RE: [SI-LIST] : Plane Splits Inspection

About this list Date view Thread view Subject view Author view

From: Zabinski, Patrick J. ([email protected])
Date: Thu Nov 09 2000 - 05:41:30 PST


In the general sense, I agree with your comments. However, I
have found exceptions.

As an example, if your board cross section looks something like:

      --- Microstrip
 -------------- Split Plane

then the statements you make below are true.

However, through empirical experimentation, we have found that
many of the issues you discuss (crosstalk, discontinuity, etc.)
can be drastically reduced. By inserting a solid plane under the
split plane, like:

      --- Microstrip
 -------------- Split Plane
                 "Thin" dielectric
 -------------- Solid Plane

we have noticed dramatic improvements in performance. We have not
taken our studies to the point of being able to engineer the
effects of the solid plane, but by inserting a solid plane under the
splits, much of what you discuss is no longer an issue (we did not
test for EMI, but I suspect it improves as well).

You also mention the stitching capacitors. We have found them to
be useful. However, what I did not predict is the frequency
(spacing) in which you must place them. Using one test board,
we placed an ideal stitching capacitor (shorting bar) across the split,
and slid the capacitor along the split. We then injected signals
of various edge rates ranging from 35 psec to 1 nsec. Prior
to making the measurements, I predicted that there would be
a relationship between the edge rate and how far the cap could be
away from the trace. What I found was that the regardless of
edge rate, the stitching cap needed to be within 2 mm of the
trace! This was quite unexpected.

Most members of this list should be well aware of the potential
issues associated with splits (it's been discussed SEVERAL
times), but it does seem like we haven't quite explored
the entire issue quite yet.


> Dear Scholars:
> It is well known that when a high-speed signal crosses a slot
> of an adjacent reference Ground or Power plane, several
> undesirable effects can occur. For instance, a disturbance of
> return current path takes place which can cause a glitch,
> increased crosstalk and EMI radiation. The rule that routing
> of high-speed nets over voids or cuts of neighboring plane
> layers must be avoided is firmly established in the SI
> literature. Yet, the complexity of modern high speed designs
> imposes many violations of above guideline.
> To make matters more complicated, many simulation programs
> assume continuous Ground and Power planes and do not
> accurately take into account effects of plane discontinuities
> on the return current path. It is therefore, important to
> visually inspect a PCB database for the signals crossing
> plane slots (and voids), before generating the Gerber files
> and releasing the design for fabrication.
> Figure 1 illustrates several concepts associated with such
> examination. A section of a power plane is shown having gap G
> (due to presence of multiple powers) and several traces (T1,
> T2, T3 and T4) of an adjacent signal layer which are routed
> over the splits. C1 and C2 represent two stiching
> capacitors. In this example the gap width is 20 mils.
> Smaller widths (such as 10 mils) can be preferable since the
> break should be as narrow as feasible. Majority of crossings
> occurs at 90 degree angle with respect to axes of slot in
> order to minimize the segment length over the void. Some of
> the traces contain serpentines but are routed to pass
> boundaries only once. Stiching capacitors are utilized to
> minimize undesirable effects of the cuts.
> Certain rules of thumb have been formulated for determination
> of the required number and values of stiching capacitors; an
> example follows:
> For every five traces which cross a plane slot, insert
> approximately one or more capacitors within each 0.250 in.
> 0.01uF is an acceptable value for "stiching" capacitors,
> though it is preferable to mix several
> 2251 Lawson Lane
> Santa Clara, CA 95054

**** To unsubscribe from si-list or si-list-digest: send e-mail to
[email protected] In the BODY of message put: UNSUBSCRIBE
si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
si-list archives are accessible at

About this list Date view Thread view Subject view Author view

This archive was generated by hypermail 2b29 : Tue May 08 2001 - 14:30:01 PDT