Subject: PCB Stack-Up - Introduction
From: "Saved by Internet Explorer 11"
Date: Thu, 2 Jul 2015 15:05:49 -0700

Henry Ott
Consultants
Electromagnetic Compatibility Consulting and
Training

PCB Stack-Up

Part 1. Introduction
PCB stack-up is
an important factor in determining the EMC performance of a product.  A
good stack-up can be very effective in reducing radiation from the loops on the
PCB (differential-mode emission), as well as the cables attached to the board
(common-mode emission).  On the other hand a poor stack-up can increase the
radiation from both of these mechanisms considerably.

Four factors are important with respect to board stack-up considerations:

1. The number of layers,
2. The number and types of planes
(power and/or ground) used,
3. The ordering or sequence of the layers,
and
4. The spacing between  the layers.
Usually not much
consideration is given except as to the number of layers.  In many cases
the other three factors are of equal importance.  Item number four is
sometimes not even known by the PCB designer.  In deciding on the number of
layers, the following should be considered:

1. The number of signals to be routed and cost,
2.
Frequency,
3. Will the product have to meet Class A or Class B emission
requirements,
4. Will the PCB be in a shielded or unshielded enclosure,
and
5. The EMC engineering expertise of the design team.
Often
only the first item is considered.  In reality all the items are of
critical importance and should be considered equally.  If an optimum design
is to be achieved in the minimum amount of time and at the lowest cost, the last
item can be especially important and should not be ignored.

Multi-layer boards using ground and/or power planes  provide significant
reduction in radiated emission over two layer PCBs.  A rule of thumb, that
is often used, is that a four-layer board will produce 15 dB less radiation than
a two-layer board, all other factors being equal.  Boards containing planes
are  much better than those without planes for the following reasons:

1. They allow signals to be routed in a microstrip (or stripline)
configuration.  These configurations are controlled impedance
transmission lines with much less radiation than the random traces used on a
two-layer board.
2. The ground plane decreases the ground impedance
(and therefore the ground noise) significantly.
Although two-layer
boards have been used successfully in unshielded enclosures at 20 to 25 MHz,
these cases are the exception rather than the rule.  Above about ten or
fifteen MHz, multi-layer boards should normally be considered.

When using multi-layer boards there are five objectives that
you should try to achieve.  They are:

1. A signal layer should always be adjacent to a plane.
2.
Signal layers should be tightly coupled (close) to their adjacent planes.

3. Power and Ground planes should be closely coupled together.
4.
High-speed signals should be routed on buried layers located between
planes.  In this way the planes can act as shields and contain the
radiation from the high-speed traces.
5. Multiple ground planes are
very advantageous, since they will lower the ground (reference plane)
impedance of the board and reduce the common-mode radiation..
Often
we are faced with the choice between close signal/plane coupling (objective #2)
and close power plane/ground plane coupling (objective #3).  With normal
PCB construction techniques, there is not sufficient inter-plane capacitance
between the adjacent power and ground planes to provide adequate decoupling
below about 500 MHz.  The decoupling, therefore, will have to be taken care
of by other means and we should usually 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.

An eight-layer board is the fewest number of layers that can be used  to
achieve all five of the above objectives.  On four and six layer board some
of the above objectives will have to be compromised.  Under those
conditions you will have to determine which objectives are the most important to
the design at hand.

The above paragraph should not be construed to mean that you can't do a good
EMC design on a four- or six-layer board, because you can.  It only
indicates that all the objectives cannot be met simultaneously and some
compromise will be necessary.  Since all the desired EMC objectives can be
met with an eight-layer board, there is no reason for using more than eight
layers other than to accommodate additional signal routing layers.

Another desirable objective, from a mechanical point of view, is to have the
cross section of the board symmetrical (or balanced) in order to prevent
warping.  For example, on an eight-layer board if layer two is a plane,
then layer seven should also be a plane.  Therefore, all the configurations
presented here use symmetrical, or balanced, construction.  If a
non-symmetrical, or unbalanced, construction is allowed additional stack-up
configurations are possible.

© 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