Subject: PCB Stack-Up - Part 4
From: "Saved by Internet Explorer 11"
Date: Thu, 2 Jul 2015 15:06:40 -0700

Henry Ott
Consultants
Electromagnetic Compatibility Consulting and
Training

PCB Stack-Up

Part 4. Eight-Layer Boards

An eight-layer board can be used to add two more routing layers or to
improve EMC performance by adding two more planes.  Although we see
examples of both cases, I would say that the majority of eight layer board
stack-ups are used to improve EMC performance rather than add additional routing
layers.  The percentage increase in cost of an eight-layer board over a
six-layer board is less than the percentage increase in going from four to six
layers, hence making it easier to justify the cost increase for improved EMC
performance.  Therefore, most eight-layer boards (and all the ones that we
will concentrate on here) consist of four wiring layers and four planes.

An eight-layer board provides us, for the first time, the opportunity to
easily satisfy all of the five originally stated objectives.  Although
there are many stack-ups possible, we will only discuss a few of them that have
proven themselves by providing excellent EMC performance.  As stated above,
eight layers is usually used to improve the EMC performance of the board, not to
increase the number of routing layers.

An eight-layer board with six routing layers is definitely not
recommended, no matter how you decide to stack-up the layers.  If you need
six routing layers you should be using a ten-layer board.  Therefore, an
eight-layer board can be thought of as a six-layer board with optimum EMC
performance.

The basic stack-up of an eight-layer board with excellent EMC performance is
shown in Fig 9.

________________Mounting Pads/Low Freq. Signals

________________Pwr.
________________Gnd.

________________High Freq. Signals
________________High Freq.
Signals
Figure  9
________________Gnd.

________________Pwr.
________________Low Freq. Signals/Test
Pads

This configuration satisfies all the objectives listed in Part 1.
All signal layers are adjacent to planes, and all the layers are closely
coupled together.  The high-speed signals are buried between planes,
therefore the planes provide shielding to reduce the emissions from these
signals.  In addition the board uses multiple ground planes, thus
decreasing the ground impedance.

For best EMC performance and Signal Integrity, when high frequency signals
change layers (e.g., from layer 4 to 5) you should add a ground-to-ground via
between the two ground planes, near the signal via, in order to provide an
adjacent return path for the current.  See "Changing Reference Planes" in
Part 6, (Return
Path Discontinuties) for a discussion of why this is important.

The stack-up in Fig. 9 can be further improved by using some form of embedded
PCB capacitance technology (e.g. Zycon Buried Capacitanceú) for layers 2-3 and
6-7. For more information on embedded PCB capacitance technology, see our Tech Tip on
Decoupling.   This approach provides a significant improvement
in the high frequency decoupling and may allow the use of significantly fewer
discrete decoupling capacitors.

Another excellent configuration, and one of my favorite, is shown in Figure
10.  This configuration is similar to that of Fig. 7 but includes two outer
layer ground planes.  With this arrangement all routing layers are buried
between planes and are therefore shielded.

________________Ground/Mounting Pads

________________Signal(H1)
________________Gnd.

________________Signal (V1)

Figure 10

________________Signal (H2)
________________Pwr.

________________Signal (V2)

________________Ground/Mounting pads if double sided surface mount

H1 indicates the horizontal routing layer for signal 1, and V1 indicates
the vertical routing layer for signal 1.  H2 and V2 represent the same for
signal 2.   Although not commonly used this configuration also
satisfies all the five objectives presented previously, and has the added
advantage of routing orthogonal signals adjacent to the same plane. To
understand why this is important see the section on Return
Path Discontinuites.  Typical layer spacing for this configuration
might be 0.010"/0.005"/0.005"/0.20"/0.005"/0.005"/0.010"

Another possibility for an eight-layer board is to modify Fig. 10 by moving
the planes to the center as shown in Fig. 11.  This has the advantage of
having a tightly coupled power-ground plane pair at the expense of not being
able to shield the traces.

________________Signal(H1)
________________Gnd.

________________Signal (V1)

________________Gnd.

________________Pwr.
Figure 11

________________Signal (H2)
________________Gnd.

________________Signal (V2)

This is basically an
eight-layer version of Fig. 7.  It has all the advantages listed for Fig.
7,  plus a tightly coupled power-ground plane pair in the center. Typical
layer spacing for this configuration might be
0.006"/0.006"/0.015"/0.006"/0.015"/0.006"/0.006."  This configuration
satisfies objectives 1 and 2, 3, and 5, but not 4.  This is an excellent
performing configuration with good signal intergity and is often preferred over
the stack-up of Figure 10 because of the tightly coupled power/ground
planes.  One of my favorites.

The stack-up in Fig. 11 can be further improved by using some form of embedded
PCB capacitance technology (e.g. Zycon Buried Capacitanceú) for layers 4-5.

There is very little EMC advantage to use a board with more than eight
layers.  More that eight layers is usually used only when additional
layers are required for signal trace routing.  If six routing layers are
needed,  a ten-layer board should be used.

© 2002-2004 Henry W.
Ott
Henry Ott Consultants,  48 Baker Road  Livingston,  NJ
07039  (973) 992-1793

Return to
top of page.

Return to HOC home
page.

Henry Ott Consultants
48 Baker Road Livingston, NJ 07039
Phone: 973-992-1793,   FAX: 973-533-1442

September 13, 2004