Printer Friendly

Quieting down a noisy problem: the ability to predict near- and far-end crosstalk per a given line spacing can make your design a success.

CROSSTALK IS THE second biggest source of noise in circuit boards, packages and connectors. It arises only from capacitive and inductive coupling, which we usually model with mutual capacitance and mutual inductance.

When the return path of a transmission line is a nice, wide, uniform plane, such as most interconnects in multilayer circuit boards, the relative contribution from the capacitive and inductive coupling is about the same, and both terms are important and must he taken into account. These two sources of noise combine to produce near-end noise and far-end noise.

When the return path is not a wide plane, but is constricted into a lead in a package or a pin in a connector, the mutual inductance can increase more than an order of magnitude and will typically dominate crosstalk noise. In this case, when mutual inductance dominates, we refer to this as switching noise. When multiple signal lines share the same return conductor, the switching noise is called ground bounce.

It is rare for ground bounce to be generated by board-level interconnects. It is typically seen only in packages and connectors. In fact, crosstalk from uniform transmission lines is one of the easiest sources of noise to design out during board layout. The most important design guide, to minimize near- and far-end noise in microstrip or stripline, is to increase the spacing between the signal lines.

But PCB designers are constantly pushing in the opposite direction. To reduce the total cost of a board, designers often use the tightest spacing between lines and the highest density possible. This will minimize the number of routing layers and keep the board footprint to a minimum. The designer is constantly battling this trade-off between the minimum, cost-effective spacing and acceptable crosstalk.

There is only one good approximation for the near-end noise in microstrip or stripline and spacing, given the impedance of the line and a few parameters. It first appeared in the National Semiconductor Application Note AN905, by James Meats. Though it is presented as the differential impedance of a microstrip or a stripline, we can modify it slightly to predict the near-end crosstalk:

For a microstrip: Kne = 0.48 x exp(-0.96 x s/h)

For a stripline: Kne = 0.37 x exp(-2.9 x s/b)


Kne = near-end crosstalk as a fraction of the signal swing

s = the spacing between the lines

h = the spacing between the signal and return plane for the microstrip

b = the total spacing between the planes for the stripline

This equation predicts that crosstalk drops off exponentially with increased spacing.

With only two exceptions, every formula used in signal integrity is either a definition or an approximation. With every approximation, the first question is, how accurate is this approximation? One way of verifying the accuracy of this approximation is by comparing the results to a 2D field solver that has been independently verified.

FIGURE 1 compares the predicted near-end crosstalk values of this approximation for three different impedance microstrip and stripline traces to the predictions of the Ansoft 2D field solver, which I have verified to better than 1% absolute accuracy.


For very tight coupling in microstrip this approximation is not too bad, but for stripline this approximation is very good. It should not be used to sign off on a design, but for a rough measure or tolerance analysis, this approximation for near-end crosstalk is good enough.

With these crosstalk results, we can also develop a simple rule of thumb for minimum spacing for acceptable crosstalk. To keep the total noise on a trace below 5%, when traces on either side switch in the same direction, we would like the near-end crosstalk to be less than about 2%. For 50 [omega] microstrip and stripline, this is achieved with a spacing equal to twice the line width.

This doesn't mean your design won't work if the spacing is closer than this; it means that crosstalk from board-level traces will never be an issue if the spacing is greater than twice the line width. If you route closer, put in the numbers before you release your artwork to fab.

DR. ERIC BOGATIN (eric@BeThe is the CTO of IDI and president of Bogatin Enterprises.
COPYRIGHT 2005 UP Media Group, Inc.
No portion of this article can be reproduced without the express written permission from the copyright holder.
Copyright 2005, Gale Group. All rights reserved. Gale Group is a Thomson Corporation Company.

Article Details
Printer friendly Cite/link Email Feedback
Title Annotation:No Myths Allowed
Author:Bogatin, Eric
Publication:Printed Circuit Design & Manufacture
Date:Jan 1, 2005
Previous Article:Services.
Next Article:A game of chance? Hardly.

Related Articles
Board stackup's important tool: for a target differential impedance, a 2D field solver, used accurately, can be a time-saver.
Deterministic jitter: by understanding the relationship between 'aggressor' line and 'victim' line bit switching, designers can keep...
Mea culpa, mea maxima culpa: even famous columnists can make the occasional error.
Tricks of the trade: a little known trick for reducing crosstalk.
Professional Development Certificate Program.
Microstrip or stripline? That is the question.
A dose of reality: do corners cause reflections? The answers to last month's puzzle may surprise you.
A sneaky noise path: one inch can make a difference.
High-speed: PCB design basics: consistency in impedance requires cooperation and coordination between the designer and the fabricator to optimize...

Terms of use | Privacy policy | Copyright © 2021 Farlex, Inc. | Feedback | For webmasters