Differential Routing

HIGH-SPEED DIGITAL DESIGN - online newsletter -
Vol. 2 Issue 30

*---------------------(QUESTION)---------------------*

DIFFERENTIAL ROUTING

Clint Lieser writes:

I've recently started my first high-speed digital design and have found your book to be extremely valuable.

I have a question regarding the routing of differential pairs such as ECL or LVDS. It has been suggested that routing differential pairs as overlapping signal traces on adjacent layers is superior to routing them as adjacent traces on the same layer.

For example, the layer stack might look like this:

        ----------------------        Ground   
                 ---                  Diff Pair +
                 ---                  Diff Pair -
        ----------------------        Ground 

I have been unable to find any literature that characterizes this geometry and was wondering if you could recommend a reference or had any comments on the subject.

Thank you,
Clint Lieser

*--------------(REPLY FROM DR. JOHNSON)--------------*

Thanks for your interest in High-Speed Digital Design.

I don't have any references to give you but I do have a couple of comments.

First, either structure can work.

Second, with either structure it's not particularly important that the lines be coupled tightly together. In fact, you couldn't achieve very tight coupling even if you tried. The coupling ratios (effectively the common-mode rejection of the structure) for typical differential lines on PCB's are only in the 20-50% range.

In contrast, for a well-balanced differential twisted pair, the coupling is 99.9%. That is, if I transmit a signal down one wire of a twisted pair, with the other wire grounded, at the far end I will receive two signals, each of half size, and having opposite polarities. This is the property called "good common-mode rejection".

To get good common-mode rejection what you need is a crosstalk coefficient of about 99.9 percent. Differential traces on a PCB won't do that. Fortunately, we don't need this property for PCB applications.

Here's a list of the reasons we normally use differential pairs on a PCB:

(1) To match to an external, balanced differential transmission medium (some kind of cabling). For this purpose, the inter-trace coupling is irrelevant. Two independent, 50-ohm traces can couple a perfectly fine signal into a 100-ohm differential transmission line. What we want in this application is to make sure that the signal is generated in a purely differential manner (no common-mode components that would radiate off the cable). Furthermore, we want to make sure that the two PCB traces have equal impedances to ground (that is, they need to be symmetrical, but not necessarily close together).

(2) To defeat ground bounce. A differential signal naturally comes with its own built-in reference voltage. The receiver of a differential signal therefore does not need to rely on its own built-in reference, which could be corrupted by ground bounce voltages internal to the receiving device. For this purpose, we need only supply the receiver with two antipodal signals, with equal delays from the driver. There is no requirement here for particularly close coupling.

(3) To reduce EMI. The radiation from one trace of a differential pair is cancelled by the radiation from the adjacent trace, resulting in a marked reduction in emissions. The cancellation is proportional to the ratio S/D where S is the trace separation, and D is the distance to the receiving antenna. If we are talking about FCC class B measurements, which are taken at a distance of 3m (117 inches), then a 1-inch separation would yield a 40-db improvement in EMI (a whopping big improvement). A 0.1 inch separation should yield 60- db. Both of these numbers are probably better than the common-mode balance between the two outputs that created the differential signal in the first place. That is, with a separation of 0.1 inch, we have balanced the signal as well as could be done given the imperfections in the source, and certainly at the 0.1-inch separation level we have probably knocked down emissions to a level far below FCC limits. For EMI purposes, a differential trace spacing of 0.1 inches is close enough to do the trick. We need not struggle to place the traces any closer than that as far as our EMI requirements are concerned.

(4) To reduce local crosstalk. Differential traces on a PCB do a poor job of this. As mentioned above, signal cancellation is a function of the ratio of the trace separation, S, to the distance, D, to the receiving antenna. For local interference (which can be very, very close), you don't get much cancellation. Whether you use differential signaling or not, the best way to improve local PCB crosstalk is to move the effected traces further away. Assuming you have solid power and ground planes, crosstalk between aggressor and victim traces falls off as the SQUARE of increasing distance. Doubling the distance cuts crosstalk to one-fourth. Cramming the two traces of a differential pair closer together helps reduce crosstalk, but you don't get the big SQUARED benefit you get from generally increasing the separation between aggressor and victim.

(5) To improve routability. Differential traces CAN be pushed really, really close together, which, if you have oodles of them, can save board area. In my opinion, the desire to save board area is the only motivation for using an unusually close spacing. Remember that once you have committed to the use of tightly packed, differential traces, you will forever be hampered by two effects: (a) you will need to compute a new trace width to compensate for the fact that the differential impedance goes down for closely spaced signals, and (b) once the signals are paired, they CANNOT be separated, or else you will mess up their impedance (unless you go back to fatter widths).

This second effect imposes a routing penalty on the side-by-side approach. It's hard to get these traces to go around obstacles without the ability to temporarily separate. The over/under format works better for long-distance complicated routing.

What do I do? Unless absolutely pressed for space, I'll choose the side-by-side format. I will set the trace separation at about 4H (which yields only 6% crosstalk, or only about 6% effect on impedance). I will instruct my layout person to keep these traces generally near each other, but permit them to separate from time to time as needed to go around obstacles. I will also insist that they be equal in length.

If you use the over/under format you should know that there is a subtle asymmetry built into this configuration. The distance from the top surface of the board down to the bottom trace is greater than for the top trace, and also any return currents associated with the bottom ground plane have to find nearby vias to provide pathways back to the top surface. The net effect is that the bottom trace has some extra delay built in at the endpoints. To minimize this problem, make sure you put a number of ground vias near the point where the signals originate.

I've heard reports of additional bottom trace delays in the range of 100 ps (in that particular design, at each end of the line, the return current had to divert about 0.16 inch out of its way, and then come back, giving a total additional delay of 0.14*2*(180 ps/inch) at each end). If 100 ps matters to you, then either put the vias closer, or don't use the over/under format.

Best regards,
Dr. Howard Johnson

To Subscribe to this HSDD Newsletter, send an email to hsdd-request@freelists.org with 'subscribe' in the subject field.

All Publications by Dr. Howard Johnson except as noted.
Signal Integrity Training Classes taught exclusively by Dr. Howard Johnson - for full schedule, see www.sigcon.com
© 1998 Signal Consulting, Inc., Dr. Howard Johnson. All rights reserved. • site map