHz: Identifying dielectric and conductor roughness models”, The PCB Design Magazine, February 2014, p. 1228. URL: http://iconnect007.uberflip.com/i/258943pcbdfeb2014/12
[6] Y. Shlepnev, “Sink or swim at 28 Gbps”, The PCB Design Magazine, October 2014, p. 1223. URL: http://www.magazines007.com/pdf/PCBDOct2014.pdf
[7] E. Bogatin, D. DeGroot , P. G. Huray, Y. Shlepnev , “Which one is better? Comparing Options to Describe Frequency Dependent Losses”, DesignCon2013 Proceedings, Santa Clara, CA, 2013.
[8] Wikipedia, “Closepacking of equal spheres”. URL: http://en.wikipedia.org/wiki/Closepacking_of_equal_spheres
[9] Simberian Inc., 3030 S Torrey Pines Dr. Las Vegas, NV 89146, USA. URL: http://www.simberian.com/
[10] Isola Group S.a.r.l., 3100 West Ray Road, Suite 301, Chandler, AZ 85226. URL: http://www.isolagroup.com/
[11] Oakmitsui 80 First St, Hoosick Falls, NY, 12090. URL: http://www.oakmitsui.com/pages/company/company.asp
[12] Electrochemicals Inc. COBRA BOND®. URL: http://www.electrochemicals.com/ecframe.html
[13] Macdermid Inc., Multibond. URL: http://electronics.macdermid.com/cms/productsservices/printedcircuitboard/surfacetreatments/innerlayerbonding/index.shtml
[14] Keysight Technologies, EEsof EDA, Advanced Design System, 2015.01 software. URL: http://www.keysight.com/en/pc1297113/advanceddesignsystemads?cc=US&lc=eng
[15] Wild River Technology LLC 8311 SW Charlotte Drive Beaverton, OR 97007. URL: http://wildrivertech.com/home/
[16] Simonovich, Bert, “Practical Method for Modeling Conductor Surface Roughness Using The Cannonball Stack Principle”, White Paper, Issue 1.0, April 8, 2015,
URL: http://lamsimenterprises.com/Copyright.html
Are Guard Traces Worth It?
Originally published in, The PCB Design Magazine, April 2013 issue.
By definition, a guard trace is a trace routed coplanar between an aggressor line and a victim line. There has always been an argument on whether to use guard traces in highspeed digital and mixed signal applications to reduce the noise coupled from an aggressor transmission line to a victim transmission line.
On one side of the debate, the argument is that the guard trace should be shorted to ground at regular intervals along its length using stitching vias spaced at 1/10th of a wavelength of the highest frequency component of the aggressor’s signal. By doing so, it is believed the guard trace will act as a shield between the aggressor and victim traces.
On the other side, merely separating the victim trace to at least three times the line width from the aggressor is good enough. The reasoning here is that crosstalk falls off rapidly with increased spacing anyways, and by adding a guard trace, you will already have at least three times the trace separation to fit it in.
In our DesignCon2013 paper titled, “Dramatic Noise Reduction using Guard Traces with Optimized Shorting Vias”, I coauthored along with Eric Bogatin, we showed that sometimes guard traces were effective, and sometime they were not; depending on how the guard trace was terminated. By correct management of the ends of the guard trace, we demonstrated it can reduce coupled noise on a victim line by an order of magnitude over not having the guard trace present. But if the guard trace was not optimized, the noise on the victim line can also be larger with the guard trace, than without.
Analysis Using Circuit Models
We started out the investigation by building circuit models for the topologies studied. Agilent’s EEsof EDS ADS software was used exclusively to model and simulate both stripline and microstrip configurations. The generic circuit model, with a guard trace, is shown in the top half of Figure 1. The circuit model, without a guard trace, is shown in the bottom half.
For the analysis, we used lossless transmission line models. The guard trace length was exactly matched to the coupled length. The ground stitching and the endtermination resistors, on the guard trace, could be deactivated, and/or shorted, as required. The linewidth space geometry was set at 555 mils, and the spacing for the nonguarded topologies was set to three times the line width.
Figure 1 ADS schematic for generic topologies with a guard trace (top) and without (bottom). The transmission line were segmented and parameterized to easily change the lengths as required. The ground stitching and the endtermination resistors, shown in top schematic, can be deactivated and/or shorted as required.
Figure 2 is a summary of results when a guard trace was terminated in the characteristic impedance, left open, or shorted to ground at each end. The red waveforms are the results for topologies without a guard trace, and the blue waveforms are with a guard trace.
Depending on the nature of the termination, the reinfected noise on the guard trace can add or subtract to the directly coupled noise on the victim line. This often makes the net noise on the victim line worse than without a guard trace.
Unlike a simple twoline coupled model, where the near end crosstalk (NEXT) and far end crosstalk (FEXT) can be easily predicted from the RLGC matrix elements, trying to predict the same for a threeline coupled model is more difficult. Manually keeping track of all the noise induced on the guard trace, and its reinfection onto the victim line, is extremely tedious. First you must identify the directly coupled reinfected backward and forward noise on the victim line from the voltage on the guard trace. Then the problem is keeping track of the multiple reflections of the noise on the guard trace. Because of this, the only real way to analyse the effect is through circuit modeling and simulation.
In microstrip topologies, as you can see, there is little to no benefit to adding a guard trace; regardless of how the ends are terminated. This is because microstrip topologies are inherently prone to far end crosstalk. Therefore any far end noise, coupled onto the guard trace, will subsequently reinfect the victim with additional far end noise; as seen by the additional ringing superimposed on the blue waveform.
In stripline topologies, without a guard trace, there is no farend cross talk generated. But when a guard trace is added, and depending on how the ends are terminated, any near end coupled noise on the guard trace can reinfect the victim. It is only when the ends are shorted to ground we see such a dramatic reduction of both near and far end noise.
Figure 2 Summary of simulation results when the ends of the guard trace was terminated, left open or shorted to ground for microstrip and stripline geometries.
Distributed Shorting Vias
When practically implementing a guard trace, to act as a shield, a rough rule of thumb suggests the spacing of shorting vias should be at least 1/10 the wavelength of the highest frequency content of the signal. For a risetime of 100 psec, the stitching via spacing, to meet l/10, is 0.18 inches; or 9 stitching vias over 1.5 inches.
Figure 3 summarizes the results when a guard trace was stitched to ground at multiple wavelengths; compared to the case of no guard. As you can see, in the case of microstrip, when the guard trace is shorted with fewer than 9 vias, there is still considerable ringing noise on the guard trace which can reinfect the victim line. But in the case of stripline, having two shorting vias at each end, or any number up to 9 shorting vias has the same result. This suggests there is no need for multiple shorting vias, other than at the end of the guard trace; as long as the guard trace is the same length as the coupled length. This dramatically simplifies the use of guard traces in stripline.
Figure 3 Summary of simulation results with guard trace stitched for microstrip and stripline geometries.
Practical Design Considerations
Up until now we have modeled and simulated ideal cases of shorting the guard traces to ground. But in reality, there are additional practical design considerations to consider. First is via size, and the impact it has on the line to line spacing. Next is the finite via inductance; since its impedance will prevent complete suppression of the noise on the guard trace. And finally, the extension of the guard trace compared to the coupled length.
Because through hole manufacturing design rules limit the smallest via and capture pads, the smallest mechanical drill size most PCB vendors will spec is 8 mils. By the time you factor in the minimum pad diameter and pad to copper spacing, the minimum space between the aggressor and victim lines would have to be at least 28 mils, as shown in Figure 4; just to fit a guard trace with grounding vias down its length.
At this point, you have to ask yourself if it is even worth it; especially for microstrip topologies. If the two signal lines were to be increased to 28 mils, the reduction in cross talk from just the added separation would likely be more significant than adding the shorted guard trace.
Figure 4 Minimum track to track spacing to fit an 8 mil drilled via and pad in throughhole technology.
Fortunately, the circuit analysis has shown there is little benefit to adding a guard trace to microstrip topologies, even if it was ground stitched appropriately. But to gain a dramatic reduction in cross talk in stripline all that is required is to short the guard trace at each end, and ensure the guard trace is exactly the same length as the coupled length. This means the minimum space to fit a via and guard trace can remain at three times the line width; as long as the guard trace is extended slightly, as shown in Figure 5(a). Alternatively, the guard trace can be made equal to the coupled length, as illustrated in Figure 5(b).
Agilent’s ADS Momentum planar 3D field solver was used to explore and quantify the implications vias and guard trace lengths have on noise reinfection. Figure 5 details a portion of the 3D model on the left end of the respective topologies. The right hand sides are identical. The reference planes are not shown for clarity.
Figure 5 Two examples of adding a grounded guard trace with minimum spacing of 3 x line width. Figure (a): guard trace is extended past the coupled length (A) by dimension B on both sides in order to satisfy minimum 5 mil padtrack spacing requirements. Figure (b): guard trace is equal to coupled length by separating the traces at each ends. Modeled in Agilent Momentum 3D field solver. Reference planes are not shown for clarity.
After simulation, the Sparameter data was saved in Touchstone format and brought into ADS for transient simulation analysis and comparison. Figure 6 shows the results. The plot on the left used 100 psec risetime for the step edge, while the plot on the right used 50 psec. Both plots are consistent with the dramatic noise reduction observed in Figure 2, except here we see some added noise ripple after about 0.8 nsec.
At 100 psec risetime, there is effectively no difference in near end noise signature for either (a) or (b) topology. But when the risetime was reduced to 50 psec, the noise ripple is more pronounced. The blue waveform shows that even when dimension B is 0 mils, there is still a small amount of noise due to the inductive length of the vias to the reference plane. The red waveform shows that adding just 12 mils to the guard trace length, at each end, the ripple magnitude is almost doubled.
It is a wellknown fact that technology advancements over time results in faster and faster rise times. If you have engineered your design on the technology of the day, any future substitution of parts, with faster rise time, may cause your product to fail, or worse be intermittent.
Figure 6 Momentum transient simulation results comparing near end crosstalk at Port 1 when aggressor voltage was applied to Port 3. The red and blue waveforms are with a guard trace. The green waveform is with no guard and 15 mils separation. Aggressor voltage = 1V, 100 psec risetime (left) and 50 psec risetime(right)..
To explore this phenomenon, the guard trace was varied by 50 and 100 mils at each end, as illustrated in Figure 7. Here we can see that as the guard trace gets longer at each end, the noise ripple grows in magnitude quite rapidly. It is remarkable to note that when the guard trace is just 100 mils longer, at each end, the peakpeak amplitude of the noise just about equals the peak magnitude of the no guard case.
Figure 7 Momentum transient simulation results with guard trace extended. B = 12 mils (red), B = 50 mils (blue) and B = 100 mils (magenta) compared to no guard (green). Aggressor voltage = 1V, 100 psec risetime. Dimensions in mils.
When the guard trace was removed, and the space was increased to five times the line width, the near end crosstalk was reduced in magnitude and was approximately equal to the guard trace scenario, as seen in Figure 8. Furthermore, because there is no guard trace, there is no additional noise ripple.
Figure 8 Momentum transient simulation results comparing near end crosstalk at Port 1 when aggressor voltage was applied to Port 3. Aggressor voltage = 1V, 100 psec risetime.
So getting back to the original question, “Are guard traces worth it?” You be the judge. Using a guard trace, shorted at each end, can be effective, if you need the isolation. But it does have caveats. If you decide to go down this path, it is imperative for you to model and simulate your topology, preferably with a 3D field solver, before signing off on the design.
Reference

Eric Bogatin, Bert Simonovich,“Dramatic Noise Reduction using Guard Traces with Optimized Shorting Vias”, DesignCon2013, Santa Clara, CA, USA, Jan 2831, 2013.
PCB Vias Are Capacitive But Not Necessarily Capacitors
Huh? …… What do you mean by that? ……
For years now the popular opinion was that PCB vias were capacitive in nature, and therefore could be modeled with lumped capacitors. Although this might be true when the rise time of the signal is greater than or equal to 3 times the delay of the via discontinuity, I’ll show you why it is no longer appropriate to think this way; even risky to continue to model your highspeed channel using this methodology.
Let’s start the discussion by saying vias are transmission lines with excess parasitic capacitance or inductance. Vias are considered transparent when their impedance equals the characteristic impedance of the transmission lines attached to them. In almost all cases, vias passing through multilayer PCBs are capacitive because of the distributed capacitance between the via barrel and antipads. As a result, they end up having lower impedance than the traces connected to them. Like any other transmission line, when a rising edge of a signal encounters a lower impedance, it will cause a negative reflection for the length of the discontinuity.
Getting back to the point, it is best demonstrated by an example as summarized in Figure 1. Consider a via at the far end of a long 50 Ohm transmission line. The via has a short through section and a long stub section. The through section is 15 mils and the stub is 269 mils for a total via length of 284 mils. This is not unusual for modern backplane designs.
For this particular via geometry, the impedance is 33 Ohms and the excess via capacitance is 1.9pf. Even with a fast 50ps rise time at the source, by the time the signal reaches the via at the far end, the rise time will degrade due to dispersion caused by the lossy dielectric. In this example, after 23 inches, the rise time has degraded to approximately 230ps.
If the total delay (TD) of the via discontinuity is 60 ps, then the 230 ps rise time at the via is greater than 3TD (180ps). As expected, when modeling the via with a lumped capacitor equal to the excess capacitance, and comparing it with the transmission line via model, the TDR plot of the reflections are virtually the same using a 230ps rise time.
Figure 1 Via model TDR comparison after 23 inches. Top topology uses 33 Ohm transmission lines for both the through and stub portion of the via. The bottom topology models the via with a 50 Ohm transmission line to represent the delay of the through portion and a 1.9pf capacitor to represent the excess capacitance. Modeled and simulated with Agilent ADS.
So far so good, right? Well maybe so. The only way to know is to explore this topology even further and compare eye diagrams. Let us say your circuit needs to work at XAUI rate of 3.125 GB/s. You modify both topologies by adding a driver and receiver. After simulating you end up with eye diagrams as shown in Figure 2.
Figure 2 Eye comparison at 3.125Gb/s. Top topology uses 33 Ohm transmission lines for both the through and stub portion of the via. The bottom topology models the via with a 50 Ohm transmission line to represent the delay of the through portion and a 1.9pf capacitor to represent the excess capacitance. Modeled and simulated with Agilent ADS.
Still ok. So what is your point, you might ask?
You are correct when you comment there is a good match for reflections and the eyes are wide open. Ah, but now let us say you want to run this at 10GB/s down the road. So you dial up the bit rate on the transmitters and simulate both topologies again. But this time, you get some unexpected results as shown in Figure 3.
Figure 3 Eye comparison at 10Gb/s. Top topology uses 33 Ohm transmission lines for both the through and stub portion of the via. The bottom topology models the via with a 50 Ohm transmission line to represent the delay of the through portion and a 1.9pf capacitor to represent the excess capacitance. Modeled and simulated with Agilent ADS.
Ouch! What happened here? Looking at the TDR, the reflections at the end of the channel look the same so why doesn’t the receive eyes match? To answer this question, we really need to look at the Sparameter plots of both channels. Figure 4 shows the insertion and return losses of both topologies. Red is the transmission line model and the blue is the capacitor model.
Figure 4 Insertion and return loss of both topologies. Red curves are the transmission line via model and blue curves are the capacitor model.
The insertion loss plot represents the transmitted output power vs. frequency while the return loss is the reflected power vs. frequency. In the time domain, the insertion loss and return loss is equivalent to the TDT and TDR plots respectively. As you can see, the return loss matches pretty well; just like the TDR plot we observed earlier, but It is only obvious when we view the insertion loss plot as to the real reason for the eye discrepancy of Figure 3.
Notice the first resonant null at approximately 4.5 GHz. This null represents the quarter wave resonant frequency fo, and is due to the long 269 mil via stub. The other null at 13.5GHz is the 3rd harmonic of fo. The longer the stub length, the lower the resonant frequency. When there is a null at or near onehalf the bit rate, then the eye will be devastated. In our example, 4.5GHz is approximately half of 10GB/s and as you can see from Figure 3 the resultant eye is totally closed.
But the Sparameters tell us even more. We can use them to confirm the rule of thumb used earlier with respect to the rise time of the signal being greater than, or equal to, 3 times the delay through the via discontinuity.
If you study the return loss plot, you will see there is an excellent match up to about 1.83GHz. This is the effective bandwidth for which the capacitor model is good for. Put another way, a bandwidth of 1.83GHz means you could use an equivalent capacitor model for the via for bitrates up to 3.6GB/s.
Equation 1 is a commonly used to convert 3dB bandwidth to equivalent 1090 rise time. Substituting 1.83 GHz for the 3dB bandwidth, the rise time equals approximately 185 ps.
Equation 1
When you divide 185 ps by 3, you end up with approximately 62ps compared to approximately 60ps for the propagation delay through the via we originally determined earlier.
Figure 5 is a summary of a simulation with the transmission line length reduced to 18 inches to reduce the rise time to 185 ps. As you can see the transmission line via model’s eye at 3.6 Gb/s is just starting to distort while the capacitor model is still relatively smooth; confirming our bandwidth rule of thumb. Using a capacitor as a via model past this bitrate will result in optimistic results and long nights when your 10 Gig prototype hits the lab.
So now you see what I mean when I say that vias are capacitive, but not necessarily capacitors.
Figure 5 Eye comparison at 3.6Gb/s. Top topology uses 33 Ohm transmission lines for both the through and stub portion of the via. The bottom topology models the via with a 50 Ohm transmission line to represent the delay of the through portion and a 1.9pf capacitor to represent the excess capacitance. Modeled and simulated with Agilent ADS.
For more Information:
If you liked this design note and want to learn more, or get more details on modeling vias using transmission lines, you can visit my web site, LAMSIM Enterprises.com , and download a copy of the white paper I wrote along with Eric Bogatin and Yazi Cao titled, “Method of Modeling Differential Vias” .
While you are there, feel free to investigate my other white papers and publications.
If you would like more information on our signal integrity and backplane services, or how we can help you achieve your next highspeed design challenge, email us at: info@lamsimenterprises.com.
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.