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.
• 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%.
Dielectric Materials
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.