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
  • A365 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

    Plated Through-Hole Vias in mmWave PCBs

    Zachariah Peterson
    |  December 2, 2019

    Through-hole vias in mmWave PCBs

    Should you plate your through-hole vias in mmWave PCBs?

    Recently, I received a question from a designer at a startup wondering about proper use of plated through-hole vias in mmWave PCBs. It got me thinking that I neglected to mention this point in a previous blog post, although space in these posts can be limited. This is a fair question, both when dealing with microwave/mmWave frequencies, and when working with high speed digital signals.

    At mmWave frequencies, signals can experience strong reflection and resulting transient behavior as a travelling wave interacts with a via in an interconnect. If improperly sized, a signal can be strongly reflected from a via plated through-hole via, or the signal can strongly resonate. The question regarding use of plated through-hole vias at mmWave frequencies brings up another question: the use of through-hole components at mmWave frequencies. Anyone familiar with through-holes knows that they are a simple solution for routing between layers, but they can create more problems than they solve when working at high frequencies.

    Modeling Plated Through-hole Vias in mmWave PCBs

    In some ways, plated-through hole vias on mmWave interconnects are much easier to model and understand than digital signals with comparable knee frequencies. With a typical mmWave signal, your signal bandwidth is generally smaller than a comparable digital signal, unless you are working with ultrafast pulses, such as in radio over fiber (ROF). As an example, consider 400G networking; running at this data rate requires using multiple signal lanes operating at 25 to 50 Gbps (16 or 8 lanes, respectively). Modulation schemes (PAM-4 in this case) allow more bits to be packed into a single channel, which sets the required repetition rate in a given channel to a much lower value.

    This spreads the bandwidth of high speed digital signals (e.g., with 20 ps rise time) out over about half a decade, whereas a frequency modulated mmWave signal has a much narrower bandwidth. For example, in 77 GHz FMCW automotive radar, the signal bandwidth is only 4 GHz, or only ~5% of the carrier frequency. In terms of analysis, this means you only need to consider what happens with the carrier frequency to a first order approximation.

    When modeling plated through-hole vias in mmWave PCBs, one must consider the intrinsic inductance and parasitic capacitance of a via when designing its geometry. The fact that a plated through-hole via has inductance should be obvious—you essentially have a loop of conductor—and flowing current can create a changing magnetic field in the core, which induces a back EMF. However, these vias also have some parasitic capacitance and DC resistance. The resistance can normally be ignored as it is typically much smaller than the reactance of a via, particularly at high frequencies. This means we need to treat a via in an mmWave interconnect as an LC circuit. It has some resonance frequency, and it can create an impedance discontinuity on a transmission line.

    Add to this the possibility of a via stub on an mmWave interconnect. The via stub effectively forms a closed resonator, and it will have a resonant frequency spectrum with fundamental quarter wavelength equal to the stub length, and higher order harmonics equal to odd multiples of the fundamental frequency. This effectively forms an antenna that splits off from the via in parallel. When excited at high frequency, the stub incurs some return loss, reflecting some of the incident wave back into the via barrel and along the interconnect. This creates a second source of resonance as you now have incident and reflected waves interfering with each other in the via barrel.

    Plated through-hole vias in mmWave PCBs

    Proper use of plated through-hole vias in mmWave PCBs

    If You Must Use Plated Through-holes, Make Sure They’re Properly Sized

    This should illustrate two important points in via design for mmWave interconnects and RF signal chains: proper sizing and elimination of resonance. The latter is rather easy; simply backdrill plated through-hole vias should you choose to use them. This relates to the other point regarding through-hole vias, which is the use of through-hole components. The leftover stub on a through-hole component can also act as a floating resonator at certain frequencies. It is best to use SMD passives to prevent these resonances.

    The LC resonance in a plated through-hole via is not as important as the impedance discontinuity it creates. All mmWave PCBs should use controlled impedance transmission lines with proper driver and receiver termination. I would advocate using grounded coplanar waveguides (GCPW) on the surface layer. If you must use a second layer for routing, use striplines in an inner layer, and keep these lines on the interior layer below the GPCW ground plane.

    Routing between layers with vias requires that the vias be precisely sized such that you do not create any impedance discontinuity along the interconnect. The primary cause of any impedance discontinuity in a via in a mmWave interconnect is parasitic capacitance in the circuit; at high frequency, the via impedance appears capacitive, leading to an impedance dip in a time-domain reflectometry (TDR) scan. If you can resize the via so that the capacitance is minimized, you can treat a via as an inductor out to a higher frequency range, which makes it easier to size and layout RF circuits with microstrip transmission lines.

    Impedance measurement with time domain reflectometer

    You can measure the impedance along the length of an interconnect with a time-domain reflectometry measurement

    If you use a vector network analyzer, an S-parameter measurement should show flatter insertion loss out to a higher frequency in your interconnect. This shows how losses can be reduced by properly sizing plated through-hole vias for mmWave PCBs. Other steps designers can take involve choosing a high frequency compatible laminate with low loss tangent.

    If you do plan to use through-hole vias in mmWave PCBs, you’ll need to use the right routing, stackup, and via design features. Altium Designer® gives you all these advanced RF PCB design tools and many more in a single program. You’ll have a full suite of layer stack, via, and pad design features that are ideal for any application.

    Now you can download a free trial of Altium Designer and learn more about the industry’s best layout, simulation, and production planning tools. Talk to an Altium expert today to learn more.

    About Author

    About Author

    Zachariah Peterson has an extensive technical background in academia and industry. 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 systems, and financial analytics. His work has been published in several peer-reviewed journals and conference proceedings, and he has written hundreds of technical blogs on PCB design for a number of companies.

    most recent articles

    Back to Home