Subject: PCB Stack-Up - Part 2
From: "Saved by Internet Explorer 11"
Date: Thu, 2 Jul 2015 15:06:07 -0700

Henry Ott
Consultants
Electromagnetic Compatibility Consulting and
Training

PCB Stack-Up

Part 2. Four-Layer Boards
The most
common four-layer board configuration is shown in Fig. 1 (power and ground
planes may be reversed). It consists of four uniformly spaced layers with
internal power and ground planes. The two external trace layers usually have
orthogonal trace routing directions.

_____________ Sig.

_____________
Ground
Figure 1

_____________ Power

_____________  Sig.

Although this configuration is significantly better than a two-layer board,
it has a few, less that ideal characteristics.  With respect to the list of
objectives in Part 1, this stack-up only satisfies objective (1).  If the
layers are equally spaced, there is a large separation between the signal layer
and the current return plane.  There is also a large separation between the
power and ground planes.  With a four-layer board we cannot correct both of
these deficiencies at the same time; therefore, we must decide which is most
important to us.  As mentioned previously, with normal PCB construction
techniques there is not sufficient inter-plane capacitance between the adjacent
power and ground planes to provide adequate decoupling.  The decoupling,
therefore, will have to be taken care of by other means and we should opt for
tight coupling between the signal and the current return plane.  The
advantages of tight coupling between the signal (trace) layers and the current
return planes will more than outweigh the disadvantage caused by the slight loss
in interplane capacitance.

Therefore, the simplest  way to improve the EMC performance of a
four-layer board is to space the signal layers as close to the planes as
possible (<0.010"), and use a large core (>0.040") between the power and
ground planes as shown in Fig. 2.  This has three advantages and few
disadvantages.  The signal loop areas are smaller and therefore produce
less differential mode radiation.  For the case of 0.005" spacing (trace
layer to plane layer),  this can amount to 10 dB or more reduction in the
trace loop radiation compared a stack-up with equally spaced layers.
Secondly, the tight coupling between the signal trace and the ground plane
reduces the plane impedance (inductance) hence reducing the common-mode
radiation from the cables connected to the board.  Thirdly, the close trace
to plane coupling will decrease the crosstalk between traces.  For a fixed
trace to trace spacing the crosstalk is proportional to the square of the trace
height.  This is one of the simplest, least costly, and most overlooked
method of reducing radiation on a four-layer PCB.  With this configuration
we have satisfied both objectives (1) and (2).

_____________ Sig.

_____________ Ground

Figure 2

_____________ Power

_____________ Sig.

What other possibilities are there for a four-layer board stack-up?
Well, we could become a little non-conventional and reverse the signal
layers and the plane layers in Fig. 2, producing the stack-up shown in Fig 3a.

_____________ Ground.

_____________ Sig.

Figure 3a

_____________ Sig.

_____________ Power

The major advantage of this stack-up is that the planes on the outer layers
provide shielding to the signal traces on the inner layers.  The
disadvantages are that the ground plane may be cut-up considerably with
component mounting pads on a high density PCB.  This can be alleviated
somewhat, by reversing the planes and placing the power plane on the component
side, and the ground plane on the other side of the board.  Secondly, some
people don't like to have an exposed power plane and thirdly, the buried signal
layers make board rework difficult if not impossible.  This stack-up
satisfies objectives (1), (2), and partially satisfies objective (4).

Two of these three problems can be alleviated with the stack-up shown in Fig.
3b, where the two outer planes are ground planes and power is routed as a trace
on the signal planes.  The power should be routed as a grid, using wide
traces, on the signal layers.  Two added advantages of this configuration
are that; (1) the two ground planes produce a much lower ground impedance and
hence less common-mode cable radiation, and (2) the two ground planes can be
stitched together around the periphery of the board to enclose all the signal
traces in a faraday cage.  From an EMC point of view this configuration, if
properly done, is the best stack-up possible with a four-layer PCB.  Now we
have satisfied objectives, (1), (2), (4), and (5) while using only a four-layer
board.

_____________ Ground.

_____________ Sig./Pwr.

Figure 3b

_____________ Sig./Pwr.

_____________ Ground

A fourth possibility, not commonly used, but one that can be made to perform
very well, is shown in Fig. 4.  This is similar to Fig  2, but with
the power plane replaced with a ground plane, and power routed as a trace on the
signal layers.

_____________ Sig./Pwr.

_____________ Ground

Figure 4

_____________ Ground

_____________ Sig./Pwr.

This stack-up overcomes the rework problem mentioned before, and still
provides for the low ground impedance as a result of two ground planes.
The planes however do not provide any shielding.  This configuration
satisfies objectives (1), (2), and (5) but not objectives (3) or (4).

So, as you can see there are more options available, than you might have
originally thought, for four layer board stack-up.  It is possible to
satisfy four of our five objectives with a four layer PCB.  The
configurations of Figures 2, 3b, and 4 all can be made to perform well from an
EMC point of view.

© 2000 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
August
5, 2002