You copied the Doc URL to your clipboard.

Overview of high-speed design

When designing a target board that will be connected to DSTREAM-PT, it is important to use good digital design practice to achieve high Signal Integrity (SI).

While many target boards already take SI into consideration for trace signals, it is also important to use the same design methodology for the debug signals. To achieve the high-data throughput that is required to debug modern target systems, DSTREAM-ST units are designed to drive their JTAG interfaces at up to 180MHz. To drive at this frequency, DSTREAM-ST units use fast output drivers with short rise-times.

Note

A target system might work perfectly when it is connected to an older or slower debug unit, but it could fail to work with DSTREAM-ST because of the faster rise-times.

There are many design rules that you can implement to ensure high SI in the debug and trace interfaces:

Note

While these rules apply to all digital signals, Arm recommends giving special attention to the clock signals, TCK, RTCK, and TRACECLK.

  • Avoid stubs

    Where possible, debug and trace signals should be point-to-point between the driver and receiver of the signal with no T-junctions or branches leading to other circuitry on the target board.

    Point-to-point signal

    For debug signals, pull-up or pull-down resistors are often required. Pull-up or pull-down resistors might create a branch or stub in the signal path. It is important to keep the stub length in the signal path as short as possible.

    Stub length

    If a signal is routed with a long stub, the signal from the driver is split two ways when it reaches the T-junction. The signal that reaches the target device initially has a lower amplitude until the other half of the signal has reflected back from the end of the stub. The reflection has the effect of creating a stepped signal at the target device. A stepped signal at the target device can cause extra false signal edges to be received.

    Long stub causing false edges

    The simplest method to avoid a long stub causing false edges is to shorten the stub length by rerouting the signal. While rerouting the signal might add length to the signal route, the reduction in stub length is much more favorable.

    Improved route with shorter stub

    Alternative methods include:

    • To prevent signal reflections affecting the incoming signal, use a buffer at T-junctions. This method is used to replicate clock signals.

    • To route a signal without stubs, use an analog switch. This method is used when a device pin has multiple functions, for example, JTAG and general I/O.

    • To deflect a larger portion of the signal away from the stub, use a resistor at the junction of the stub. This method is used when the stub leads to lower-bandwidth circuitry.

  • Ensure the continuity of return signals

    As a digital signal propagates along its route, an inverse signal travels through the adjacent plane because of the electric-field coupling between the signal and the plane. When the signal edges are short, the return signal usually follows the path of least inductance, rather than resistance. This means that the return signal flows through a path in the adjacent plane, that is as close as possible to the signal route. When the return path is interrupted, it causes distortion and some loss in the signal.

    To minimize return path issues:

    • Ensure that the return path that is adjacent to the signal is continuous with no slots or accidental voids that are caused by anti-pads.

    • When routing a signal from one layer to another, link the planes close to the signal via using a return via. If the planes are at different voltages, use a low-value capacitor to AC-couple the return path.

    • When routing signals to and from a cable connector, ensure that all of the return signals of the cable are used. Directly link the return signals or AC-couple them to ground, as necessary.

  • Minimize crosstalk

    Every signal route on a target board has some effect on nearby signal tracks because of the coupling of electric and magnetic fields between the tracks. The electric and magnetic field coupling causes small variations in the surrounding signals which, over long enough distances, can cause data corruption.

    There are several ways to minimize electric and magnetic field coupling:

    • Space the signal tracks further apart. Arm recommends to keep adjacent signals at least three times further apart than they are from the nearest plane (the 3W rule).

    • Bring the plane closer to the signals. To reduce the 3W distance that is needed between adjacent signals, use thinner laminates between the signal and plane layers.

    • Keep the signal tracks as short as possible. To cut down on routing while also reducing crosstalk, place a debug or trace connector closer to the target device.

  • Use impedance matching

    Every signal route on a target board has an effective impedance that is measured in Ohms. Effective impedance is the equivalent resistance to ground a signal experiences when it initially enters a signal route, before any reflection from the far end has occurred.

    If the different portions of a signal route have different impedances, it can cause reflections in the route. Reflections reduce the integrity of the signal.

    DSTREAM-ST is designed to work with target boards that use 50Ω signal tracks.

    Most modern PCB design tools include functionality for calculating track impedance. There are also various free resources online for calculating the impedance of the various types of PCB track.

Was this page helpful? Yes No