In Part 1 and Part 2 I covered a list of items that are not particularly well handled by typical implementations of SPICE. Now, you'll get the other side. Don't get the idea that nothing works in circuit solvers at microwave frequencies. A lot does work.

As pointed out earlier, there are things that cannot be handled without the aid of field solvers, but the idea is to characterize features with the aid of the field solver, translate that characterization into lumped models that SPICE can deal with, and then do the signal integrity work with the SPICE tool.

Any time such a translation is made, there is a frequency range wherein those models are valid. Any time such a model is generated, it should also have the frequency range of applicability specified.

Again, I want to emphasize that there are numerous tools - circuit solvers - which, at heart, are versions of SPICE. The one critical property that such a tool absolutely needs if it is to be useful at microwave frequencies, is the ability to work accurately with transmission lines that have frequency-dependent loss.

Without this capability, it is very difficult to get useful information out of a simulation. That is not to say that without such capability you are not going to be able to work with microwave frequencies; rather, without that capability, reconcile yourself to working with some tool other than SPICE.

Frequency Dependent Loss
Frequency-dependent loss (FDL) is due primarily to two factors: copper loss and dielectric loss. The word "primarily" is used intentionally. Other sources, such as EMI, are important, even very important, from some perspectives. But, for the signal integrity modeling of transmission lines, these two are what will be covered by the description of frequency-dependent loss.

Numerous of the factors impacting the signal available at the receiver are functions of frequency. Examples are radiation reflections and crosstalk, all of which SPICE can be really good at. But these are not included in the meaning assigned here. Here, the words "frequency-dependent loss" mean resistive losses in the copper and dielectric losses.

In fact, signal available at the receiver is often described in terms of eye opening, a concept that will be described later. In that sense, even crosstalk can be a major contributor to signal loss. But all that is yet to come. If you needed something to look forward to, there it is. For now, you need details about copper and dielectric losses.

Copper Loss
Copper has resistive loss as does any conductor. At high frequencies, the internal inductance of conductors pushes the current to the outer surfaces; this effect, shown in Figure 7.15 below, is called skin effect.

Figure 7.15. Skin Effect

This phenomenon decreases the effective area available for current flow and so increases the effective resistance. It is as if there is only a thin layer on the surface of the conductor that is involved in high-frequency current flow, and the thickness of this layer is called the skin depth. As with many physical constants, mathematical operators, and similar scientific things, skin depth is designated by the Greek delta symbol as shown below.

In this equation, pi has its usual meaning, 3.14 and so on, f is the frequency in Hertz, mu is the magnetic constant—usually that of free space, except when not—and sigma is the conductivity of the metal. In this list, the one that is often overlooked is mu.

In copper, gold, silver, and such metals, the relative magnetic constant is unity so that of free space is correct. In metals such as nickel and iron, the relative magnetic constant can be very high. If you want to generate a low-loss conductor for microwave frequencies, magnetic materials are a poor choice. On the other hand, if you really want to have a lot of loss, such as in a chassis, iron might be a really good choice.

The loss due to skin-effect is high at microwave frequencies. Increasing the value of sigma can reduce it. If gold is substituted for copper, this loss will decrease by a couple percent. On the other hand, the loss is inversely proportional to the circumference of the conductor, so increasing the conductor size by a few percent can do the same. Decide for yourself which to do - which makes better economic sense for your design.

The current density decreases exponentially with depth in the conductor. The meaning of skin depth is that it is the equivalent depth if the current were evenly distributed in that skin layer. It is used to calculate the effective resistance of the conductor for a particular frequency.

As an aside, consider what might happen if the skin depth is larger than the thickness of the conductor. Consider this in the context of a reference plane. Fields will be attenuated, but not blocked, by the conductor.

Can this be a problem? Consider one more situation. Your board has a switching regulator mounted on it. That regulator is running at 70 or 80 kilohertz and switching tens of amps. It is a very bad idea, a very bad idea, to run a signal trace under the switching transistor, even though there may be a reference plane between.

Conductor thickness
In printed circuit boards, conductor thickness is usually a constant, so loss in a trace is strongly dependent on trace width. If the impedance is to be maintained, increasing trace width requires greater dielectric thickness. That dependency often means that the total thickness of the board stackup is strongly related to the trace loss, and so can strongly influence the maximum frequency that can be transported a specified distance on a circuit board.

Although dielectric loss increases at a faster rate than does copper loss and at high enough frequencies becomes the dominant material loss, copper loss never becomes negligible. Dielectric loss is sometimes regarded as the only loss that counts. This is a mistake.

In real circuitry, total loss is made up of numerous contributors and, while dielectric loss can become a major contributor at frequencies of one or more gigahertz, it is never the sole contributor. In fact, when package losses, impedance mismatches, connector losses, passives, and copper loss are all accounted for, dielectric loss seldom even contributes the majority of the loss.

Copper loss comes not only from the bulk resistivity of the copper, it also comes from surface roughness and from other materials used at the surface of the copper. Sometimes the copper has a solder plating on it—note that solder has a resistivity about five times higher than copper. Tin plating is often used. Tin has much higher resistivity than copper.

When a fiberglass core is made, often the copper is roughened and coated with copper oxide to increase adhesion. That is unfortunate, but needed. It is always advisable to remove any metal coatings, except perhaps gold, that are not absolutely required for reliable manufacturing of the board. In short, make it as good as you can, but not better.

Dielectric Loss
In dielectrics, the relative dielectric constant is thought to be due to such things as the physical distortion of molecules, the reorientation of molecules, the changing of the shape of electron orbits, etc., as shown in Figure 7.16 below. Each case has a stimulus and a response.

Figure 7.16. Molecules in an Electric Field

In such systems, the response always lags the stimulus by some amount. The lag in response shows up in vector representations of the dielectric constant as an imaginary part. When calculating the response of the system to fields through this dielectric, the imaginary part of the dielectric constant shows up as a loss.

It is typical that the delay in field response is somewhat constant. That is, the dielectric response to the imposed field lags by a small, fixed amount of time. In this case, the relationship between the real and imaginary parts of the dielectric response vector is linearly dependent on frequency of the imposed field. Thus, dielectric loss is approximately linearly dependent on frequency.

The dielectric loss is often specified by the angle of the dielectric vector, illustrated in Figure 7.17 below. The tangent of this angle—that is, the tangent equal to the imaginary part divided by the real part of the dielectric constant—is often published as the loss factor for the dielectric.

Figure 7.17. The Dielectric Constant

In another feat of scientific innovation, the ratio itself is designated by the Greek lower-case delta symbol. This is done, presumably, to maximize the probability of confusing the dielectric loss with the skin depth.

Of course, there is no relationship between the two, but why miss such a golden opportunity to generate confusion? The dielectric loss factor is thus designated tan-delta, which delta is symbolically identical to the skin depth, but is physically unrelated in any way as shown below:

At low frequencies and in practical materials, copper loss dominates and dielectric loss is safely ignored. Depending on geometry, at moderate frequencies of about one gigahertz in FR4, dielectric loss catches up and becomes about equal to copper loss. At higher frequencies, dielectric loss dominates.

The dominance of dielectric loss does not mean that copper loss has gone away. It is still there. It still is increasing as frequency increases. You will occasionally encounter the idea that changing the board material to one of the low-loss materials will reduce signal loss by an amount equal to the improvement in dielectric loss. This of course is far from true. To see for yourself, simulate your total link, silicon to silicon, and vary only the dielectric loss parameter.

When you are looking for a SPICE simulator capable of dealing with frequency-dependent loss, one choice is the W element available in HSPICE. This is not intended to be an endorsement of HSPICE, but rather a simple statement that it is an option, and it appears to work.

Other options also appear to work; not all include the word "SPICE" in their names. The advantage of tools that include that word in their names is that they tend to be fairly standard in the code format that they accept. Other tools have other advantages and, as usual, you need to choose the tool that fits the job.

Drivers and Receivers
From the perspectives of circuit simulators, all drivers are essentially the same. Circuitry will vary, but it makes little difference to the circuit simulator whether that circuit is outputting microwave signals or lower frequencies.

My own bias is to simplify drivers and receivers through use of ideal sources surrounded by appropriate parasitics whenever possible. The advantage of this method is that it typically runs a couple orders of magnitude faster in SPICE than do transistor-level models. Of course, some refuse to believe that this method could ever generate acceptable accuracy.

To them I point out that even the transistors in the transistor-level models are themselves parametric models. Useful models are sometimes as simple as the one depicted here in Figure 7.18 below, but often need to be substantially more complex.

Figure 7.18. My Favorite Driver Model

Certainly there are cases where there is no choice available other than running the transistor-level circuitry. But avoid doing so when possible. Whether at microwave frequencies or not, these complicated circuits cause numerous problems in trying to get a simulation running. Such models are often automatically generated from the layouts of the driver or receiver circuit.

When so generated, they often are found to include component arrangements that are physically possible but cannot be handled by SPICE. Most common is the situation where a node joins three capacitors, and nothing else. The DC solution at this node is indeterminate, so SPICE will fail.

It is my recommendation that a vendor should never release a SPICE model that has not been verified functional in a real simulation, and a customer should never accept such a model. Getting back to the real world, if you are stuck with such a model, the only choice may be to go through it line-by-line and modify it so it will work. Take that three-capacitor node and add a ten-meg resistor to ground.

Packages
At microwave frequencies, packages cannot be ignored. Nor is it likely to be adequate to model a package pin as a simple inductor or even a capacitor and inductor. The length and crosstalk of the trace in the package coupled, with the tolerance of the termination presumably on the chip, will result in a frequency-dependent impedance at the pins of the connector.

An optimized board interconnect has to, absolutely must, include these factors. It would not be as bad if the termination could be relied on as being purely resistive, but the pin capacitance at the silicon will typically, at the very least, be significant, and sometimes even the dominant impedance at the high-frequency end of the spectrum. Also, crosstalk in the package will sometimes be a significant factor.

Even though signal characteristics may well be specified at the pin at the point where the package meets the board, it is not adequate to specify impedance as a single number at that point. Optimized board design will require that the impedance either be explicitly defined as a function of frequency, or be implied by specifying a transmission line model for the package.

Significant problems can occur when generating a model of a package. You might rely solely on simulations, but the real physical entity might not really hit the mark chosen for the simulation. Simulations are great tools, but measured values make a better basis for a working model.

Note that there is not exactly universal agreement on that last statement, but authors get to state their opinion. The design of the package will have made good use of simulations, but the final characterization of the physical part should be based on measurement.

Two measurements are available: time domain (TDR) and frequency domain (NA). In either case, SPICE models will usually be the translation of these into some form of transmission line model. This can be done by something such as the application of the peeling algorithm. If you are using such a model, you have the easy job. If you are the one who must generate this model, you probably already know that you have the hard job.

The special mechanical requirements of packages make the use of field solvers unavoidable in many cases. Often the physical size requirements force the use of very thin conductors and result in the accompanying high loss. Mechanical requirements placed on the reference planes often result in geometries that cannot be accommodated by the 2D field solvers found in many signal integrity tools.

Recall that as shown earlier in this series, a lumped element transmission line model, and a single section was deemed adequate because the section was physically short. In the case of packages, the transmission lines are often not short enough to model with a single section.

If you try to model a transmission line that is too long as a single lumped section, you'll get substantial errors at high frequencies. This can easily be seen by SPICE frequency sweeping the model with a single and with multiple sections.

To model a line with n sections, simply calculate the inductance and capacitance values for a single section, then divide those values by n; repeat the section n times. Recall that knowledge of the dielectric constant and impedance of a line is adequate to calculate the inductance and capacitance per unit length. Scale those values to the actual length of the segment that is to be modeled.

I modeled an inch-long segment of transmission line with one, two, and three segments. The frequency response, shown in Figure 7.19 below , of each look good up to about a gigahertz. By the time you get to two gigahertz, the one-segment model begins looking inadequate.

By the time you get to five, only the three-segment case looks usable. This illustrates the impact of using too few segments to model a section of transmission line for a particular range of frequency.

Figure 7.19. Three L-C models

Reference was previously made to a rule sometimes called the tenth-wavelength rule. It says something like, "Always keep segment size in your models at most a tenth wavelength of the highest frequency you are concerned about." Examination of Figure 7.19 can show just how much error would result from relaxing this rule in this case.

Let me climb onto my soap box: It is no worse to violate a rule of thumb than it is to use it without understanding what it does for you. Rules of thumb save us a lot of time. If used intelligently, they can even promote good engineering.

Breakouts
Breakouts, the circuitry that interfaces the package or connector to the circuit board, are problematic. The realities of snaking a trace through a pin field, or attaching a connector to a pad, often force significant deviations from the ideal geometries and impedances desired for the traces.

At microwave frequencies, the first half inch or so of trace can easily account for the majority of the near-end crosstalk. This much trace can easily be entirely in the breakout region. The breakout region is best treated as a distinct entity when you do your modeling.

Figure 7.20. The Break-Out Under a BGA

Sometimes the electrical characteristics of the package or connector itself are significantly influenced by the details of the breakout. In such cases, it makes sense to include some or all of the breakout on the circuit board as part of the package or connector, including it in the package or connector model.

It makes little sense, for example, to characterize a connector that mandates use of a through-hole via of some size, without including that via in the characterization of the connector. The problem with this is that the model may then need to include a board-thickness parameter in some way.

For reasons of cost, packages are tending to finer pitches and closer spacings. At the same time, higher frequencies and the attendant greater losses call for wider traces. It is often found that traces in breakout regions simply cannot meet impedance, loss, and crosstalk characteristics desired for the rest of the board.

In simulations, it is necessary to optimize the breakouts and then choose the remaining interconnect to accommodate what is left of the interconnect budgets. That is, it is much easier to limit crosstalk in the long trace run across the board than it is to do so on the breakout region. It is much easier to hit the precise desired impedance out in that open space than it is in the very confined regions of the breakout.

Figure 7.21. A Typical Interconnect Design

Interconnects
The interconnect circuit is the entire assembly of features and traces that connect a transmitter to a receiver, as seen in Figure 7.21 above. This often involves numerous discontinuities and variations that are difficult to reliably deal with in hand calculations.

Up to now, the discussion has focused on how to calculate impedance as a function of distance from a discontinuity, how to calculate the cumulative effect of multiple discontinuities, and how to do all sorts of things by hand. SPICE simulators do an excellent job of dealing with all those things for you.

Having been told that, do not conclude that all the mathematical derivations have been for nothing. Without understanding the mathematics and physics behind what is happening, you would have no idea of how to make improvements when SPICE says that the interconnect link is broken.

You may have little interest in working with things like hyperbolic functions to determine the impedance at a position in the line, when SPICE can do it easily. But now you know how it works and will have ideas of what to do when SPICE says your link is busted.

In modeling the interconnect, it is important to recognize that, unless you take steps to overcome it, all simulations treat the world as ideal. The transmission line in the simulator does not randomly vary in width. The transmission line doesn't encounter regions of varied dielectric constant as traces on FR4 really do. In a simulation, unless you intentionally model the variations, everything is beautifully perfect—and not very realistic.

Connectors
Connectors are a real challenge for measurements and modeling. But that is starting to sound like a mantra by now. What isn't a real challenge? The dominant thing you need to know about connectors is that they often will be major locations of crosstalk in the link.

Assume you choose a connector that matches your line impedances. It is typical for the crosstalk of connectors to have a bigger impact on signal integrity at microwave frequencies than loss in the connector has. Never consider using a particular connector if its crosstalk is not well specified.

Don't settle for statements such as a connector has such-and-such percent crosstalk. Drill down and find out what that statement really means. It is fairly easy to get good crosstalk from a single aggressor signal or a slow rise time. But what is needed is the total sum of the contributions of all nearby signals at an appropriate rise time or frequency range.

Take a look at Figure 7.22 below. In some geometries there can be many more than just one or two aggressors coupling into a particular pin or pin-pair. You can't really blame a vendor if all they give you are accurate numbers, but not necessarily the numbers you need.

Figure 7.22. A Connector with Multiple Crosstalk Aggressors

If it is necessary to model this connector in a system simulation, who will provide the model and what type of model will it be? Every model for any device has a limited range of accuracy.

Questions you need to ask about connector models include over what frequency range is the model accurate and what level of accuracy does it provide in that frequency range? Also understand the conditions under which the model is characterized.

There have been cases where board features that were absolutely required for the connector were not included in the model because they made the connector performance look worse. A useful model is a model that accurately represents how the device will perform in a real application. Real applications often use board-to-board connectors actually mounted on boards.

Another aspect of connector selection you need to think about is the physical length of the path through the connector. Consider modeling an ideal lossless connector in SPICE. The only parameter you need to vary in this model is the length of the connector.

As an example, make the impedance of the path through the model exactly 50 ohms. In a real implementation, the circuits that go to this connector may target 50-ohm impedance too, but there will be a real-world tolerance. So model the line in and out of the connector as 45 ohms and terminate both ends at 45. Now run frequency sweeps at various physical lengths in the connector.

If you do this experiment, what you will see is that the connector, even with ideal lossless lines, acts something like a low-pass filter. And you will see that the knee frequency depends on the length of the connector.

Cables
Cables are not all that different from what has been already covered. Losses in cables tend to be substantially less than in FR4. Some really good cables are out there, but even the mediocre ones that are practical for use in consumer electronics are really good compared to FR4.

Expect losses in cables to be in the range of cable loss-per-meter equal to FR4 loss-per-inch. If microwave cabling is new to you, you should know some things.

The first goes something like this: if you name a loss figure, a cable can be found that can meet it. This fact, that exceedingly wideband and low-loss cables exist, is not really relevant to the design of circuitry for consumer applications.

It is not an exaggeration to state cables that cost over $1,000 per meter are readily available. I have some in my lab. For their application, they are the right choice. Their application is definitely not consumer electronics.

The $600 and the $30 per meter cables also have valid reasons for existence. In consumer applications, what you need are the cables that are closer to the dollar-or-less per meter items. These, too, exist. In these, the connectors on the ends may cost more than the cable material itself. The nemesis of the engineer with a cable need is the vendor who claims to have a cable that solves all those problems, but the price isn't stated.

Besides that, one of the major differences between cable and trace is that it is quite difficult to get really good length matching on the individual conductors in a cable. As the number of pairs in a cable increase, this problem becomes worse.

In traces on the board, matching lengths is fairly easy and matching velocities more difficult. In cables, matching lengths is the more difficult proposition. It sometimes is also useful to note that the common-mode impedance in a cable may be very different than that on the circuit board. This can be true even though both have precisely the same differential impedance.

It is significant to note that cables can present very severe ESD problems. Those center conductors in cables can sometimes support thousands of volts of charge. The human body ESD model includes a 1,500-ohm series resistor. But when that cable plugs in, the series resistance is in milli-ohms.

So, at least in the lab, always put a terminator on a cable to discharge it before plugging it into your equipment. It is a good idea to lose sleep at night, figuring out how this will be handled by consumers if you have a cable that goes outside your chassis.

The same frequency-dependent-loss transmission lines that were used to model traces are used to model cables in SPICE. Of course, the loss tangents are quite different.

An interesting phenomenon has shown up in cable assemblies designed to meet specific interconnect standards. When the maximum loss allowed for a cable at a specific frequency is specified, all cables, independent of length, tend to have that loss. Consider a cable of some length and loss, cut it in half, and the measured loss will now also be cut in half. That is not what is happening here.

Figure 7.23. Quad and Twin-Ax Cable Constructions

When all else is the same, the cable loss tends to decrease as the cable diameter is increased; the cable cost increases as the cable diameter increases. If the maximum loss is specified, the manufacturer minimizes cost by decreasing cable diameter, increasing cable loss to the specified limit. So it is that in this circumstance, cable diameter tends to decrease as length decreases, rather than cable loss decreasing as length decreases.

Crosstalk in differential cables, both quad construction and twin-ax construction, illustrated in Figure 7.23 above, is typically dominated by the connectors. If the cable length is doubled, the crosstalk does not double, it may even show very little increase. Often an important cable parameter is the quality of the shielding.

Again, it is possible for the connectors to make major contributions to EMI. If there was no common-mode signal entering the cable, radiation would not be a significant problem, but since cable lengths are difficult to match and connectors are not perfect, common mode can be generated by the cable connectors themselves.

Next  in Part 4:  Modeling philosophy
To read Part 1, go to "Unmodelable features of high performance designs"
To read Part 2: go to: "Differiental transmission lines and  receivers."

Dennis Miller has worked in electronics since 1963. His early engineering interests and education centered on control theory and numerical analysis. Now his interests are signal integrity and numerical analysis. Since joining Intel Corp. in 1991, he has been instrumental in the development of Infiniband technology and similar high speed signaling technologies.

This series of articles is based on material from Designing High Speed Interconnect Circuits," by Dennis Miller, used here with the permission of Intel Press which holds all copyrights. It can be purchased on-line.