RE: [SI-LIST] : Plane Splits Inspection

About this list Date view Thread view Subject view Author view

From: abe riazi (ariazi@serverworks.com)
Date: Wed Nov 08 2000 - 18:26:44 PST


A section of my previous email had been deleted. The missing part is pasted below:

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 different values (i.e. 0.001uF, 0.01uF, 0.1uF) to maximize the bandwidth.

Critical lines such as clock signals can have special requirements and need for additional caps.
However, in a high density PCB it may prove difficult to exactly follow such rules when space constraints allow room for fewer capacitors.

The example of Figure 1 has focused only on voids associated with plane slots, but the copper voids due to anti-pads of vias and component through hole pins can also present adverse effects and require examination.

Regarding differential signals, the best case is of course when none of the traces cross the split, and the worst situation can arise when
only one of the pair runs over the void

To summarize, it is important to inspect a PCB database for plane discontinuities before released for fabrication, for at least two reasons:

1. When a high speed-signal crosses a split (or voids) of an adjacent plane layer a sudden change can occur in the signal AC return current path and trace impedance, accompanied by undesirable SI and EMI effects.
2. Many EDA simulation tools are incapable of accurately evaluating effects of splits on the inductive return current path.

Such visual examination involves superimposing a signal layer, a neighboring power (or ground) reference plane and a layer which shows the stiching capacitors (usually the top or bottom Silkscreen layer). The width of the gaps should be as small as manufacture-able .
When it is unavoidable for a high-speed net to cross plane discontinuities, the routing should be orthogonal (with respect to the axis of the slot) to minimize the segment length over the gap.

A final note, I have been informed by Dr. Lynne Green that in a recent PADS user conference it has been requested to add the capability of highlighting high speed nets which cross plane boundaries. Indeed, this would be a desirable feature for a routing or a simulation program!

Thank you in advance for your valuable comments.

Respectfully,

Abe Riazi
ServerWorks
2251 Lawson Lane
Santa Clara, CA 95054

-----Original Message-----
From: abe riazi [SMTP:ariazi@serverworks.com]
Sent: Wednesday, November 08, 2000 5:53 PM
To: 'si-list@silab.eng.sun.com'
Subject: [SI-LIST] : Plane Splits Inspection

 << File: figure1.gif >>
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
majordomo@silab.eng.sun.com. 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 http://www.qsl.net/wb6tpu
****


About this list Date view Thread view Subject view Author view

This archive was generated by hypermail 2b29 : Tue May 08 2001 - 14:30:00 PDT