The Fiber Weave Effect: Skew, Losses, and Resonance
This 16 GHz oscilloscope measurement illustrates how the fiber weave effect can impair signal integrity
Look at the cross section of a PCB substrate under a microscope with decent contrast, and you’ll see that the substrate is not a homogeneous material. PCB laminates are composed of a fiber weave structure, where a glass fabric is encased in a resin. Although the glass weave pattern repeats throughout the laminate, the material is actually inhomogeneous throughout the substrate.
The electrical properties of these materials are very different, which creates signal integrity problems involving dispersion, absorption, and changes in the effective dielectric constant along an interconnect. With lower speed signals that run with smaller clock frequencies, the skew that accumulates on an interconnect may be too small to notice, but this becomes problematic in any application that requires high data rate. Here’s what you need to know about the fiber weave effect and how you can address these problems during design and testing.
Fiber Weave Effect and Dielectric Constant
Common PCB substrates like FR4 are inhomogeneous, meaning the dielectric constant varies throughout the substrate. PCB laminates are normally a square-grid glass weave that is filled with an epoxy resin to provide rigidity. The electrical properties of these two materials are very different: the glass weave has very low loss and a dielectric constant near 6. On the other hand, the epoxy has some loss and a dielectric constant approximately 3 or less. The dielectric constant of FR4 and other substrates is normally quoted as a single measurement throughout an interconnect is essentially a length-weighted average of the glass and epoxy refractive indices.
Any fiber weave effect results from the periodic variation in the weave pattern throughout the substrate. Because of the repeated variation in the dielectric constant of the substrate material, the dielectric constant of the substrate is also anisotropic, meaning the dielectric constant seen by a signal also depends on the direction the signal travels.
If you take a look at a diagram of a substrate weave, it should become somewhat obvious how the weave affects travelling digital and analog signals. Take a look at the figure below. This image shows a schematic of the fiber weave in the substrate and two traces laid out at an angle along the substrate.
Two traces across a PCB substrate, illustrating the fiber weave effect.
The glass regions and the epoxy regions have different dielectric constants, thus the characteristic impedance of a trace will be different in each region. This will then affect all the other impedance values of the pair of traces in each region. The losses in each trace will also be different because the effective dielectric constant is different in each region.
It should be rather easy to see that the effective dielectric constant in each region is a function of the trace’s location, the angle with respect to the fiber weave direction, and the separation between weave regions. In general, a substrate with a tighter glass weave (meaning smaller pores between glass sections) will have smaller variations in the dielectric constant. The differences in effective dielectric constant along the trace produce two effects in this pair of traces:
The signals in each trace will take slightly different lengths of time to travel along this interconnect. As a result, skew will accumulate between these signals, which can take them completely out of sync. At low clock rates, the skew between these signals is generally too small to be noticed and will not be noticed as long as the traces are length matched within some tolerance. However, with channels running at 10 Gbps or higher, skew between traces can completely desynchronize parallel signals. With differential pairs, this eliminates common mode noise immunity and creates bit errors.
Impedance and Dispersion Discontinuities Along a Trace
The effective dielectric constant of a trace determines the impedance seen by a signal traveling along the trace. Because the substrate dielectric constant and losses determines the effective dielectric constant and losses in the trace, the impedance and losses in the trace also vary throughout an interconnect. These effects are minimal as long as traces are relatively short, but the more important effect that results at high data rates is signal distortion due to dispersion in your PCB substrate.
If two traces are routed in parallel along the exact same weave pattern, the two traces will experience the same total harmonic distortion due to dispersion, which eliminates the possibility of bit errors. In a practical case, this is near impossible. The resulting pulse distortion along the trace becomes noticeable at high data rates. This manifests itself as different signals in different parallel traces having slightly different ON times.
Substrate Resonance Under Periodic Loading
This particular problem was ignored by the R&D community for years. As signals are periodically injected into an interconnect and propagate along a trace, the signal is not really confined inside the conductor. A portion of the electromagnetic field bleeds into the substrate as the signal travels along a trace. This causes some portion of the electromagnetic field to remain trapped between fiber weave and epoxy regions in the substrate. The high refractive index contrast between the glass weave and the epoxy leads to relatively strong reflection, which is sufficient to cause superposition between incident and reflected waves in these substrate cavities.
This means that cavities between the glass weave and epoxy have some resonance frequency spectrum. In FR4, a glass weave pitch of 60 mils has lowest order resonance frequency (half a wavelength) of approximately 45 GHz. In other words, data transmitted at a rate of 45 GHz (not 45 Gbps, these are not always the same!) will create some resonance in the substrate around the trace that is confined between the glass and epoxy. The same can be said for analog signals. This resonance can create inductive crosstalk in another nearby trace.
High speed Ethernet cards and backplanes regularly suffer from the fiber weave effect
The complicated structure of a PCB substrate can lead to resonances at lower frequencies, depending on the trace-to-glass-weave angle; a trace running diagonal to a glass-epoxy cavity can excite a resonance with lower frequency simply due to the geometry. In addition to the impedance issue mentioned above, these resonances affect the insertion/return loss along an interconnect.
This leads to additional losses in the insertion loss profile due to repetitive signal injection at midrange data rates/clock frequencies. As data rates continue to increase we are getting closer to these GHz resonance frequencies, particularly the lowest order glass-weave cavity frequency. This is already a problem in devices that run at mmWave frequencies.
Measure the Fiber Weave Effect in Your Substrate Materials
You can anticipate these important signal integrity problems early if you measure the skew, losses, and resonances due to the fiber weave effect before beginning a new design. Some basic measurements with a test coupon can help you determine the average skew between parallel signals you would expect to see in your board. You can also determine insertion loss along an interconnect by extracting S-parameters with a vector network analyzer.
The idea is to try and determine the average insertion loss and skew as a function of trace direction and location on your desired substrate material. If you can account for the fiber weave effect early in the design phase, then you can determine the appropriate tolerances on interconnects that will help ensure these signal integrity problems do not affect the performance of your PCB.
Analyzing and compensating for the fiber weave effect in any PCB substrate can be a difficult task, but you can define any measures required for compensation as design rules and constraints when you use the right PCB design and analysis software package. Allegro PCB Designer and Cadence’s full suite of analysis tools make it easy to layout your board and simulate its performance.
If you’re looking to learn more about how Cadence has the solution for you, talk to us and our team of experts.