PCB transmission line stitching vias

Do High-Speed PCB Transmission Lines Need Stitching Vias?

By

Digital designs can range in speed from very low data rates used in common serial protocols to very high data rates seen in SerDes and networking protocols. Regardless of the data rate, the main factor impacting the performance of a digital interconnect is its edge rate, which partially defines its power spectrum. Then there is the required bandwidth in the channel for a receiver to recover data from a digital bitstream. Failure to lay out and route the PCB correctly could impact any one of these areas, and one layout choice that is sometimes seen on digital transmission lines is the use of stitching vias.

Stitching vias are a common feature in PCBs generally. They are also the subject of EMI guidelines, as they are commonly cited as a shielding mechanism, particularly around the board edge. In addition, they are cited in power supply PCB layout, where the stitching vias can be used to reduce the impedance of a connection between two layers operating at high power. Because of the EMI guidelines regarding shielding of radiated emissions, they are often cited as a mechanism to reduce crosstalk, particularly in digital lines.

So the question becomes, when can you use stitching vias along a trace that is carrying a digital signal? I’ll break down why you should and should not do this.

What Are Stitching Vias?

Stitching vias are arrays of vias placed in a PCB, which are normally connected to ground. If not connected to ground, a group of stitching vias would be connected to the same net, thereby connecting copper on multiple layers. Stitching vias can also be used on power connections as mentioned above, which would increase the total current-carrying capacity of the vertical portion of the design.

On digital interconnects, stitching vias are most often invoked as a solution to crosstalk. While there is some truth to this, they also impact the channel bandwidth, which will limit the power spectrum of a signal that is allowed to reach the receiver. The thought process generally goes as follows:

  1. Stitching vias placed as an array can act like a semi-closed cavity
  2. As long as the power spectrum does not span to very high frequencies, very little radiation leaks through the vias
  3. This confines most of the power within the via-stitched region

In very fast digital systems, you would actually have differential pairs, and if used with stitching vias, this would be a differential grounded coplanar waveguide. Such an interconnect would look like the example shown below; the image shows an RX pair and TX pair originating from a transceiver and routing into an SFP connector on the left side.

 

PCB transmission line stitching vias

Differential pairs routed as coplanar waveguides into an SFP connector.

 

Here we have loosely-spaced stitching vias running along the differential pairs in microstrip configuration with pour on the top layer.

The reality is that stitching vias and the surrounding copper pour on a digital interconnect create two effects that are very important in very high speed signals:

  1. Bandwidth limiting based on the span between vias on each side of the trace
  2. Change in the trace impedance compared to the case without copper pour

Whether the interconnect actually creates a change in the intensity of crosstalk depends on the span across the vias, the distance between traces, and the via pitch along the trace. If the via pitch is not selected to have the right value with respect to the signal rise time, then the via pitch creates a semi-closed resonant cavity that increases crosstalk. Let's look at each of these effects.

Via Pitch and Crosstalk

When speaking at Altium Live a few years ago, Eric Bogatin gave a presentation on common mistakes in PCB design, particularly mistakes committed by beginners. One of these issues had to do with the idea of crosstalk suppression using stitching vias. It was here that he pointed out the relationship between via pitch and signal rise time.

When stitching vias are present on a digital trace, it is possible that the crosstalk could be higher or lower, the former of which occurs from a resonant effect. This reflects two facts about stitching vias and ground shielding in general: shielding effectiveness and resonances from propagating waves.

First, let's zoom into the differential Small Form-Factor Pluggable (SFP) connection shown above. Each of the vias in the stitching via arrangement acts like a cylindrical scatterer. When multiple vias are placed together, vector function solutions can be used to estimate the resonant frequencies that would arise within these structures. In the simplest sinusoidal (zero-order) assumption, we have the following estimates for the lowest-order eigenmodes.

 

PCB transmission line stitching vias

Simple estimates of lowest-order resonant frequencies near these vias based on half-wavelength values.

 

Obviously, these are very high-frequency values and we would only expect these with very high-frequency signals or very fast edges. All other resonant frequencies will occur at higher values. These would create spikes and dips in a differential crosstalk spectrum to another differential pair or single-ended trace.

As Bogatin pointed out, the simple way to understand a resonance for a digital signal would be based on the round-trip time between two vias, essentially forming a standing wave as we would understand in a basic physics class. Just looking at the round-trip time between two vias, the lowest order frequency that we might expect to create a strong resonance would be:

 

PCB transmission line stitching vias

 

This is why we might want to make our arrangement of stitching vias closer together—if we include them at all—as it increases the lowest-order frequency corresponding to a resonance that would couple stronger crosstalk into a victim interconnect. When the vias are put very close together, it could make that lowest-order resonance so large that the resonant frequency is outside of the channel bandwidth and essentially undetectable by the receiver.

Bandwidth Limiting

Next, there is a bandwidth-limiting effect based on the span of the vias across a trace or differential pair. The span of the stitching vias is one factor that determines the quasi-TEM propagation mode cutoff. In other words, this is the maximum frequency at which a signal can propagate in the quasi-TEM mode. Above that frequency, it will only operate in the TE or TM mode, which is useful in some cases, such as exciting specific resonant structures like antennas.

To estimate the bandwidth limit, we need to estimate when we excite the first rectangular resonance in the coplanar waveguide cross section. This would be done by taking the larger of the via span or the substrate thickness. Again, a basic estimate is to use the half-wavelength value:

 

PCB transmission line stitching vias

 

An example of this in practice is shown below for a coplanar waveguide being routed from a radar transceiver to a center-fed patch antenna. Clearly, the TEM cut-off is very high given the 5-mil thick substrate, dielectric constant (Dk = 3) and the closely spaced blind vias around the microstrip.

 

PCB transmission line stitching vias

 

In general, we can calculate the power loss into your mode as a function of the various geometric parameters and arrive at a plot such as that shown below. This power loss plot and the corresponding insertion loss plots for various via spacing geometries tell you when the TEM bandwidth ends. As we would expect, tighter via pitch and via span give higher TEM mode cut-offs potentially reaching 100 GHz or more.

 

Coplanar waveguide with ground equations

Source: Sain, Arghya, and Kathleen L. Melde. "Impact of ground via placement in grounded coplanar waveguide interconnects." IEEE Transactions on Components, Packaging and Manufacturing Technology 6, no. 1 (2015): 136-144.

 

I have cited the above paper many times, but it is a very useful paper for understanding when transmission lines on printed circuit boards stop acting like quasi-TEM lines as we understand them in theory. Eventually, they act more like a fiber optic cable in that they allow specific eigenmodes to propagate to the other end with a specific electromagnetic field distribution in the cross section.

Final Thoughts

In summary, the effect of stitching vias as shielding elements is to increase the shielding effectiveness around a microstrip, thereby reducing both crosstalk and radiated emissions. Placement of vias, specifically by selecting the right geometry, gives you the ability to engineer the interconnect bandwidth to the desired value and maintain the desired mode of propagation. The trade-off is potentially greater cost in the manufacturing process, especially when vias are closely spaced and you are forced into HDI construction. Remember that closely spaced vias essentially prohibit you from routing anywhere else on another layer when the vias are through-hole vias. Therefore, blind vias may be preferable as these will not take up space on the inner layers.

 

Whether you're designing high-speed PCBs for mil-aero embedded systems or a complex RF product, you should work with a design and development firm that can ensure your product will be reliable and manufacturable at scale. NWES helps aerospace OEMs, defense primes, and private companies in multiple industries design modern PCBs and create cutting-edge embedded technology, including power systems for high reliability applications and precision control systems. We've also partnered directly with EDA companies and advanced ITAR-compliant PCB manufacturers, and we'll make sure your next high speed digital system is fully manufacturable at scale. Contact NWES for a consultation.

 



Ready to start your next design project?



Subscribe to our updates

* indicates required



Ready to work with NWES?
Contact us today for a consultation.

Contact Us Today

Our Clients and Partners