Here is the newest version of PCBWay Multi-layer laminated structure.
A printed circuit board (pcb) mechanically supports and electrically connects electronic components using conductive tracks, pads and other features etched from copper sheets laminated onto a non-conductive substrate. pcb's can be single sided (one copper layer), double sided (two copper layers) or multi-layer. Conductor on different layers are connected with plated-through holes called vias. Advanced PCB's may contain components - capacitors, resistors or active devices - embedded in the substrate.
This Application Note details tried and proven techniques for planning high speed Multilayer PCB Stackup configurations.
Planning the multilayer PCB stackup configuration is one of the most important aspects in achieving the best possible performance of a product. A poorly designed substrate, with inappropriately 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 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 two layer board.
When 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 outside interference.
6 Layer 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 stackup calculator to provide quick ‘what if’ analysis of the possibilities.
The ICD 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.
Figure 3 - 6 Layer Stackup
8 Layer 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.
Figure 4 - 8 Layer Stackup
10 Layer Stackup
A ten layer board should be used when six routing layers and four planes are required and EMC is of concern.
Figure 5 - 10 Layer Stackup
Figure 5 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.
12 Layer Stackup
Figure 6 - 12 Layer Stackup
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 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.
Figure 7 - 14 Layer Stackup
16 Layer 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.
Figure 8 - 16 Layer Stackup
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 fabrication yield.
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 reevaluate 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?
Well this one I have made easy for you. In-Circuit Design Pty Ltd has developed a Stackup Planner. This new release builds on the familiar ease of use of the popular In-Circuit Design online Impedance Calculator that has been utilized by tens of thousands of Engineers and PCB Designers world wide since 1996.
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.
The generic stackups use default values for all variables that can be adjusted to achieve the desired Characteristic (Zo), Edge Coupled (Zdiff) and Broadside Coupled (Zdbs) Impedance. The Dielectric Constant (also called Relative Permittivity), Dielectric Thickness, Copper Thickness, Trace Width and Trace can be varied.
PCBWay, PCB prototype and Fabrication the Easy Way!
