Controlled impedance (stripline etc.) boards

Johnson and Graham's "High Speed Digital Design" (ISBN-0-13-395724-1) talks about this in section 5.6 - Guard Traces - on pages 201-204 in my copy.

The message is that running your traces over a solid ground plane is the way to substantially reduces cross-talk. Adding guard traces between acitve tracks already running over a ground plane roughly halves the residual cross-talk, and you can halve this again by putting lots of vias along the guard trace to tightly couple it to the ground plane.

"Lots of vias" (actually "vias at frequent intervals") is referred back to J.A.Coekin "High Speed Pulses Techniques" Pergamon Press, Oxford,

Hope this helps. I've got a pair of text books specifically covering microstrip, but they weren't a good investment - I could poke around in them if you are desperate, but I don't like my chances of coming up with anything useful.

----------- Bill Sloman, Nijmegen

Hi,

Does anyone have references for crosstalk and impedance of stripline and microstrip designs that have analog signal traces relatively close to ground strips (on the same layer as the signal traces)?

The spacing I get for the desired max level of crosstalk without this is uncomfortably large.

Thanks in advance.

Best regards, Spehro Pefhany

If it's the January issue, it's here (3.9M zip file):

But he doesn't seem to address the issue of guard traces in that article ("Quieting Down a Noisy Problem").

Best regards, Spehro Pefhany

You can probably treat the guards as being very wide, since there won't be much field on the far side of a guard trace. So just use the signal trace dimensions and the gap distance to the guard traces and pretend it's coplanar waveguide. Appcad or Txline or one of those progs will then calculate the trace impedance.

We had a crosstalk problem a while back and did a bunch of measurements to determine trace-trace capacitances among rows of parallel runs and a couple of cases with guard traces. This was slow stuff, so we were only concerned about capacitance, not full e-m coupling. On the surface of a typical multilayer with three closely-spaced traces, the effective c between the two outer traces dropped about 4:1 if the middle one was grounded, as opposed to floating or just not there.

John

Hi, Bill:-

Okay, thanks, I've found some info in "High-Speed Circuit Board Signal Integrity" (Thierauf) which suggests vias every 1/10 of a rise time in the guard trace(s). An example shows crosstalk reduced by 4:1 for the same *signal* trace spacing. References for double guard traces ("coplanar transmission line") are to (neither of which I have easy access to at the moment):

Gopinath "Losses in Coplanar Waveguides" IEEE Trans. Microwave Theory and Techniques, Vol. MTT-30, No. 7, July 1982, pp. 1101?1104.

and

Knorr "Analysis of Coupled Slots and Coplanar Strips on Dielectric Substrate" IEEE Trans. Microwave Theory and Techniques, Vol. MTT-23, No. 7, July 1975, p. 541.

If there's anything (simple) on the effect of the guard traces on the characteristic impedance, I'd really appreciate having it. This isn't picosecond stuff I'm working with.

Thanks,

Best regards, Spehro Pefhany

Hi Spehro,

The descendants of the Vikings have done research on this:

After passing through the math heavy start it gets to be more down to earth later and includes some Spice files, too.

Regards, Joerg