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


Download the latest in PCB design and EDA software

  • Altium Designer

    Complete Environment for Schematic + Layout

  • CircuitStudio

    Entry Level, Professional PCB Design Tool

  • CircuitMaker

    Community Based PCB Design Tool


    Agile PCB Design For Teams

  • Altium 365

    Connecting PCB Design to the Manufacturing Floor

  • Altium Concord Pro

    Complete Solution for Library Management

  • Octopart

    Extensive, Easy-to-Use Component Database

  • PDN Analyzer

    Natural and Effortless Power Distribution Network Analysis

  • See All Extensions

    World-Renowned Technology for Embedded Systems Development

  • Live Courses

    Learn best practices with instructional training available worldwide

  • On-Demand Courses

    Gain comprehensive knowledge without leaving your home or office

  • 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


    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


    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

    Noise Transfer is Annoying, Learn How to Contain Crosstalk

    Lee Ritchey
    |  January 14, 2019

    The words crosstalk and coupling are used to describe the injection of electromagnetic energy from one transmission line to another running nearby. In printed circuit boards crosstalk is usually two traces running side by side in the same layer or one over the top of the other in adjacent layers. This coupled energy appears as noise on the victim trace and can cause malfunctions if the amplitude is too large. Learn how this noise is transferred from trace to trace and methods for preventing it from happening.

    For more applied applications of these concepts, click below to watch the video and learn how to calculate impedance for a single and differential transmission line in Altium Designer®.


    The words crosstalk and coupling are used to describe the injection of electromagnetic energy from one transmission line to another running nearby. In printed circuit boards crosstalk is usually two traces running side by side in the same layer or one over the top of the other in adjacent layers. This coupled energy appears as noise on the victim trace and can cause malfunctions if the amplitude is too large. This section will describe how this noise is transferred from trace to trace and methods for preventing it from happening.

    Figure 1 is a diagram showing two transmission lines traveling side by side. The upper transmission line is shown switching and the lower one is inactive. Notice that there are two waveforms along side the victim line. One is at the end of the lines where the driver is on the driven line and the other is at the opposite end or far end. Note that the waveshapes are different. The waveform at the driver end of the victim line is usually called backward cross talk or “near end cross talk”, “NEXT” and the waveform at the far end of the victim line is “forward cross talk or “far end cross talk”, “FEXT”.

    Exactly what these two waveforms wilt look like depends on what is on the four ends of the transmission lines. The possibilities are: a short circuit, a termination or an open circuit. Reference 1 at the end of this unit describes in detail how these end terminations affect the signals seen on the victim line. From that paper it will be observed that the worst case is when the far ends of both lines are open circuits and the near end of the victim line is a short circuit. That happens to be how most CMOS circuits operate. Under these conditions, the waveforms seen on the victim line will look very much like those shown in Figure 1.

    In this discussion, the analysis will be done using this “worst case” set of conditions.

    Figure 1 Two Transmission Lines Side by Side Interacting

    Figure 2 shows how the two forms of crosstalk (forward and backward) vary as the length that the two transmission lines traveling side by side grow longer. Notice that forward crosstalk increases more slowly than backward crosstalk as the coupled length gets longer   Also, notice that there comes a point where backward crosstalk does not increase with increases in coupled length. This is called the “critical length” or the length at which backward cross talk does not continue to increase or saturate.

    Forward crosstalk increases much more slowly than backward crosstalk and does not become a factor in printed circuits as the length of the parallel run is too short. This form of crosstalk was a major problem for phone companies when lines were many meters long. This section will focus on ways to control backward crosstalk.

    Figure 2. Forward and Backward Crosstalk as a Function of Coupled Length

    Methods for Controlling Backward Crosstalk with Side by Side Routing

    When transmission lines run side by side the coupling mechanism is dominated by the magnetic component of the electromagnetic field. In over and under routing the electric field will dominate.

    Several methods have been proposed for controlling backward crosstalk. Among these are:

    • Restricting length that transmission lines run side by side
    • Inserting “guard traces” between the two transmission lines
    • Rows of “ground” vias on both sides of a sensitive signal

    Restricting Length of Parallel Run

    The most method proposed for controlling crosstalk is to limit the length that two transmission lines run side by side. There are even routines in several PCB routers that allow the to insert a length number and allow the routing tool to prevent routing longer than this amount. For this method to work, this length must be less than the critical length shown in Figure 2. If the length of a parallel run reaches the critical length it can be seen that continuing to run parallel beyond that point does not result in increased crosstalk. Figure 3 is a plot of critical length as a function of signal rise time. There are three curves on the graph corresponding to three different dielectric constants (er). two corresponds to Teflon, three corresponds to most ribbon cables and four corresponds to most dielectrics found in PCBs.

    As can be seen, as rise times get faster the critical length gets shorter. With a rise time of 1.4 nSec, the critical length is about 6 inches or 15 cm. If the router were set to allow three inches of parallel run, it would be possible to make most of the connections in most designs without running out of board space or layers. Unfortunately, very few modern integrated circuits are that slow. Currently, rise times as fast as 100 picoseconds are very . Looking at Figure 3, it can be seen that critical length at 100 picoseconds is less than half an inch or about 1.5 cm. At these rise times, length control will not work. This has been well known in the supercomputer industry for a very long time and has not been the method used to control backward crosstalk.

    Figure 3. Critical Length as a Function of Signal Rise Time

    If length control for limiting crosstalk does not  work, what method does work?

    Referring back to Figure 2, it can be seen that once critical length has been reached, continuing to route parallel does not result in additional crosstalk. At this point there are only two parameters that affect the amount of cross talk. These are height to the nearest plane and edge-to-edge separation. Figure 4 is a graph showing how cross talks varies with height above the nearest plane and edge-to-edge separation once critical length has been reached.


    Figure 4. Backward Crosstalk as a Function of Height Above Plane and Separation, Stripline

    Figure 4 is titled “Offcenter” Stripline. This means that the transmission lines are between two planes but are not centered between the two planes. This is typical of PCBs that have two signal layers between a pair of planes. Notice that crosstalk decreases substantially as the height above the nearest plane is reduced. It also decreases even more rapidly as the traces are moved apart from each other. Figure 5 is a plot showing these values for micro-stripline, signal layers that are on the outside of a PCB.

    Figure 5. Backward Crosstalk as a Function of Height Above Plane and Separation, Micro-stripline

    Guard Traces

    Many rules of thumb have recommended inserting “guard traces” between transmission lines as a method for controlling crosstalk. If this works, why does it work? And if it works is there any downside to using this method?  The “standard practice” in many companies is to route with 5 mil line and 5 mils spaces. Referring to Figure 4, if a PCB were routed to these rules and the height above the nearest plane was 5 mils (also ) the crosstalk would be about 8%. If this were determined to be excessive and a guard trace were added, what would that involve?  To make room for the guard trace a 5 mil space and a 5 mil trace need to be added. Now, the edge to edge separations is 15 mils instead of 5 mils and the crosstalk is less than 1%. It was not the guard trace that caused this decrease. It was the separation.

    Downsides to adding guard traces are: This makes routing much more difficult. The guard trade is not a barrier. It is a resonant circuit that may enhance crosstalk by creating a band pass filter.

    The proper method for controlling crosstalk in side-by-side routing is separation only.

    Rows of “Ground” Vias

    On method proposed by some applications notes and gurus is to place “ground” vias on both sides of a “critical” trace to protect a sensitive transmission line. This sort of rule is not accompanied by any proof that it is valid. It is also accompanied with vague answers when asked how many vias to use  and at what spacing. If it were useful and necessary, none of the servers and routers we design every day would be possible as there would not be enough room for all of those vias. This is a bogus rule and should not be used. An overriding observation is that valid design rules have straight forward proofs. This one does not.

    Methods for Controlling Backward Crosstalk with Over-Under Routing

    When over and under routing is done, where one transmission line is in one layer and the other is in the layer above or below, coupling is dominated by the electric field much as if a small capacitor had been connected between the two transmission lines. The coupled waveforms have that appearance. With the fast edges of modern logic, the amount of energy coupled grows so fast with the overlap between two traces that it exceeds allowable limits with very short runs.

    The only safe way to control cross talk with adjacent signal layers is by routing traces in one layer in the X direction and in the other layer in the Y direction. Most PCB layout systems have the ability to specify one layer as X and the other as Y to prevent this kind of overlap. Unfortunately, many of them will violate this constraint from time to time, so a needs to double check after routing to ensure that this rule has been followed.


    Calculating Crosstalk

    There are many rules of thumb circulating on how to space traces to control crosstalk. Among these are: three times the height above the nearest plane; two times the trace width and four times the trace width. These sound a bit arbitrary and they are. In order to determine what the spacing needs to be the first question that needs to be answered is how much crosstalk noise is acceptable?  This depends on several things including is the victim trace running next to another trace with a much higher amplitude or is it running alongside another trace with the same amplitude signal.

    Determining How Much Noise is Acceptable

    In reference 2 at the end of this section there is a chapter on design rule creation using noise margin analysis. In this section it shows that the noise budget of a logic family is consumed by several noise sources. For CMOS there are four primary noise sources. These are: crosstalk, reflections, ripple on Vdd and Vdd and ground bounce in the IC packages. Once the amount of noise from the last three is calculated this is subtracted from the noise margin of the logic family to arrive at the amount of crosstalk that can be tolerated.

    An Analytical Method for Determining Crosstalk

    There are analytical tools that allow one to calculate the crosstalk that will result from a proposed geometry between two transmission lines. Figure 6 is a screen shot in Hyperlynx® of a pair of transmission lines that will be used to calculate crosstalk for a proposed geometry. It is two CMOS circuits with the upper one active and the lower one set at a logic 0.

    Figure 6. Circuit Diagram used to Calculate Crosstalk

    Figure 7 is a screen showing how the separation between traces is specified as well as the trace width and height above the plane. It should be noted that trace width has no bearing on crosstalk, only edge-to-edge separation and height above the nearest plane are involved once transmission lines have been routed beyond the “critical length”.

    Figure 7. Screen Showing Geometry of Coupled Pair in Figure 6

    Figure 8 is a set of waveforms that result when the driven line switches from a logic 1 to a logic 0. The red waveform is the signal at the driver on the driven line and the purple waveform is the signal at the receiver on the driven line. The flat yellow line is the output of the victim line which is at a logic 0 and the waveform with the bump on it is the receiver end of the victim line.

    Figure 8. Waveforms When Driven Line in Figure 6 Switches

    The noise on the victim line appears at the “forward’ or receiver end of the victim line and does not seem to be backward crosstalk which should appear at the “backward” end of the victim line. The reason for this is the driven end of the victim line is a logic 0 which is a short circuit. From the section on transmission lines it was observed that short circuits do not absorb energy. Instead, they reflect it as an inverted waveform as has been shown in Figure 8. The second observation in the transmission line section is that open circuits also do not absorb the energy but reflect it back doubled, as is the case in Figure 8.

    The crosstalk amplitude in Figure 8 is about 1 volt on a 3.3 volt signal line. This is clearly too large. The solution is to return to the screen where height and spacing are set and adjust one or both until the crosstalk that results is within the design window. Once this analysis has been done, the crosstalk rules that result will be precise and not the result of some arbitrary rule of thumb.


    • “90 Degree Corners, The Final Turn” Doug Brooks, etal, Printed Circuit Design, January 1998.
    • SIGNAL INTEGRITY- SIMPLIFIED, Eric Bogatin, Prentice Hall, 2004.
    • “Reflections and Crosstalk in Logic Circuit Connections,” John A DeFalco, IEEE Spectrum, July 1970.
    • “Right the First Time, a Practical Handbook on High Speed PCB and System Design, Volumes 1 & 2,” Zasio and Ritchey, Speeding Edge 2003 and 2006.

    Altium is a top-notch PCB design software platform that gives you all the tools you need to design the best circuit boards. Click on the free trial to try it for yourself or watch the OnTrack Podcast episode with guest Lee Ritchey below.


    Sign up and try Altium 19 today.

    About Author

    About Author

    Lee Ritchey is considered to be one of the industry’s premier authorities on high-speed PCB and system design. He is the founder and president of Speeding Edge, an engineering consulting and training company. He conducts on-site private training courses for high technology companies and also teaches courses through Speeding Edge and its partner companies. In addition, Lee provides consulting services to top manufacturers of many different types of technology products including Internet, server, video display and camera tracking/scanning products. He is currently involved in characterizing materials for ultra high speed data links used throughout the Internet.
    Prior to founding Speeding Edge, Ritchey held a number of hardware engineering management positions including Program Manager for 3Com Corporation in Santa Clara and Engineering Manager for Maxtor. Previously, he was co-founder and vice president of engineering and marketing for Shared Resources, a design services company specializing in the design of high-end supercomputer, workstation and imaging products. Earlier in his career, he designed RF and microwave components for the NASA Apollo space program and other space platforms. Ritchey holds a B.S.E.E. degree from California State University, Sacramento where he graduated as outstanding senior. In 2004, Ritchey contributed a column, “PCB Perspectives” which appeared on a monthly basis in the industry-renowned trade publication, EE Times.

    most recent articles

    Back to Home