Design A Multilayer PCB , One of the important things is planning the Multilayer PCB stack-up in achieving the best possible performance of a product. A poorly designed substrate, with inappropriately selected materials, can degrade the electrical performance of signal transmission increasing emissions and crosstalk and can also make the product more
susceptible to external noise. These issues can cause intermittent operation due to
timing glitches and interference dramatically reducing the products performance and
long term reliability.
In contrast, a properly built PCB circuit board substrate can effectively reduce electromagnetic emissions, crosstalk and improve the signal integrity providing a low inductance power distribution network. And, looking from a fabrication point of view, can also improved
Manufacturability of the product.
Suppressing the noise at the source rather than trying to elevate the problems once the product has been built makes sense. Having the project completed ‘Right First Time’ on time and to budget means that you cut costs by reducing the PCB design cycle, have a shorter time to market and an extended product life cycle.
Boards containing copper planes allow signals to be routed in either microstrip or stripline controlled impedance transmission line configurations creating much less radiation than the indiscriminate traces on a two layer board. The signals are tightly coupled to the planes (either ground or power) reducing crosstalk and improving signal integrity.
Planes, in Multilayer PCB’s, provide significant reduction in radiated emission over two
layer PCBs. As a rule of thumb, a four layer board will produce 15 dB less radiation than
a Double side PCB board.
When selecting a multilayer stackup we should consider the following:
• A signal layer should always be adjacent to a plane. This limits the number of signal
layers embedded between planes to two and top and bottom (outer) layers to one
• Signal layers should be tightly coupled (<10 MIL) to their adjacent planes
• A power plane (as well as a ground) can be used for the return path of the signal.
• Determine the return path of the signals (which plane will be used). Fast rise time
signals take the path of least inductance which is normally the closest plane.
• Cost (the boss’s most important design parameter).
Soldermask – Affects on Impedance
Since Printed circuit board ’s are normally covered in Solder mask then the affects of the conformal
coating should be considered when calculating impedance. Generally, soldermask will
reduce the impedance by 2 to 3 ohms on thin traces. As the trace thickness increases
the soldermask has less affect.
Above Picture illustrates the affect of soldermask coating on microstrip impedance. This
example is of commonly used liquid photoimageable soldermask having a thickness of
0.5 MIL and a Dielectric Constant of 3.3.
The soldermask drops the microstrip characteristic impedance by 2 ohms and the
differential impedance by 3.5 ohms. So, if you don’t consider soldermask then the
calculation could be out by as much as 3 to 4%.
The most popular Dielectric material is FR4 and may be in the form of core or prepreg (pre impregnated) material.
The core material is thin dielectric (cured fibreglass epoxy resin) with copper foil bonded to
both sides. For instance: Isola’s FR406 materials – include 5, 8, 9.5, 14, 18, 21, 28, 35, 39, 47,
59 and 93 MIL cores. The copper thickness is typically ½ to 2 oz (17 to 70 um).
The prepreg material is thin sheets of fibreglass impregnated with uncured epoxy resin
which hardens when heated and pressed during the PCB fabrication process. Isola’s FR406
materials – include 1.7, 2.3, 3.9 and 7.1 MIL prepregs that may be combined to achieve the
desired prepreg thickness.
The most common stackup called the ‘Foil Method’ is to have prepreg with copper foils
bonded to the outside on the outer most layers (top and bottom) then core alternating with
prepreg throughout the substrate. An alternate stackup is called the ‘Caped Method’ which
is the opposite of the Foil Method and was used by old-school military contractors.
Let’s take a look at the most common multilayer configurations.
4 Layer PCB Stackup
A typical four layer board stackup is shown below. The Characteristic and Differential
Impedances of the substrate are calculated
It is common to see four layer boards stacked evenly. That is, four evenly spaced layers
with the planes in the centre. Although, this certainly makes the board symmetrical it
doesn’t help the EMC.
Also, another common mistake is to have the planes closely coupled in the centre with
large dielectrics between the signal layers and planes. This certainly creates good inter plane capacitance but again doesn’t help with signal integrity, crosstalk or EMC – which is why we opt for a 4 layer PCB over a two layer.
To improve the EMC performance of a four layer board, it is best to space the signal
layers as close to the planes as possible (< 10 MIL), and use a large core (~ 40 MIL)
between the power and ground plane keeping the overall thickness of the substrate to ~
62 MIL. The close trace to plane coupling will decrease the crosstalk between traces and
allow us to maintain the impedance at an acceptable value.
A good range of impedance (Zo) is from 50 to 60 ohms. Keep in mind that lower impedance
will increase the dI/dt and dramatically increase the current drawn (not good for the PDN)
and higher impedance will emit more EMI and also make the design more susceptible to
6 Layer PCB Stackup
A six layer board is basically a four layer board with two extra signal layers added
between the planes. This improves the EMI dramatically as it provides two buried layers
for high-speed signals and two surface layers for routing low speed signals.
The signal layers should be placed very close to there adjacent planes and the desired
board thickness (62 MIL) made up by the use of a thicker centre core. It is always a
compromise between trace impedance, trace width and prepreg/core thickness and it is
best to use a Rayming suggestion to provide quick ‘what if’ analysis of the possibilities.
The Rayming Stackup Planner calculates characteristic impedance plus edge coupled and
broadside coupled differential impedance. The latter for embedded dual stripline layers
only. Differential pairs are becoming common place in high speed design reducing noise
by using differential mode signalling.
8 Layer PCB Stackup
To improve EMC performance, add two more planes to the six layer stackup. It is not
recommended to have more then two adjacent signal layers between the planes as this
creates impedance discontinuities (~20 ohms difference in impedance of signal layers)
and increases crosstalk between these signal layers.
In the case below, two plane layers are added to the centre of the substrate. This allows
tight coupling between the centre planes and isolates each signal plane reducing
coupling hence crosstalk dramatically. This configuration is commonly used for high
speed signals of DDR2 and DDR3 designs where crosstalk due to tight routing is an issue.
If you are risk aversive – then this is the stackup to use
10 Layer PCB Stackup
A ten layer board should be used when six routing layers and four planes are required
and EMC is of concern.
Above demonstrates a typical 10 layer stackup. This stackup is ideal because of
the tight coupling of the signal and return planes, the shielding of the high speed signal
layers, the existence of multiple ground planes, as well as a tightly coupled
power/ground plane pair in the center of the board. High speed signals normally would
be routed on the signal layers buried between planes (layers 3-4 and 7-8 in this case).
However, care should be taken to route these signal orthogonally, with respect to each
other, to avoid coupling (crosstalk) between adjacent layers.
Twelve layers is the largest number of layers that can usually be conveniently fabricated in a
62MIL thick board. Occasionally you will see 14 to 16 layer boards fabricated as a 62MIL
thick board, but the numbers of fabricators capable of producing them are limited to those
that can produce HDI boards.
High layer count boards (ten plus) require thin dielectrics (typically 5MIL or less on a
62MIL thick board) and therefore they automatically have tight coupling between layers.
When properly stacked and routed they can meet all of our high speed requirements and
will have excellent EMC performance and signal integrity. The above twelve layer stackup
provides shielding on six of the internal layers.
14 Layer PCB Stackup
The fourteen layer stackup below is used when eight routing (signal) layers are required
plus special shield of critical nets is required. Layers 6 and 9 provide isolation for sensitive
signals while layers 3 & 4 and 11 & 12 provide shielding for high speed signals.
16 Layer PCB Stackup
A sixteen layer PCB provides ten layers of routing and is normally used for extremely
dense designs. Generally, you see 16 layer PCB’s where the routing technology used in
the EDA application doesn’t have ability to route the design to completion. “If it won’t
route – just keep adding layers”. Although this is a common saying it is not good practice.
If a board won’t route to completion then there may be a number of reasons. Poor
placement is often the course. Open routing channels, reduce the number of crossovers
in the rats nets, place vias on a 25 MIL grid to allow through routing and basically help
the router as much as possible.
There is really no limit to the number of layers that can be fabricated in a multilayer PCB
(please check the capabilities of your fabricator first though). Of course, the board thickness
increases as the layer count goes up to accommodate the minimum thickness of materials
used. Also the aspect ratio (board thickness to smallest hole diameter) has to be considered.
Generally this is 10:1 for boards thicker then 100MIL. For example, a 200 MIL thick substrate
has a minimum hole size of 20 MIL.
Determining the Layer Count
The technology rules are based on the minimum pitch of the SMT components employed
and are basically the largest trace, clearance and via allowable whilst minimising PCB
fabrication costs. Technology of 4/4 MIL (trace/clearance) and Vias of 20/8 MIL (pad/hole)
are generally required for complex high speed design incorporating ball grid arrays (BGA).
However, if you can use less demanding dimensions then this will reduce cost and improved
Once these rules have been established, calculate the stackup required for the desired
characteristic impedance (Zo) and the differential impedance (Zdiff) as per the component
datasheets. Generally, 50 ohm Zo and 100 ohm Zdiff are used. Keep in mind that lower
impedance will increase the dI/dt and dramatically increase the current drawn (not good for
the PDN) and higher impedance will emit more EMI and also make the design more
susceptible to outside interference. So, a good range of Zo is 50 – 60 ohms.
The total number of layers required for a given design is dependent on the complexity of the
design. Factors include: the number of signal nets that must break out from a BGA; the
number of power supplies required by the BGA’s; component density and package types.
Experienced designers get a feel for it after a while but a good way to check if you have
enough layers is to autoroute the board. With no tweaking, the router needs to complete at
least 85% of the routes to indicate the selected stackup is routable. You may have to re evaluate the placement a couple of times to get the best results.
How do you calculate the characteristic and differential impedance of the entire stackup
using the established design rules?
For those who are new to multilayer PCB stackup planning, standard 2 to 16 layer stackups
have been provided that are commonly used. However, you can edit, rename and save a
favourite custom stackup to use again.