Via spacing on high-performance PCBs
Steve Hageman - February 6, 2013
In the last twenty years multilayer PCBs have become nearly a must for all electronic designs. This is for several reasons:
- Higher density pins and pin count on ICs has increased the routing density of our designs.
- Twenty years ago there were no QFNs and 144-pin packages in everyday use.
- The speed at which our circuits operate has increased probably four fold.
- Twenty years ago RF was commonly defined as everything below 1 GHz; now RF is everything below 6 GHz.
These speeds and densities have driven PCB design also. Where 20 years ago we may have only used microstrip for our RF traces, today we use microstrip, co-planar waveguide and stripline in our multilayer designs .
In RF design we typically need to work with only the fundamental frequency of operation. For instance: In a 2.4-GHz RF design the goal is to have a nice 2.4-GHz sine wave on our board with low harmonics. The frequencies that we need to be concerned with are really 2.4 GHz.
In digital design, the goal is to have a nice square wave on our board. A 1-GHz digital data signal needs to be square for a good eye diagram. This means that the true operating bandwidth of these traces needs to be at least five times the fundamental frequency or 5 GHz. This is from the rule of thumb that for a good-quality digital signal you need to pass at least the 5th harmonic of that signal.
Naturally there are exceptions to these two rules, but for the majority of the signals and designs we encounter they hold true.
At 6 GHz, a wavelength on FR-4 PCB material is only about 1 inch. With the speeds and frequencies we work with today we can easily get a wavelength or more on our board, so via spacing starts to be an important question.
What is the proper via spacing for a PCB and what happens if we get it wrong?
Multilayer PCBs, especially when designed for RF, may have many layers of ground; even the signal layers typically have ground flooded on them. These grounds need to be all tied together to keep them from acting like stubs or transmission line segments themselves. Or put another way, they need to be a low impedance at all the operating frequencies of the PCB, otherwise they don't look like ground anymore - they start looking reactive to the signals on them.
Any piece of copper, if it isn't terminated in its characteristic impedance, can resonate at 1/4 of a wavelength of the frequency of the current flowing in it (and every 1/2 wavelength after that). Typically we control this by placing stitching vias around the ground planes at some interval. But what is that interval?
I've seen little FM transmitter modules operating at 100 MHz that had vias spaced 30 mils apart, and I've personally built 1-GHz RF circuits that have via spacings of 250 mils (see Figure 1). Clearly the 30-mil spacing of the FM transmitter will work, since it is way closer than 1/4 of a wavelength – but is it overkill?
Figure 1: A section of a 1-GHz PLL synthesizer used in a 1-GHz receiver. The small grey grid dots are spaced at 0.05 inches. The ground vias (yellow circles) are spaced at about 250 mils on average. This circuit operates perfectly well with this via spacing with no signs of ground impedance issues.
Years ago I heard the rule of thumb: “If you space your ground vias at 1/8 of a wavelength or less your ground plane will look like a solid ground.”
This is based on the general RF Stub Length principle: “A stub on a trace starts to become a problem as it approaches 1/8 of a wavelength.” A stub is any piece of copper that extends away from a terminated trace .
The ECL guys of the 1970s knew this well  and it is a good rule of thumb for general purpose work .
An effective stub can also form on a ground plane. On a section of copper ground plane that is terminated at both ends with ground vias but not in the middle. The impedance of that middle section can actually look very reactive as the length of the spacing between the grounding vias exceeds 1/8th of a wavelength.
On our example FR-4 PCB operating at 6 GHz, a wavelength may be calculated from the well known formula as,
Where F = MHz, λ (wavelength) = meters, Er = 4.4 (for typical FR-4 PCB material ).
In tabular form for FR-4 PCB material, 1/8 of a wavelength is approximately,
Figure 2 shows an interesting result: For example - for a small 2x2-inch FM transmitter PCB operating at 100 MHz, a single via in each corner of the board will be way less than 1/8th of a wavelength! And the board will work fine from an RF point of view!