Detailed explanation of multilayer PCB laminate structure (1)

1.1 The number of layers and the principle of stacking


There are many factors to consider when determining the multilayer structure of a multilayer PCB. From the aspect of wiring, the more layers are more favorable for wiring, but the cost and difficulty of making the board will also increase. For manufacturers, whether the laminated structure is symmetrical or not is the focus of attention when manufacturing PCB boards, so the choice of the number of layers needs to consider the needs of various aspects in order to achieve the best balance.


For experienced designers, after completing the pre-layout of components, they will focus on the PCB bottlenecks. Analyze the wiring density of the circuit board with other EDA tools; then combine the number and types of signal lines with special wiring requirements such as differential lines, sensitive signal lines, etc. to determine the number of signal layers; then according to the type of power supply, isolation and anti-interference Requirements to determine the number of internal electrical layers. In this way, the number of layers of the entire circuit board is basically determined.


After the number of layers of the circuit board is determined, the next work is to arrange the circuit placement order of each layer reasonably. In this step, there are two main factors that need to be considered.


(1) Distribution of special signal layers.


(2) Distribution of power layer and ground layer.


If the number of layers of the circuit board is larger, the types of special combinations of signal layers, ground layers, and power layers are more numerous. It is also more difficult to determine which combination method is optimal, but the general principles are as follows.


(1) The signal layer should be adjacent to an internal electrical layer (internal power / ground layer). The large copper film of the internal electrical layer is used to provide shielding for the signal layer.


(2) The internal power plane and the ground plane should be tightly coupled, that is, the dielectric thickness between the internal power plane and the ground plane should be taken to a smaller value to increase the capacitance between the power plane and the ground plane and increase the resonance frequency. . The dielectric thickness between the internal power plane and the ground plane can be set in Protel's Layer Stack Manager. Select the [Design] / [Layer Stack Manager…] command, the system will pop up the layer stack manager dialog box, double-click the Prepreg text with the mouse, and the dialog box shown in Figure 11-1 will pop up. You can change the insulation in the Thickness option of this dialog box. The thickness of the layer.


If the potential difference between the power supply and the ground is not large, a smaller thickness of the insulation layer can be used, such as 5mil (0.127mm).


(3) The high-speed signal transmission layer in the circuit should be a signal intermediate layer and sandwiched between two internal electrical layers. In this way, the copper films of the two internal electrical layers can provide electromagnetic shielding for high-speed signal transmission, and can also effectively limit the radiation of high-speed signals between the two internal electrical layers without causing external interference.


(4) Avoid two signal layers directly adjacent. Crosstalk is easily introduced between adjacent signal layers, which causes the circuit function to fail. Adding a ground plane between the two signal layers can effectively avoid crosstalk.


(5) Multiple grounded internal electrical layers can effectively reduce ground impedance. For example, A signal layer and B signal layer use separate ground planes, which can effectively reduce common mode interference.


(6) Consider the symmetry of the layer structure.


1.2 Common Laminated Structures


The following example of a 4-layer board is used to explain how to optimize the arrangement and combination of various laminated structures.


For the commonly used 4-layer boards, there are several stacking methods (from top to bottom).

(1) Siganl_1 (Top), GND (Inner_1), POWER (Inner_2), Siganl_2 (Bottom).

(2) Siganl_1 (Top), POWER (Inner_1), GND (Inner_2), Siganl_2 (Bottom).

(3) POWER (Top), Siganl_1 (Inner_1), GND (Inner_2), Siganl_2 (Bottom).


Obviously, the power layer and ground layer of scheme 3 lack effective coupling and should not be adopted.


So how should you choose options 1 and 2? Generally, designers will choose Option 1 as the structure of the 4-layer board. The reason for choosing is not that scheme 2 cannot be adopted, but that general PCB boards only place components on the top layer, so it is more appropriate to adopt scheme 1. However, when components are placed on the top and bottom layers, and the dielectric thickness between the internal power layer and the ground layer is large and the coupling is poor, it is necessary to consider which layer has fewer signal lines. For scheme 1, there are fewer signal lines at the bottom layer, and a large-area copper film can be used to couple with the POWER layer. Conversely, if the components are mainly arranged at the bottom layer, scheme 2 should be used to make the board.


If the stacked structure shown in Figure 11-1 is used, then the power layer and the ground layer are already coupled. Considering the requirements of symmetry, Solution 1 is generally used.


After the analysis of the laminated structure of the 4-layer board is completed, the arrangement and combination method and the preferred method of the 6-layer board laminated structure will be explained by an example of the combined method of the 6-layer board.


(1) Siganl_1 (Top), GND (Inner_1), Siganl_2 (Inner_2), Siganl_3 (Inner_3), POWER (Inner_4), Siganl_4 (Bottom).


Solution 1 uses 4 signal layers and 2 internal power / ground layers, with more signal layers, which is beneficial to the wiring between components, but the disadvantages of this solution are also obvious, as shown in the following two aspects.


① The power plane and the ground plane are far apart and are not sufficiently coupled.

② The signal layer Siganl_2 (Inner_2) and Siganl_3 (Inner_3) are directly adjacent, the signal isolation is not good, and crosstalk is prone to occur.


(2) Siganl_1 (Top), Siganl_2 (Inner_1), POWER (Inner_2), GND (Inner_3), Siganl_3 (Inner_4), Siganl_4 (Bottom).


Compared with the solution 1, the solution 2 has sufficient coupling between the power layer and the ground layer, and has certain advantages over the solution 1. However, the signal layers of Siganl_1 (Top) and Siganl_2 (Inner_1) and Siganl_3 (Inner_4) and Siganl_4 (Bottom) are directly Adjacent, the signal isolation is not good, and the problem of prone to crosstalk has not been solved.


(3) Siganl_1 (Top), GND (Inner_1), Siganl_2 (Inner_2), POWER (Inner_3), GND (Inner_4), Siganl_3 (Bottom).

Compared with schemes 1 and 2, scheme 3 has one less signal layer and one more internal electrical layer. Although the layers available for wiring are reduced, this scheme solves the defects common to schemes 1 and 2.


① The power and ground planes are tightly coupled.

② Each signal layer is directly adjacent to the internal electrical layer and has effective isolation from other signal layers, making it less prone to crosstalk.

③ Siganl_2 (Inner_2) is adjacent to two internal electrical layers GND (Inner_1) and POWER (Inner_3), which can be used to transmit high-speed signals. The two internal electrical layers can effectively shield the external interference to the Siganl_2 (Inner_2) layer and the external interference of Siganl_2 (Inner_2).


Summarizing all aspects, Option 3 is obviously the most optimized one. At the same time, Option 3 is also a commonly used laminated structure of 6-layer boards.


Through the analysis of the above two examples, I believe that the reader has a certain understanding of the layered structure, but in some cases, a certain solution can not meet all the requirements, which needs to consider the priority of various design principles. Unfortunately due to


The layer design of the circuit board is closely related to the characteristics of the actual circuit. The anti-interference performance and design focus of different circuits are different, so in fact these principles have no established priority for reference. However, it can be determined that Design Principle 2 (the internal power plane and the ground plane should be tightly coupled) must be satisfied first when designing. In addition, if high-speed signals need to be transmitted in the circuit, then Design Principle 3 (high-speed signal transmission layer in the circuit It should be the signal intermediate layer, and sandwiched between the two internal electrical layers) must be satisfied. Table 11-1 gives the reference plan of multilayer laminate structure for readers' reference.