PCB Layer Stack Up

Layers Stack Up
A typical 4 Layer Stackup looks as follows 

Signal 1 
Ground 
Power 
Signal 2 


Notice that the ground and power are interchangeable. If it this PCB has many power islands AND there are controlled impedance traces, then it may be a better idea to keep all the controlled impedance traces on Signal 1 and Ground layer beneath it. If controlled impedance traces refer the power planes it must not either cross the split power plane junctions. If it is unavoidable to pass the split power plane junctions, we should place stitching capacitors. 
The four layer trace has one inherent drawback. You can not keep the power and ground traces tightly coupled for a typical 0.063” thick PCB. 

6 Layer stack up 

A 4 layer stack up is pretty much straight forward. A 6 layer stack up can have a number of variations. We should know the reasons behind choice of these variations and select the one that suites our requirements. A typical 6 Layer Stack up looks as follows. 

Signal1 
Ground 
Signal2 
Signal3 
Power 
Signal4 

In this stack up the traces on signal2 and signal3 should be routed in orthogonal fashion to avoid any potential cross talk. Care must be taken not to route traces in parallel along signal 2 and signal 3. 

All 4 signaling layers can refer to at least on power plane. So all the four signaling layers can have controlled impedance traces. One drawback of this arrangement is that the power and ground layers are not adjacent. Adjacent power and ground planes provide inter plane capacitance which is essential for providing low impedance path for the high frequency power supply noise. With this in mind some engineers use the following stackup.

Signal1 
Signal2
Ground
Power 
Signal3
Signal4 


The drawback of this stackup ? The Signal 1 and Signal 4 layers do not refer to the power planes directly. This problem results in inability to provide a controlled impedance on Signal 1 and Signal 4 layers.

So which stack up do you choose? If your design has very few high speed signals that need controlled impedance routing, the second stack up is better choice. You can route all the controlled impedance traces on Signal 2 and Signal 3 layers. The outer layers can be used for normal traces that do not need controlled impedance.

If however, your design has large number of high speed traces that need controlled impedance, the second stack up may not provide enough room. In such case the first stack up is a better choice. If you happen to choose the first stack up, try to fill the unused spaces on signal layers with plane flooding. This will provide extra plane capacitance between the power and ground layers required for the suppressing high frequency power supply noises. 

A six layer stack up lacks the number of the power planes. A typical microprocessor based system will need many small power islands, for which a single power plane is not sufficient. In this scenario some of the power islands will have to be on signal2 and/or power plane. If you find the things hard you may use 8 Layer stack up.  

8 Layer stack up

A four layer or a 6 six layer stack have one or other shortcoming. An 8 layer is the minimum number of layer that sufficiently addresses all the signal integrity requirements. It does not mean that 4 layers and 6 layers can not be used. The 4 layer and 8 layer can be and should be used for lower cost. But they will not fulfill all the signal integrity and EMI requirements is a dense PCB routing environment. 

A typical 8 Layer Stackup looks as follows 

Signal1 
Ground 
Signal2
Power 
Ground
Signal3 
Power 
Signal4 

The 8 Layer stack up provides ample routing space for multiple power islands. In the above typical stack up all signaling layers have at least one referencing power plane. The power and ground layer in the center provides good inter plane capacitance. If your system has many power islands and these power islands are next to the bottom layer, they do not have enough power to ground capacitance. Also the return path for the high speed signals in bottom layer (signal4) refer to the power plane which is not adjacent to a ground plane. For these reasons, some engineers use an alternate stackup as shown below. 

Signal1 
Ground 
Power
Signal2
Signal3
Ground 
Power
Signal4 

By keeping the separation between signal2 and signal3 large we can eliminate any potential crosstalk between signal2 and signal3.

A 4 layer stackup is pretty much straight forward. A 6 layer stack up can have a number of variations. We should know the reasons behind choice of these variations and select the one that suites our requirements. 

Symmetry and Board Warping 
In designing stackup, we should keep the it symmetrical with respect to the copper and non copper planes. For example of second layer from the top is a power or ground layer, then the second layer from the bottom should also be a ground or a power layer. This requirement has to do more with the mechanical requirement than the electrical requirement. An unsymmetrical stack up will create warping during any process that applies heat the PCB. A warped PCB will decrease yield especially if it has BGAs. The heights of the solder balls will be different in a warped board leading to open conditions and reducing yield. Keep your stack up symmetrical. If a power plane is partially filled, fill up the remaining are with copper, even if they are not connected to a net.