4-layer PCB stackup

List of 4-Layer PCB Stackups and Their Applications

By

The most common types of PCBs used in commercial products are 2-layer and 4-layer PCBs. When there are digital interfaces present on the board, the best option is almost always a 4-layer PCB. The same could be said for various types of mixed-signal PCBs, RF PCBs, and even PCBs used in power electronics. The additional layers provide several advantages, namely the inclusion of ground, but today the cost of 4-layer PCBs does not create a budgetary obstacle that outweighs the advantages of the internal layers.

Despite 4-layer PCB stackups being the ideal entry level stackup for a new product, many designers still perceive these as being too difficult or too expensive for use in their products. This is especially true for hobbyists, students, young professionals, and even some startups. In this article, I will focus on outlining some of the important applications of four layer PCBs, and specifically, I will outline the common uses of 4-layer PCBs and link to some important applications.

The Common 4-Layer PCB Stackups

There are three common PCB stackups that use four layers. All of these take advantage of ground in one or more layers, which is intended to support digital signals, including high-speed signals. These 4-layer stackups are:

  • (SIG & PWR) / GND / GND / (SIG & PWR)
  • GND / (SIG & PWR) / (SIG & PWR) / GND
  • SIG / GND / PWR / SIG

There are also some variations on these stackups, which can actually be quite advantageous in some applications. Some of the variations I have seen include:

  • SIG / GND / PWR / GND
  • GND / (SIG & PWR) / SIG / GND
  • GND / SIG / PWR / GND

These options all vary the placement of power and signal around two ground planes somewhere else in the PCB stackup.

There is no single 4-layer stackup that is required for every product; some products will function correctly on any of these stackups.But to be sure you are linking the right stack of the right design application, take a look at the guidelines below to see how each of these might be used.

(SIG & PWR) / GND / GND / (SIG & PWR) and GND / (SIG & PWR) / (SIG & PWR) / GND

Primary use: Digital PCBs with high-speed signals on both SIG layers

I'll address these 4-layer stackups first because they are essentially inversions of each other. The main reason we would want to use (SIG & PWR) / GND / GND / (SIG & PWR) is to have ground planes adjacent to both signal layers. This is the ideal situation for high-speed PCBs with fast single ended signals, and it is beneficial for EMI control. The presence of ground near the signals ensures there is always a return path adjacent to digital signals on the top and bottom layer.

 

4-layer PCB stackup Altium

This 4-layer stackup can use INT1 and INT2 as GND in the (SIG & PWR) / GND / GND / (SIG & PWR) arrangement.

 

If you calculate the impedance of single-ended traces with signal on the top and bottom layers, you would find that the trace width required for 50 Ohms is 10 mils. you could then use 8 mils linewidth and 10 mils spacing for your differential pairs to get to 100 Ohms differential impedance. These values would be sufficient trace widths and settings for most commercial applications, including any RF components. The remaining space on the SIG layers can be filled in with power routing.

The inverse of this stack-up, the GND/(SIG & PWR)/(SIG & PWR)/GND arrangement, essentially performs the same functions. We would prefer to use this when cost is a factor, such as when we want to reduce the cost of the laminate by using a thicker dielectric. The 6 mil thin dielectric in the above example is not exceedingly expensive, but a thicker dielectric on the outside of the stack-up could offer a cost reduction. If thickening the dielectric on the outside makes your controlled impedance traces too wide, then you can put the traces on the inner layers and place ground on the outer layers. Watch out for crosstalk with traces on the inner layers and prefer to route orthogonally in this case.

SIG / GND / PWR / SIG

Primary use: Power electronics with a small digital section

This version of a 4-layer PCB stackup is best used in power system designs. The use of a power plane allows for high current to be routed anywhere on the PCB. it could also be broken up into multiple rails, which could then power other components at lower voltages and lower current. The SIG layer on the surface of the stackup can be used for digital signals. It is preferable that this board keep the digital signals only on the top layer, while slower configuration signals could be used on the bottom layer.

 

4-layer PCB stackup Altium

This 4-layer stackup uses PWR in an internal layer instead of two GND layers.

 

Due to the challenges in maintaining ground close to the PWR layer, it is possible that this stackup creates challenges with EMC. Sometimes, it will be possible to get around this with copper pour on the bottom layer (or rather, adjacent to PWR). This is also where a designer will start using a different type of stackup, such as that listed in the group of less common 4-layer stackups.

Alternative 4-Layer PCBs

The alternative 4-layer stackups listed below all implement some kind of swap with power and ground. The idea is to overcome the EMC-related disadvantages of the SIG / GND / PWR / SIG stackup. To this end, you’re essentially adding ground around power or signal, basically creating coplanar routing everywhere. The need to balance copper pour everywhere causes the PCB layout to look similar to what I show below.

 

4-layer PCB stackup Altium

GND is not required on the top layer in this example, but it is included in order to balance all the other layers in this SIG / GND / PWR / GND.

 

Some justifications I have seen for these alternative 4-layer PCB stackups include:

  • SIG / GND / PWR / GND: GND on layer 4 provides additional noise suppression, such as if switching node for a power regulator is on layer 3.
  • GND / (SIG & PWR) / SIG / GND: This confines all signals internally in the PCB stackup and can be used to dedicate some internal board space to power. I would not prefer this for high-speed digital PCBs, but ratther for power systems that need enhanced control of EMI.
  • GND / SIG / PWR / GND: This is very similar to the above but would provide much higher power handling at one voltage, or availability for many rails at different voltages, thanks to the dedicated power layer.

In all of these internal trace routing schemes, you still have signals close to a ground plane, so you have the benefits of the inherent shielding of the ground plane. This aids protection against crosstalk, EMI susceptibility, radiated emissions, and allows for impedance control if needed. For some mixed-signal applications, such as mixing of digital, power, and analog interfaces into the same board, these alternatives can be quite useful and they should not be eliminated just because they are not intended for high-I/O count high-speed PCB design.

 

Whether you're designing high-speed PCBs for mil-aero embedded systems or a complex RF product, you should work with a design and development firm that can ensure your product will be reliable and manufacturable at scale. NWES helps aerospace OEMs, defense primes, and private companies in multiple industries design modern PCBs and create cutting-edge embedded technology, including power systems for high reliability applications and precision control systems. We've also partnered directly with EDA companies and advanced ITAR-compliant PCB manufacturers, and we'll make sure your design is fully manufacturable at scale. Contact NWES for a consultation.

 



Ready to start your next design project?



Subscribe to our updates

* indicates required



Ready to work with NWES?
Contact us today for a consultation.

Contact Us Today

Our Clients and Partners