Author: Donald Telian, SI Guys - Guest Blogger
The way high-speed signals interact with trace impedance has changed a bit over time, making the subject worthy of our attention. Thankfully, the importance - and even mechanics - of proper trace impedance is widely understood and agreed
upon. So much so, the concept almost seems mundane – particularly against the rising importance of proper via impedance
. However, I have found that engineers can benefit by improving their trace impedance intuition. For example if my trace impedance is low, should I make my trace thinner or wider? And if I can’t do that, should I move it closer to or further from ground? And do single-ended and differential signals interact with trace impedance in the same way? Not sure? Let’s have a look.
Capacitance and Impedance Intuition
Impedance intuition is readily acquired through two simple equations. Trace impedance “Z” is directly related to trace inductance (L) and capacitance (C), or Z=sqrt(L/C). While I’ve met a few who prefer to look at things inductively, the majority of us find capacitance simpler to grasp. In the realm of PCB traces, the terms in the common approximation for Capacitance (C=εA/d) are easily transferred to trace construction and simple to visualize. In the equation, “d” is a trace’s distance to ground, “A” is the area or size of the trace (i.e., its width), and “ε” is the dielectric constant of the surrounding material. Keeping this equation in mind impedance intuition follows, allowing you to predict the
effects physical changes will have on impedance. Just keep in mind the inverse relationship between capacitance and impedance. In
other words, as “C” goes up “Z” goes down, and vice versa.
So let’s try a few examples. Say I need to make traces thinner to route through a dense area, will the impedance go up or down? In this case “A” decreases causing “C” to decrease as well, resulting in an increase in “Z” or a higher impedance. Or what if production wants to swap in some modern materials that have a lower dielectric constant #8220;ε”? Once again, capacitance goes down so impedance goes up. As both these common occurrences have raised impedance, is there something I can do in the stackup to lower impedance back to where I want it? You guessed it, manipulate “d” which is the trace’s distance to ground. Indeed, if I decrease “d” then “C” increases causing “Z” to go down. See how that works? If you keep the capacitance equation around, it will be simpler to keep an eye on maintaining trace impedance when you trade-off common PCB parameters.
Typical Trace Impedances
Taking the capacitance equation (C=εA/d) forward, we might expect trace impedance to scale inversely with dielectric constant “ε” if we hold the ratio of trace width and distance to ground constant (A/d). Figure 1 shows this is generally true. Spanning the range of common dielectric constants (on the X axis), we note that trace impedance (on the Y axis)
decreases ~linearly. The upper cluster of lines are microstrip (outer layer trace, ground on one side) impedances, varied by constant H=W (Height=Width, or d=A) values in mils. The lower cluster shows stripline (inner layer trace, grounds on both sides, hence two heights “H”) impedances, again with a constant A/d ratio.
Figure 1: How Trace Impedance Scales with Dielectric Constant
Figure 1 also reveals that microstrip traces are not as amenable to 50 Ohms. That’s not too problematic because the use of microstrip is decreasing; it is primarily used for short connections from components to vias. Long microstrip routes are avoided for a variety of reasons, such as:
- Component density leaves little room for routing on outer layers
- Fabrication parameters such as pre-preg thickness and etch angle are harder to control
- Noise radiating from outer layer traces is not shielded by ground
As serial links became the high-speed interconnect of
choice, PCB traces became predominately “differential”. In practice, signal connections now required
two routes instead of one; and that changes the impedance situation a bit. Furthermore, there are some differences in
how trace impedance interacts with differential and/or single-ended signaling
we need to be aware of.
Differential traces came into the mainstream for a number of
good reasons. If you think about it, all
signals are in a sense “differential”, because the logic level they transmit is
always referenced to something – typically “ground”. As voltage swings decreased and “ground”
became less consistent between components, PCBs, and systems, signals began to
carry their own reference – or the other side of a differential “pair”. At the same time, single-ended signals became
more fragile as the criticality and complexity of their design escalated and
their margin to “reference” eroded.
Other reasons typically cited for differential signaling are
decreases in crosstalk, power/ground rail noise, and EMI. Some of these attributes relate to the fact
that a diff-pair often couples more to itself then its ground reference and/or
neighboring signals – although some diff-pairs are implemented with wide gaps
making them uncoupled or loosely coupled. And differential pairs are certainly better for long-distance
The differential impedance of an uncoupled diff-pair is two
times the trace’s single-ended impedance, and is typically specified to be 100
Ohms or 85 Ohms. Impedance-wise, the
thing to remember is that as spacing between the pair decreases the
differential impedance also decreases. One way to think about that is to picture coupling increasing, increasing
capacitance (“d” in C=eA/d
decreasing), and hence impedance “Z” decreasing. This decrease can be substantial. For example, the differential impedance of 4
mil stripline traces with distant grounds can decrease 30 Ohms as the traces move
closer together. However in practice, a
10 Ohm decrease is more common.
PCB fabrication introduces a variety of factors that affect
trace impedance. Etch angle (the way fabricated
traces turn out to be trapezoids instead of rectangles) raises impedance
because “A” and hence “C” go down, causing “Z” to increase. Outer-layer plating (and hence etch angle)
and solder mask dielectric thicknesses vary as well – both issues causing more
change in impedances than you might think. And the thickness of copper on your signal layers (½ ounce, 1 or 2
ounce) also affects impedance, albeit to a lesser degree.
Fiberglass weave effects, fabricator re-imaging, and
pre-preg thickness variation also significantly affect impedance. These effects are discussed in more detail here
Impedance and Loss
Serial links have forced us to pay attention to high-frequency
loss in traces, while trace impedance gets set to a constant. Differential impedances typically target 100
Ohms, I’ve been amazed by how stable links perform across a wide range of trace
impedance – as long as impedance discontinuities are managed. Figure 2 shows how chip-to-chip 15 Gbps
channel performance is influenced primarily by loss, or the choice of a dielectric
material’s Dissipation factor “Df” (red=0.2, blue=0.1, green=0.002 – sometimes
called “loss tangent”). Even though the
Tx and Rx impedances are 100 Ohms, eye heights (Y axis) are shown to almost
constant against a +/- 20% tolerance in trace impedance (X axis). More impactful are material choices, which cause
a 4x (blue) to 6x (green) increase in eye heights – even without any Tx or Rx equalization. Applying 30% Tx de-emphasis improves Df=0.2
performance 3x (light red, X markers) with no material change, demonstrating
power of SerDes Equalization Settings, or SES.
Figure 2: 15 Gbps Eye Heights, Varying Trace Impedance and Dielectric Loss
To emphasize the relevance of material loss the channel used
in Figure 2 had constant impedance, as might occur in a simple chip-to-chip
connection of about 7”. As such, the
only discontinuities occurred at the chip boundaries. Note that channel impedance
discontinuities must be carefully managed
to realize Figure 2’s
immunity to trace impedance. In practice
this can be difficult, however – depending on data rate – some
discontinuities can be ignored
Though differential serial links show some immunity to trace
impedance, the relevance of trace impedance to proper voltage swings in single-ended
signaling schemes (such as DDRx) cannot be overstated. Indeed, this is the dynamic that forced us to
get good at modeling, designing and fabricating PCB traces 30 years ago. So whether you are managing discontinuities
in serial links, or buffer/trace impedance trade-offs in DDRx, a working
knowledge of trace impedance is essential; which brings us back to the importance
of understanding PCB trace impedance, in practice.
While the concept of trace impedance has been with us
throughout the digital signal integrity journey, its interaction with signaling
schemes has changed somewhat. What
hasn’t changed is the mechanics of trace inductance and capacitance, and hence
impedance. Equation-based schemes to
visualize how impedance changes against physical parameters are helpful.