It’s getting to the end of the year, so I thought it best to wrap up the year by addressing a common myth in PCB design that just won’t die: never using right-angle PCB traces. Among the many myths in PCB design, this is one of the most prominent myths that old-school designers still cling to.
If you read some PCB design guidelines on the internet, much is made about right-angle routing and how these sharp corners should not be used. This includes Eagle’s blog, where a particular manufacturing concern (acid traps) based on decades-old technology is cited as the reason for avoiding 90-degree trace routing. I’ve seen everyone from beginners to layout engineers with decades of experience state that 90-degree routing should be avoided at all costs. Where does this idea come from, and why is it still touted as an example of bad routing?
If you look at the objections to right-angle routing, they are often presented with no evidence or sufficient justification. These objections fall into five areas:
This is complete nonsense. In fact, if this were true, then signals would not be able to move between layers through a via. This is one of those fun facts I’ve seen a number of senior PCB design engineers overlook.
When you understand how charges are excited in a conductor, then you’ll understand how the field can propagate between two points regardless of the geometry. First, let’s look at this electrostatically. When a conductor is brought up to some potential, some charge density is then brought to the surface of the conductor. This charge density then emits an electric field, which points perpendicular to the surface of the conductor. If there is a nearby region of negative charge (such as a ground plane in a PCB), then the electric field lines from the positive charge density will converge to the region of negative charge density. This creates the well-known field patterns seen in many tutorials and simulations of crosstalk in PCBs.
If you then cause the voltage connected to the signal trace to switch polarity or oscillate in some way, this does not mean that electrons are physically moving from one end of the trace to the other. Electrons actually move a very short distance before being scattered by an atom that makes up the conductor, and yet electronic signals still propagate through a trace regardless of "bunching" or scattering.
What really happens in a conductor is that a propagating electromagnetic wave excites a localized oscillation in electric charge from positive to negative. In other words, the net charge density in the region where the wave propagates switches from positive to negative, and this travelling disturbance is a propagating electromagnetic wave.
The electric field distribution follows the PCB trace regardless of right-angle corners.
The current does not travel from one end of the trace to the other. Instead, this localized oscillation grows and dies as the wave passes, but the oscillation only exists within a region that spans the spatial extent (e.g., the wavelength) of the electromagnetic wave. For current-sensing receivers (e.g., power buffers), the input signal is only seen as an oscillating electric current very near the receiver input.
For a digital signal, you really have an infinite number of localized oscillations (i.e., at different harmonics of some fundamental frequency) that produce an apparent continuous motion of charge along an interconnect. Again, the superposition of these localized oscillations of current create what appears to be a motion of charge directly from the driver to the receiver, but charge in a conductor does not actually move in this way.
There is a miniscule shred of truth to this, although it has nothing to do with electrons bouncing off the edge of a conductor. Yes, it is true that right-angle traces create an impedance discontinuity, but it is no more severe than the impedance discontinuity that could be seen at a long via, slightly-mismatched filter/termination network, 45-degree trace, or a serpentine length matching segment. This means you should worry about designing traces with consistent geometry if you want to prevent an impedance discontinuity. You should also minimize or eliminate the use of vias on extremely high speed, low-level links.
The wall of a right-angle trace does not cause total internal reflection of electromagnetic waves back into the trace; in fact, a young student would know from basic physics that this does not happen at normal incidence. Similarly, a 45-degree trace is not required to force an electromagnetic wave to turn a corner; if this were true, then only very specific 45-degree bend pairs would allow a signal to reach a receiver in a PCB.
What actually happens? There is a slightly higher electric field density near the corners of a right-angle trace compared to the smooth wall of a 45-degree trace. This actually leads us to the third claim in this signal integrity myth…
There is a shred of truth to this claim, but this only becomes critical above certain frequencies. Most designers will state you should never route right-angle PCB traces due to the EMI that is created at the corner. This would create radiated EMI away from the surface of the board (near-field and far-field radiation), as well as crosstalk in nearby traces. Let’s address the crosstalk issue first.
Regarding crosstalk, this signal integrity problem can be seen as a signal induced through parasitic capacitance and/or inductance between nearby traces, but crosstalk would happen regardless of the presence of a right-angle corner in a PCB. Furthermore, although the field generated inside a right-angle corner in the aggressor trace will be stronger than that along a flat trace wall, the field can be concentrated at the outside corner of the victim trace. As a result, there is no appreciable effect on crosstalk in nearly all situations.
The real shred of truth can be found when we consider far-field radiation. Mathematically, there is an impedance mismatch between the edge of a right-angle PCB trace and the dielectric. Whenever you have an impedance mismatch in a structure with forward and backward propagating waves, you have reflection and the potential for standing wave resonance, similar to transmission line resonance. However, EMI only becomes severe if you can excite a standing wave resonance, or multiple resonances within a partially open structure.
Example current distribution in a right-angle trace. Image source.
The limiting factor that will determine whether any resonances are excited is the size of the square region in a right-angle PCB trace. In particular, the lateral size of the region will be approximately equal to the quarter wavelength of the lowest order resonance, so this gives you a good baseline for estimating the fundamental resonance frequencies. The remaining harmonics will be approximately odd multiples of the fundamental frequency. If we allow a very generous trace width of 30 mils with an effective dielectric constant of 3.5, the lowest order frequency is 112 GHz! If we take this as a knee frequency for a digital signal, this is equivalent to a 3 ps rise time, which is well-below that for commercially available digital components.
As of today, digital designers need not worry about right-angle PCB traces as a source of EMI. The smart RF designer should already use isolation techniques to prevent this form of EMI from inducing noise in other circuit blocks. Even designers working beyond the mmWave regime will implement sufficient isolation measures in their board, regardless of frequency.
This objection used to be valid in the 1980’s, but with newer etchant solutions used for copper etching during manufacturing, you can effectively ignore this problem unless you are working with a typical Chinese manufacturer. A few decades ago, etchant solutions tended to have higher surface tension and viscosity, causing them to accumulate and sit in the 90-degree corners in right-angle PCB traces. This would cause over-etching at corners, leading to excessive surface roughness on copper traces. Today, any American manufacturer that wants to keep their doors open knows not to use these older etchants. However, this continues to be a problem with low-quality overseas manufacturers.
Microscope image showing over-etching on some copper traces.
This is probably the least-known claim and is generally found among manufacturers, rather than designers. The high current density found near corners (see the above graph) and resulting high field is thought to produce strong electromigration. However, experimental tests by Croes et al. (see source below) found that electromigration near right-angle PCB traces was no more severe than that from standard 45-degree traces or curved traces.
There is a related, legitimate claim that should be considered, which relates to the electric field produced from right-angle PCB traces. The higher field emitted from these traces means larger creepage and clearance distances should be used in high voltage design. Because the field is higher, dielectric breakdown between two conductors is easier, thus the high voltage isolation distance between two points should be increased. This is the only legitimate objectection to right-angle PCB traces.
By now it should be clear; the problems with right-angle PCB traces are mythical and should not receive attention unless you are working at high voltage. Unfortunately, some of these design myths just won’t go away anytime soon, but we’ll be here to try and shed light on the truth.
At NWES, we help innovators understand all aspects of their most advanced technical problems. If you're looking for a cutting-edge PCB design service bureau and thought leadership marketing services, contact NWES for a consultation.