Signal integrity modeling, simulation and measurements can demand frequent examination of PCB databases.

During high-speed PCB design, the need frequently arises to view the PCB database for signal integrity objectives; for instance, to ensure the widths and lengths of routed traces are consistent with routing guidelines (constraints) generated via simulations. It can also prove beneficial to inspect the PCB prior to extracting the database for post-route simulations. Another occasion that necessitates careful database viewing is for identifying locations and net names of PCB test points for laboratory probing and measurements after board fabrication.

A high-speed digital design team¹ may include specialists in different fields such as logic design, product design, signal integrity, EMI, mechanical engineering and PCB design. Such a diverse and complex design environment creates the need for the SI engineer to regularly examine the PCB database at different stages (i.e., when the board is partly routed, completely routed or after fabrication).

The PCB database examples in this column employ Cadence Allegro design software, but the signal integrity concepts apply to boards produced with other PCB programs. Williams² is a good reference. It presents a listing of numerous PCB design programs. Williams uses CadSoft Eagle software for several reasons, including availability of a useful free version, relatively inexpensive upgrades, a comprehensive library, and Windows or Linux capability.

When selecting a PCB design package, ensure that the software can output Gerber files (hence, avoid programs that output only to proprietary formats or require use of a particular PCB fabricator), has extensive/expandable part library, and an efficient autorouter feature (for instance, a rip up/retry router can perform well, whereas a grid router type is usually less effective²).

Some useful information obtainable when viewing a PCB database are the stackup layer names. Figure 1 displays the name of each layer for an eight-layer board examined with the Allegro Free Physical Viewer.

Let us briefly consider the application and significance of layer names and PCB stackup in producing accurate board simulations. A modern approach to high-speed PCB design involves extensive use of EDA tools¹, modeling and simulation. One such tool is Mentor’s XTK. XTK simulations require creation of numerous files, one of which is the Global Control File (.GCF). It is composed of several sections: Design, Defaults, Control, Constants, Files, and Stack³. Figure 2 shows the Stack section of a .GCF file applicable for nominal simulation of the aforementioned eight-layer board. Stack layer names (i.e., TOP, GND1, S1, PWR1, GND2, S2, GND3, BOTTOM) in Figure 2 are the same as layer names in Figure 1. Figure 2 also contains thicknesses for each layer.

These layer thickness values needed for accurate XTK simulations are usually obtained from the board stackup diagram (or spreadsheet) as illustrated by Figure 3. Here, thickness of top and bottom (outer) layers are given as 0.70 mil (0.5 oz), which represent values before plating. The thickness of outer layers after plating can increase to ~ 2 mils. The (total) PCB thickness is about 62 mils, a standard value. Other standard PCB thicknesses are 39, 93 and 125 mils. PCB stackups are typically constructed by alternating layers of prepreg and core. Prepreg is uncured fiberglass-epoxy resin, which becomes cured (hardened) when heated and pressed. The core is a thin piece of dielectric (cured fiberglass-epoxy resin) with copper foil bonded on both sides.

Regularly, the need arises to highlight a single-ended line, a differential pair or a group of nets for various types of inspections. Allegro Free Viewer allows two ways of highlighting a net: a) temporarily, using the show element⁴, and b) permanently via the hilight command, which requires dehilight to be turned off. The shadow mode can be used to make highlighted nets stand out.

For high-speed PCBs, it is often advantageous to specify small trace widths in order to minimize board real estate⁵ and manufacturing costs. Avoid multiple vias along high-speed nets. Subsequently, single-ended (or differential) traces are examined for width, length and number of vias on the net.

A differential pair can be highlighted and inspected for imbalances⁶ that may cause electromagnetic radiation. The length difference between traces of a differential pair can demand evaluation, because achieving length matching (within a specified tolerance, such as 10 mils) can prove critical for optimum timing margins⁷, common-mode signal prevention and EMI.

Figure 4 shows a section of a high-speed differential pair, which includes pads for AC coupling capacitors. Some high-speed links such as PCI Express⁸ have AC coupling capacitors, specify using individual 0603 (or a package with smaller lead inductance) capacitors and avoid the use of capacitor packs (C-packs). Capacitor pads should be implemented symmetrically for both signal lines of the differential pair. When viewing a high-speed PCB database, it is important to ensure that such bus specifications are satisfied.

High-speed differential pairs, traces traversing reference plane splits, BGA escape regions and relative routing of adjacent signal layers are frequently inspected for SI objectives. Differential nets are often closely examined due to their prevalence and significance in high-speed PCBs. For instance, they are evaluated for length matching⁷, and other factors that can cause skew⁹. When a differential pair includes termination resistors, DC blocking capacitors, via pairs or serpentine sections, it needs to be checked that such elements are implemented symmetrically^10,11.

Sometimes a PCB design needs to be inspected for high-speed traces crossing slots¹² in a neighboring power/ground plane. An example is illustrated by Figure 5. It displays several traces close to and routed over splits in the reference planes. This may cause impedance discontinuities, crosstalk and other undesirable effects¹². Figure 5 also shows stitching capacitors aimed at reducing the adverse effects associated with high-speed traces crossing plane cutouts. This PCB database was evaluated using the Allegro Free Physical Viewer, by turning on the desired signal layer and its reference plane with other layers turned off.

The Allegro viewer can be utilized to open board files having .brd extensions. Its menu and toolbar are depicted by Figure 6. It contains file Open, several zoom features (such as Zoom Points, Fit, In, Out, Previous), Color (and visibility), Show Element, Measure, Hilight, De-hilight, Grid Toggle, Rats Toggle, and Help.

One application of the Show Element feature is to ascertain trace lengths, as illustrated by Figure 7.

The Show Element window (Figure 7) displays the total etch length, the percent and the total Manhattan lengths. The Manhattan length defines the shortest path¹³ between two ends of the connection if routed orthogonally. In addition to net length, the Show Element window can reveal other information such as trace widths and properties/electrical constraints associated with the net.

It needs to be noted, when viewing nets with series components such as a resistor or a capacitor, that the trace can have sections of different net names. For instance, a clock line with a driver U1, a series resistor R1 and a receiver U2, may have a short section (from pin of U1 to one pin of R1) with net name CLK and a long section (from the other pin of R1 to pin of U2) named CLKR. The CLK and CLKR segment lengths then need to be added for calculating the total trace length. When inspecting such multiple sectioned nets, it can also prove beneficial to review the schematic drawing of the design to gain a more clear understanding of components and topology.

The wildcard character (*) of Allegro Viewer can be utilized for various applications. For instance, it is possible to simultaneously examine a family of nets and to ascertain the min/max routed lengths for a group of traces belonging to a bus. The zoom and pan features of this software can be applied to closely inspect various PCB features including long nets.

As mentioned in Part 1, the examples in this column utilize Cadence Allegro; however, similar inspections and SI evaluations are feasible on databases produced by other PCB design programs.

Several features of BGA breakout as depicted by Figure 8 deserve appraisal. Connections between differential pairs and BGA balls, the necking down of traces, which can cause impedance discontinuities, and power delivery to the chip usually demand inspection.

It is desirable that traces routed between neighboring pins (or vias) be properly centered and to avoid routing over plane splits (and other plane voids such as anti-pads) whenever feasible.

BGA escape regions often routed in a radial¹⁴ fashion (out from the center of the land array) can produce a horizontal and a vertical slot useful for placing surface-mount decoupling capacitors on the bottom layer. It also allows superior power feed (wider power channel) to the BGA.

It is often necessary to identify test or access points for oscilloscope probing and signal measurements. Some standard¹ SI measurements include: rise/fall times, propagation delay, noise margin, timing budget, overshoot/undershoot, and crosstalk. A suitable access point for probing is often on the bottom layer underneath the BGA at a dog-bone via. A ground close to the signal pin is also needed for probing to minimize ground loops and associated inductive noise when applying oscilloscope probes¹⁵.

When the PCB stackup includes two adjacent signal layers such as dual (or broad-side-coupled) stripline structure as shown in Figure 9, it is sometimes necessary to evaluate the routing.

Figure 10 displays numerous nets belonging to two such adjacent inner layers. In certain regions, the traces of the two layers are routed parallel, and in other areas, they are orthogonal to each other.

For high-speed PCBs, it is preferable that signals on adjacent layers^16,17 be routed in an orthogonal (90 degree conductor crossing) fashion to minimize crosstalk. However, coupling would also depend on such factors as separation distance between the layers, the parallelism length, driver strength and signal edge rates. It is preferable (for diminishing crosstalk) to place the signal layers close to the reference planes, to use thin trace widths, short parallel lengths and offset the traces. The exact magnitude of crosstalk can be ascertained via modeling and simulation.

An outstanding resource for exploring additional information related to topics discussed in this column is the Signal Integrity List email reflector (SI-LIST). It is free to subscribe to the SI-LIST and the list archives are available¹⁸ for viewing. PCD&F

Dr. Abe (Abbas) Riazi is a senior staff electronic design scientist with ServerWorks (a Broadcom Company). He can be reached at ariazi@serverworks.com.

ACKNOWLEDGEMENTS

My gratitude to Richard Kuo, Greg Albers, Peter Arnold , Mark Furnace, and Suresh Vegesna for reviewing the manuscript and furnishing excellent feedback.

REFERENCES