Printer Friendly

Microstrip or stripline? That is the question.

IS IT BETTER to route signals in microstrip or stripline traces? Most designers would say "It depends."

The answer really depends upon your definition of "better." So much of the design process is balancing tradeoffs, usually between acceptable performance and on-schedule delivery with acceptable risk and lowest cost.

This is why it is so dangerous to base designs on rules. Every design is custom. Design guidelines and rules of thumb are powerful tools to help zero in on possible design options, but ultimately, as design margins tighten up, every engineer needs to become proficient with the tools required to reach the optimum custom design as quickly as possible.

All we can do is point out the pros and cons of microstrip and stripline, illustrate the tools for exploring design space and ssuggest examples so you can decide what is "better."

Obviously, fewer traces can be routed in microstrip than in a stripline multilayer board, especially if the surface is already cluttered with components. This analysis applies to a situation where we have the opportunity to route a surface trace or a stripline trace, and we wish to evaluate which path is preferred.

For performance, what's important in a signal trace? In most high-speed designs, the first-order factors are controlled impedance, crosstalk and attenuation, which influences interconnect bandwidth.

What's not on the list is EMI. While it is correct that a microstrip signal trace will radiate more than a stripline, due to the finite total inductance in the return plane, very rarely do products fail FCC certification tests because of microstrip traces. They fail because of common signals on external cables; either shielded cables or twisted pair. If you have this problem nailed and do not have a shielded enclosure but still have an EMI issue, then consider stripline over microstrip.

Most fab houses don't do a very good job of controlling the impedance of outer surface layers, but there is nothing inherent about microstrip that would make it a poor controlled impedance interconnect. It is more an issue of risk with the fab house, which can be reduced by qualifying your supplier.

One advantage of microstrip is that to achieve an impedance of 50 [ohm] in a single-ended line, the dielectric thickness is about half the line width when using FR-4. For stripline, to achieve 50 Q for a single-ended line requires a total dielectric thickness between the two reference planes of about twice the line width.

In a differential pair, the difference is even more dramatic. You can use a pair of traces with tighter coupling and thinner dielectric in microstrip than in stripline traces. For example, with .005" wide, half-ounce traces, in edge-coupled microstrip with a spacing equal to the line width, the dielectric thickness is .0035". In edge-coupled stripline, with the same traces, you can't even get as high as 100 [ohm] with a space as tight as the line width. If we go to a space twice the line width, the total dielectric thickness is .028".

Stripline traces will have very little far-end crosstalk, while microstrip can have enough to easily exceed noise budgets. This is a real issue in the decision process. If far-end noise is a problem, don't use microstrip.

But when the trace-to-trace spacing is less than twice the line width, stripline actually has more near-end noise than microstrip. For spacings larger than twice the line width, stripline has lower near-end noise.

Attenuation is subtler. For the same 100 [ohm] differential impedance pairs, with .005" wide lines, the conductor loss is almost comparable between microstrip and stripline. However, the dielectric loss is lower in microstrip than stripline for FR-4. FIGURE 1 illustrates why. Some of the field lines in microstrip are in air, where they see a Iower dissipation factor than the bulk laminate. This gives microstrip about 30% lower attenuation than stripline, which means, potentially, a higher interconnect bandwidth by 30%.

[FIGURE 1 OMITTED]

FIGURE 2 shows the attenuation per length for microstrip and stripline. Above about 1 GHz bandwidth, there is an attenuation advantage for microstrip lines.

[FIGURE 2 OMITTED]

No decision is based on one answer. There are too many factors to be balanced in the tradeoffs. PCD&M

DR. ERIC BOGATIN is the CTO at IDI, and president of Bogatin Enterprises; eric@BeTheSignal.com.
COPYRIGHT 2006 UP Media Group, Inc.
No portion of this article can be reproduced without the express written permission from the copyright holder.
Copyright 2006, Gale Group. All rights reserved. Gale Group is a Thomson Corporation Company.

 Reader Opinion

Title:

Comment:



 

Article Details
Printer friendly Cite/link Email Feedback
Title Annotation:NO MYTHS ALLOWED
Author:Bogatin, Eric
Publication:Printed Circuit Design & Manufacture
Date:Feb 1, 2006
Words:715
Previous Article:Thermal design software.
Next Article:Offshoring: friend or foe?


Related Articles
Microstrip propagation time: the difference in determining stripline and microstrip propagation time is more than a fine line.
The absolute accuracy of 2D field solvers: built product is no baseline for absolute accuracy.
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.
Length matching for high-speed differential pairs: loops and serpentines can add length to eliminate imbalance in your differential pairs.
Loading effects on transmission lines, part 1: device loading can influence critical transmission line characteristics, and the design of high-speed...
Loading effects on transmission lines, Part 2: a minimum loaded line impedance may be essential to your design.
TDR for differential pair characterization, Part 2: single-ended and differential TDR signatures encompass broad signal integrity applications.
Minimizing insertion loss: proper PCB stackup and trace geometry design are key elements in the fight to lower losses.
Noise abation: what is the true value of a guard trace?
Calculating characteristic impedance: when taking measurements or doing simulations, it's good to anticipate your results ahead of time.

Terms of use | Copyright © 2014 Farlex, Inc. | Feedback | For webmasters