PCB transmission line stitching vias

The Impact of Copper Roughness on Signal Integrity in PCBs

By

There is no perfect conductor in any electronic system, and that includes the copper foils used in PCBs. Copper foils have some nonzero resistance, which leads to losses in transmission lines in a PCB. The copper losses in a transmission line are determined by two factors:

  • DC resistance of the line
  • Skin effect resistance

These two factors, combined with the dielectric losses (via the loss tangent), determine the propagation loss along a high-speed or high-frequency interconnect.

Copper Roughness and Signal Integrity

Now, add some roughness to that copper. What happens to signal integrity when the copper is roughened? The roughness of copper does more than just affect the copper losses. On some laminates and in some frequency ranges, copper loss will be the dominant loss factor, and it can only be overcome with the use of smoother copper or wider traces. In this article, I’ll discuss the effects of copper roughness on signal integrity, which will apply to both digital and RF systems.

Copper Roughness as a Bandwidth Limiting Element

The major effect of all losses in a high-frequency channel, whether they are power losses or reflection losses, is to limit the bandwidth of the channel. Losses in copper are already bandwidth limiting when they dominate the loss in the channel, and roughness simply adds to the existing skin effect losses from copper. The amount of copper roughness also slightly modifies the dielectric constant seen by the signal in the PCB substrate, which should also be considered when designing traces with roughened copper.

To summarize before looking at each point, we have three effects of copper roughness on signal integrity:

  • Increased skin effect losses
  • Copper loss dominating in certain frequency ranges
  • Increased dielectric constants seen by a propagating signal

Modification of the Dielectric Constant

Modification of the dielectric constant occurs due to the infiltration of rough copper into the dielectric, as shown in the graphic below. In this graphic, the electric field is confined to a slightly smaller volume, and the change in the thickness of that region containing the electric field depends on the average roughness of the copper. This can be quantified using a 10-point roughness measurement, as shown in the associated equation.

 

Dielectric losses in microstrip lines and striplines due to copper roughness

Effects of copper roughness on dielectric losses in microstrip lines and striplines. Source: V. Dmitriev-Zdorov, B. Simonovich, and I. Kochikov.

 

Note that the modification applies to the real part of the dielectric constant and the imaginary part of the dielectric constant, the latter of which determines losses.

We have Bert Simonovich to thank for this work and for helping us quantify this modification in the dielectric constant. This means that a measurement of the dielectric constant in PCB laminate materials will be different from the true value, depending on the roughness of the test fixture used to perform the measurement. Therefore, when looking at a datasheet, the dielectric constant value you see might not have the roughness factor removed.

For trace design, this means you need to use a slightly different dielectric constant to determine the impedance. What is more important, though, is the effect on copper losses when roughness is present.

Higher Skin Effect Losses

The impact on skin effect losses can be quantified using a copper roughness factor, the value of which is dependent on frequency and the morphology of the rough copper film. There are multiple models used to describe copper roughness factors for various morphologies, and in recent years there has been increasing support for these models in many applications.

Regardless of the specific model used, these models often produce an analytical function for the roughness factor, which increases monotonically with frequency. Roughness factors can be determined through measurement or through calculation. Essentially, this means you should perform the following functional transformation on the skin effect resistance term in an impedance equation.

 

lossy transmission line impedance

 

This transformed value would then appear in the full impedance equation for a single-ended transmission line with losses as follows:

 

lossy transmission line impedance

Characteristic impedance of a transmission line with all loss terms included.

 

For a differential pair, we could now apply the usual transformation with mutual capacitance and inductance between the two traces.

 

odd-mode impedance

Odd-mode impedance of one trace in a differential transmission line.

 

From here, you can determine losses in the usual manner. If we use the common square root approximation on the propagation constant, we arrive at the simple linear approximations for dielectric and copper losses, which are commonly cited in high-speed PCB design.

 

transmission line losses

Losses on a single-ended transmission line. For differential lines, we would replace Z0 with the odd-mode impedance Z(odd) and swap the capacitance for (C + Cm), where Cm is the mutual capacitance. Note that within the capacitance is embedded the modified dielectric constant, which may be different from the datasheet value due to roughness.

 

Using these two equations, we can now determine which is the dominant loss mode in a high-speed interconnect or RF interconnect.

Dominance of Copper Loss

Losses along an interconnect in a PCB with a ground plane come from dielectric losses, which absorb energy, and copper losses, which also absorb energy. When operating with broad bandwidths reaching very high frequencies, we prefer low-loss tangents PCB laminates in order to reduce the dielectric loss. What ends up happening in mid-range frequencies is a change in the dominant loss mode from dielectric loss to copper loss.

To see what happens, take a look at the graphs below. In the first graph, we see a quantification of the dielectric loss and the rough copper loss individually in terms of their decibel contribution to total loss. As is clearly seen, on a standard FR4 laminate, the dielectric loss is comparable to the copper loss in mid-range frequencies and then quickly starts to dominate above 20 GHz, as expected.

 

Microstrip impedance equation for impedance control in PCB design

Copper versus dielectric loss for a 57 micron wide 50 Ohm microstrip on Megtron 7(G) (Dk = 4, Df = 0.01) and 1 micron copper roughness.

 

If we now switch to a low-Dk/low-loss dielectric like Megtron 7(G), we still have remnant loss due to the skin effect in copper. The next graph shows losses with the same amount of copper roughness for a 50 Ohm trace.

 

Microstrip impedance equation for impedance control in PCB design

Copper versus dielectric loss for a 65 micron wide 50 Ohm microstrip on Megtron 7(G) (Dk = 3.37, Df = 0.001) and 1 micron copper roughness.

 

It’s quite clear in the mid-range frequencies that copper loss has become the dominant loss mechanism, and this is despite widening the trace to reduce the skin effect loss. If the copper were now smooth, that would reduce the copper loss and the dielectric loss so the large difference between these two curves will persist. I’ll leave this as an exercise for the reader.

Given the square root of frequency dependence on skin effect loss and the fractional power increase in loss due to the copper roughness factor, the skin effect loss will increase slower than the dielectric loss with its linear dependence on frequency. This means that, eventually, the dielectric loss will overtake the copper loss. The effect of using a lower loss PCB laminate material is to push this crossover frequency to progressively higher values.

What Can a Designer Do?

Aside from requesting smoother copper foil and opting for microstrip circuits, copper will eventually reach the limit of its usefulness in a PCB, particularly for serial channels. Lower decay dielectrics help because they force a designer to use wider trace widths in order to hit impedance targets. But in general, we are reaching a point in 2024 where copper will continue to be the barrier to reaching higher channel bandwidth. Eventually, interconnects on PCBs may require a totally new material, such as polymer waveguides or even glass waveguides.

 

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