Free Trials

Download a free trial to find out which Altium software best suits your needs

How to Buy

Contact your local sales office to get started on improving your design environment

Downloads

Download the latest in PCB design and EDA software

  • PCB DESIGN SOFTWARE
  • Altium Designer

    Complete Environment for Schematic + Layout

  • CircuitStudio

    Entry Level, Professional PCB Design Tool

  • CircuitMaker

    Community Based PCB Design Tool

  • NEXUS

    Agile PCB Design For Teams

  • CLOUD PLATFORM
  • Altium 365

    Connecting PCB Design to the Manufacturing Floor

  • COMPONENT MANAGEMENT
  • Altium Concord Pro

    Complete Solution for Library Management

  • Octopart

    Extensive, Easy-to-Use Component Database

  • PRODUCT EXTENSIONS
  • PDN Analyzer

    Natural and Effortless Power Distribution Network Analysis

  • See All Extensions
  • EMBEDDED
  • TASKING

    World-Renowned Technology for Embedded Systems Development

  • TRAININGS
  • Live Courses

    Learn best practices with instructional training available worldwide

  • On-Demand Courses

    Gain comprehensive knowledge without leaving your home or office

  • ONLINE VIEWER
  • Altium 365 Viewer

    View & Share electronic designs in your browser

  • Altium Designer 20

    The most powerful, modern and easy-to-use PCB design tool for professional use

    ALTIUMLIVE

    Annual PCB Design Summit

    • Forum

      Where Altium users and enthusiasts can interact with each other

    • Blog

      Our blog about things that interest us and hopefully you too

    • Ideas

      Submit ideas and vote for new features you want in Altium tools

    • Bug Crunch

      Help make the software better by submitting bugs and voting on what's important

    • Wall

      A stream of events on AltiumLive you follow by participating in or subscribing to

    • Beta Program

      Information about participating in our Beta program and getting early access to Altium tools

    All Resources

    Explore the latest content from blog posts to social media and technical white papers gathered together for your convenience

    Downloads

    Take a look at what download options are available to best suit your needs

    How to Buy

    Contact your local sales office to get started improving your design environment

    • Documentation

      The documentation area is where you can find extensive, versioned information about our software online, for free.

    • Training & Events

      View the schedule and register for training events all around the world and online

    • Design Content

      Browse our vast library of free design content including components, templates and reference designs

    • Webinars

      Attend a live webinar online or get instant access to our on demand series of webinars

    • Support

      Get your questions answered with our variety of direct support and self-service options

    • Technical Papers

      Stay up to date with the latest technology and industry trends with our complete collection of technical white papers.

    • Video Library

      Quick and to-the-point video tutorials to get you started with Altium Designer

    Analyzing Crosstalk on FIFO and DDR4 Parallel Bus Interfaces

    Zachariah Peterson
    |  September 28, 2020
    Analyzing Crosstalk on FIFO and DDR4 Parallel Bus Interfaces

    High speed buses, whether single-ended or differential, can experience any number of signal integrity problems. A primary problem created by propagating signals is crosstalk, where a signal superimposes itself on a nearby trace. For parallel nets, this is particularly problematic as it leads to data corruption in severe cases. While you could slow down the rise time of a signal, this may require lowering the data transfer rate and may be unacceptable in some applications.

    If you want to identify crosstalk on parallel buses, it can be quite difficult when the bus is quite wide. For an N-bit parallel bus, you would need to run N(N - 1) crosstalk simulations to examine crosstalk between every possible combination of victim and aggressor trace. Once you get to wide bus widths, this becomes very time-consuming without the right set of analysis tools. Typically, you only need to extract the peak crosstalk signal and compare it to your signalling specs.

    The industry-standard PCB design tools in Altium Designer® already include a post-layout simulator for examining crosstalk. Still, you can speed up crosstalk analysis in parallel buses when you use a powerful field solver. You can expedite crosstalk analysis on parallel buses and other groups of signals when you import your Altium Designer layout into Ansys SIwave®. When you can conveniently visualize crosstalk between nets in a wide parallel-to-serial interface, you can speed up your analysis and quickly correct errors in your PCB layout.

    Ansys Altium Webinar Register Now

    What Goes into Signal Integrity on Parallel Nets?

    In Identifying Near-field EMI in a PCB’s Power Distribution Network and Spotting DDR4 Impedance Violations in High Speed PCB Design, we’ve looked at the Mini PC example project in Altium Designer, and we examined near-field EMI due to a poorly-planned return path and impedance variations on DDR4 nets. As the DDR4 nets form a parallel bus (containing both differential and single-ended signals), there is also the potential for crosstalk on these nets. Another wide parallel bus with potential for cross talk between specific layers is a 32-bit wide bus routed to a FIFO-to-USB interface.

    As these groups of parallel nets form wide buses, analyzing crosstalk on every signal and extracting a peak-to-peak induced crosstalk voltage can be very time-consuming. You can certainly do this by looking at waveforms, but who wants to pick signal values off of waveforms all day?

    Instead, crosstalk on these nets can be extracted directly using the field solvers in the Crosstalk Scanner in Ansys SIwave. After your layout is finished in Altium Designer, the Ansys EDB Exporter extension can be used to transfer the design into SIwave and run simulations directly from the PCB layout data. Some of the other important signal integrity metrics that can be examined include:

    • Impedance variations on single-ended and different nets
    • Return paths for high speed signals
    • S, Y, and Z-parameter extraction on critical nets
    • Parasitic extraction on critical nets

    In this example, we’ll start by looking at single-ended crosstalk on the FIFO nets, followed by the DDR4 nets. As we’ll soon see, Ansys SIwave provides a convenient visualization that allows the victim/aggressor net pair to be identified. A potential solution for the net pair can be implemented, and the modified net can be analyzed in more detail using the post-layout simulation tools in Altium Designer.

    FIFO-to-USB Nets

    Figure 1 shows the highlighted FIFO nets on Layers 1, 5, and 7. These nets form a 32-bit wide parallel bus with single-ended source-synchronous clocking that connect to a FIFO-to-USB interface IC (U33 in the Mini PC project). Length matching has been enforced to prevent skew between the synchronous clock and the 32-bit data lines in this bus. The nets in these layers are separated by large ground planes on the intervening layers.

    32-bit parallel FIFO bus
    Figure 1: FIFO nets connected to a FIFO-to-USB interface (U33) in the Mini PC layout. The dashed lines show connections made to a 32-bit parallel FIFO bus.

    DDR4 Nets

    The Mini PC board contains two onboard 8 GB DDR4 DRAM chips running at 1866 MHz routed in fly-by topology. Byte lanes 0 and 1 are grouped together with tight routing and length matching in one area of the board, while the address lines are routed around the edge of the DDR4 modules in the typical fly-by topology. Here, we basically have two parallel buses to simulate: the address lines and the DQ/DM lines leading to each module. Figure 2 shows the address, DQ, and DM lines that will be examined in the Mini PC layout.

    DDR4 routing and crosstalk parallel bus
    Figure 2: Highlighted single-ended DDR4 nets routed to DRAM module (U15) in the Mini PC layout.

    Crosstalk Scanner Results

    After running the Crosstalk Scanner in SIwave for the parallel buses shown above, we can see precisely which net pairs exhibit the greatest crosstalk signal (NEXT and FEXT). This tool uses an idealized stimulus signal that matches the rise/fall time for the FPGA in this board. The peak-to-peak voltage can be shown in a 3D bar graph, where the net names are placed on the x and y axes to form a symmetric square matrix. The FEXT and NEXT crosstalk signals produced by a given net pair can also be visualized in the time-domain.

    Figure 3 shows the peak-to-peak crosstalk (NEXT) for the FIFO nets shown in Figure 1; only a subset of the FIFO nets leading to the FIFO-to-USB IC are shown for clarity. The peak-to-peak voltage for the induced crosstalk signal is quite large and reaches 100 mV or 8.33% of the nominal single-ended signal level (1.2 V) on these nets. This indicates relatively low isolation, particularly between the clock signal (USB3_CLK) and some nearby data nets (strongest NEXT seen USB3_D10).

    The bottom portion of Figure 3 shows the extracted crosstalk signal from USB3_D2 to USB3_D3 in the time domain. Here, we see that the FEXT signal is quite low and only reaches ~10 mV (-21 dB). In contrast, NEXT is relatively high and reaches ~100 mV.

    FIFO crosstalk parallel bus
    Figure 3: Crosstalk (NEXT) for the FIFO nets in the Mini PC layout.

    Figure 4 shows the peak-to-peak crosstalk (NEXT) for the DDR4 nets shown in Figure 2; only a subset of the nets in Figure 2 are shown for clarity. The peak-to-peak voltage for the induced crosstalk signal does not exceed 7.5 mV, or 0.625% of the nominal common-mode signal level on these single-ended nets. This equates to minimum of -22 dB isolation between address nets, which is sufficient for high-performance memory systems. The other nets in the DQ/DM section have much higher isolation. Finally, the address and DQ/DM sections are clearly separated by enough space that crosstalk is not problematic.

    DDR4 routing and crosstalk parallel bus
    Figure 4: NEXT for some single-ended DDR4 nets routed to DRAM module (U15) in the Mini PC layout.

    Because the Mini PC board is a linear time-invariant (LTI) system and the electromagnetic field does not pass through any biased nonlinear media, one would reasonably expect the system to be reciprocal, i.e., the crosstalk signal will be the same if the victim and aggressor nets are swapped. This can indeed be seen in the crosstalk results for the FIFO nets and the DDR4 nets. Because the DDR4 bus falls within the crosstalk limits found in high-performance memory systems, we can focus on potential modifications to the FIFO bus.

    Reducing Crosstalk on the FIFO Bus

    When we inspect the FIFO layout and the NEXT results, it is clear inductive crosstalk dominates in the traces in this bus. Therefore, the natural solution, in this case, is to decrease the inductance of these traces by making them wider or by bringing them closer to their reference plane. The latter option is impractical in a completed layout, especially considering the solutions proposed in our earlier blogs in this series.

    Although changing the stackup is insufficient, there is sufficient room on Layers 1, 5, and 7 to widen the traces. Spacing between traces should be maintained to prevent an increase in mutual capacitance as these traces are spread out. If we look at Figure 1, the FIFO bus should be spread out towards the right side of the image. Length matching will need to be enforced as modifications are applied to traces in the FIFO bus.

    Summary

    Crosstalk on parallel bus interfaces Altium Designer’s Mini PC example project was examined using the Crosstalk Scanner in Ansys SIwave. Specific nets in FIFO and DDR4 buses were identified for modification using a convenient crosstalk visualization, which summarizes induced crosstalk signals for pairs of aggressor and victim nets. Furthermore, the dominant crosstalk mechanism (inductive vs. capacitive) can be identified from looking at time-domain waveforms, which then helps determine some solution to implement in Altium Designer.

    Register for the joint Altium and Ansys webinar to learn more.

    By using the Ansys EDB Exporter extension in Altium Designer®, PCB designers can transfer their PCB layout into Ansys SIwave® and run multiple signal integrity and power integrity simulations. This simulation package takes data directly from your PCB layout and gives designers access to numerous 3D field solvers for time domain or frequency domain simulations and analyses.

    About Author

    About Author

    Zachariah Peterson has an extensive technical background in academia and industry. He currently provides research, design, and marketing services to electronics companies. Prior to working in the PCB industry, he taught at Portland State University. He conducted his Physics M.S. research on chemisorptive gas sensors and his Applied Physics Ph.D. research on random laser theory and stability. His background in scientific research spans topics in nanoparticle lasers, electronic and optoelectronic semiconductor devices, environmental sensing and monitoring systems, and financial analytics. His work has been published in over a dozen peer-reviewed journals and conference proceedings, and he has written hundreds of technical blogs on PCB design for a number of companies. Zachariah currently works with other companies in the electronics industry providing design, research, and marketing services. He is a member of IEEE Photonics Society, IEEE Electronics Packaging Society, and the American Physical Society, and he currently serves on the INCITS Quantum Computing Technical Advisory Committee.

    most recent articles

    Back to Home