Multilayer Laminated Structure
Many PCB engineers often draw computer motherboards and are very proficient with excellent tools such as Allegro. However, it is a pity that they rarely know how to control impedance and how to use tools for signal integrity analysis. IBIS model. I think the real PCB masters should still be signal integrity experts, not just on the basis of connecting wires and vias. It is easy to layout aboard, but difficult to layout a good one.
Multilayer Laminated Structure
Multilayer Laminated Structure Plan
After determining the number of power, ground, and signal layers, the relative arrangement of them is a topic that every PCB engineer cannot avoid.
General rules of Multilayer Laminated Structure Plan
1. The bottom of the component surface (the second layer) is the ground plane, which provides a device shielding layer and a reference plane for the top layer wiring.
2. All signal layers are as close as possible to the ground plane.
3. Try to avoid two signal layers directly adjacent to each other.
4. The main power supply is adjacent to it as much as possible.
5. Take into account the symmetry of the laminated structure.
For the layer layout of the motherboard, it is difficult for the existing motherboard to control the parallel long-distance wiring. For the board-level operating frequency above 50MHZ (the case below 50MHZ can be appropriately relaxed).
6. The component surface and welding surface are a complete ground plane (shield).
7. No adjacent parallel wiring layer;
8. All signal layers are as close as possible to the ground plane;
9. The key signal is adjacent to the stratum and does not cross the partition.
Note: When setting up the specific PCB layers, the above principles should be flexibly mastered. Based on the understanding of the above principles, according to the actual requirements of the single board, such as: whether a key wiring layer, power supply, and ground plane division is required, Determine the arrangement of the layers, and don’t just copy it or stick it at all.
The following is a specific discussion on the arrangement of the veneer layers:
*Four-layer board, preferred option 1, available option 3
Scheme Power Layer Number Ground Layer Number Signal Layer Number 1 2 3 4
1 1 1 2 S G P S
2 1 2 2 G S S P
3 1 1 2 S P G S
Plan 1 Multilayer Laminated Structure
The main selection layer setting scheme of the four-layer PCB of this scheme, there is a ground plane under the component surface, and the key signal is preferably arranged on the TOP layer; as for the layer thickness setting, the following suggestions are provided:
To meet the impedance control core board (GND to POWER) should not be too thick to reduce the distributed impedance of the power supply and ground plane; to ensure the decoupling effect of the power plane; in order to achieve a certain shielding effect, someone tried to put the power supply and ground plane on the TOP, BOTTOM layer,
Plan 2 Multilayer Laminated Structure
In order to achieve the desired shielding effect, this solution has at least the following defects:
The power and ground are too far apart, and the power plane impedance is large
The power and ground planes are extremely incomplete due to the influence of component pads
The signal impedance is not continuous due to the incomplete reference plane
In fact, due to a large number of surface mount devices, as the devices become denser, the power and ground of this solution can hardly be used as a complete reference plane, and the expected shielding effect is difficult to achieve; solution 2 has a limited range of use. But in individual boards, scheme 2 is the best layer setting scheme.
The following are the use cases of Option 2;
Case (special case): During the design process, the following situations occurred:
A. The whole board has no power plane, only GND and PGND occupy one plane each;
B. The wiring of the whole board is simple, but as an interface filter board, the radiation of wiring must be paid attention to;
C. The board has fewer SMD components, most of which are plug-ins.
Analysis:
1. Since the board has no power plane, the power plane impedance problem does not exist;
2. Due to the small number of SMD components (single-sided layout), if the surface layer is made as a plane layer and the inner layer is routed, the integrity of the reference plane is basically guaranteed, and the second layer can be laid with copper to ensure a small amount of top-level wiring reference plane;
3. As an interface filter board, the radiation of PCB wiring must be paid attention to. If the inner layer is wired, the surface is GND and PGND, the wiring is well shielded, and the radiation of the transmission line is controlled;
In view of the above reasons, when laying out the layers of this board, we decided to adopt option 2, namely: GND, S1, S2, and PGND. Since there are still a few short traces on the surface layer, and the bottom layer is a complete ground plane, we are in S1 The wiring layer is laid with copper to ensure the reference plane of the surface wiring; among the five interface filter boards, based on the same analysis as above, the designer decided to adopt Option 2, which is also a classic layer setting.
The above special cases are to tell everyone that you must understand the principle of layer arrangement, not copy it mechanically.
Plan 3 Multilayer Laminated Structure
This scheme is similar to scheme 1, which is suitable for the main components in the BOTTOM layout or the bottom wiring of key signals; in general, this scheme is restricted;
*Six-layer board, preferred option 3, available option 1, alternative option 2, 4
Scheme Power Ground Signal 1 2 3 4 5 6
#1 1 1 4 S1 G S2 S3 P S4
#2 1 1 4 S1 S2 G P S3 S4
#3 1 2 3 S1 G1 S2 G2 P S3
#4 1 2 3 S1 G1 S2 G2 P S3
For a six-layer board, scheme 3 is preferred, and the wiring layer S2 (stripline) is preferred, followed by S3 and S1. The main power supply and its corresponding ground are placed on the 4th and 5th layers. When the layer thickness is set, increase the spacing between S2-P and reduce the spacing between P-G2 (correspondingly reduce the spacing between G1-S2 layers), In order to reduce the impedance of the power plane, reduce the influence of the power on S2;
When the cost requirements are high, solution 1 can be used, preferably wiring layers S1, S2, followed by S3, S4. Compared with solution 1, solution 2 ensures that the power supply and the ground plane are adjacent to reduce the power supply impedance, but S1, S2, S3, S4 are all exposed, only S2 has a better reference plane;
For occasions with high requirements for a small number of local signals, solution 4 is more suitable than solution 3, and it can provide an excellent wiring layer S2.
*Eight-layer board: preferred plan 2, 3, available plan 1
Scheme Power Ground Signal 1 2 3 4 5 6 7 8
#1 1 2 5 S1 G1 S2 S3 P S4 G2 S5
#2 1 3 4 S1 G1 S2 G2 P S3 G3 S4
#3 2 2 4 S1 G1 S2 P1 G2 S3 P2 S4
#4 2 2 4 S1 G1 S2 P1 P2 S3 G3 S4
#5 2 2 4 S1 G1 P1 S2 S3 G2 P2 S4
For single power supply:
Scheme 2 reduces the adjacent wiring layers compared with scheme 1, increases the adjacent main power supply and the corresponding ground, and ensures that all signal layers are adjacent to the ground plane. The cost is: sacrificing a wiring layer;
For the case of dual power supplies:
Scheme 3 is recommended. Scheme 3 takes into account the advantages of no adjacent wiring layers, symmetrical laminate structure, and adjacent main power supply to ground, but S4 should reduce key wiring;
Solution 4: No adjacent wiring layers, symmetrical laminate structure, but the high impedance of the power supply plane; appropriately increase 3-4, 5-6, and reduce the layer spacing between 2-3 and 6-7;
Solution 5: Compared with Solution 4, it ensures that the power and ground planes are adjacent; but S2 and S3 are adjacent, and S4 uses P2 as the reference plane; there are fewer key wiring at the bottom and the inter-line interference between S2 and S3 can be controlled This plan can be considered in the case of;
*Ten-layer board: recommended plan 2, 3, available plan 1, 4
Option 3: Expand the respective spacing between 3-4 and 7-8, reduce the spacing between 5-6, the main power supply and its corresponding should be placed on the 6th and 7th layers; preferably the wiring layers S2, S3, S4, followed by S1, S5; this solution It is suitable for occasions where the signal wiring requirements are not much different, taking into account performance and cost; it is recommended for everyone, but you need to pay attention to avoid parallel and long-distance wiring between S2 and S3;
Option 4: EMC effect is excellent, but compared with Option 3, one wiring layer is sacrificed; for key single boards that require low cost, high EMC indicators, and double power layers, this solution is recommended; wiring layer is preferred S2, S3, for the case of a single power layer, first consider Option 2, and then consider Option 1. Solution 1 has obvious cost advantages, but there are too many adjacent wiring, and it is difficult to control parallel long lines;
*Twelve-layer board: recommended plan 2, 3, available plan 1, 4, alternative plan 5
Schemes 2 and 4 have excellent EMC performance, and schemes 1 and 3 have better cost performance;
The above layer arrangement is a general principle and is for reference only. In the specific design process, you can combine the above arrangement principles according to the number of power layers required, the number of wiring layers, the number and proportion of signals required for special wiring, and the division of power and ground. Be flexible.
EMC problem Multilayer Laminated Structure
You should also pay attention to EMC suppression when laying out the board! This is very unsure, distributed capacitance exists at any time!
How to ground
PCB design originally had to consider many factors, and different environments need to consider different factors.
Land division and tandem
Grounding is one of the important means to suppress electromagnetic interference and improve the EMC performance of electronic equipment. Correct grounding can not only improve the product’s ability to suppress electromagnetic interference, but also reduce the product’s external EMI emission.
The meaning of grounding
The “ground” of electronic equipment usually has two meanings: one is “earth” (safe ground), and the other is “system reference ground” (signal ground). Grounding refers to the establishment of a low-resistance conductive path between the system and a certain potential reference plane. “Connecting to the earth” is to use the earth’s potential as the reference and the earth as the zero potential to connect the metal casing of electronic equipment and the circuit reference point with the earth.
Connecting the ground plane to the earth is often due to the following considerations:
A, improve the stability of the equipment circuit system;
B, static discharge;
C, to provide security for the staff.
The purpose of grounding
A Safety considerations, that is, protective grounding;
B. Provide a stable zero potential reference point (signal ground or system ground) for the signal voltage;
C, the shield is grounded.
Basic grounding method
There are three basic grounding methods in electronic equipment: single-point grounding, multi-point grounding, and floating ground.
Single point grounding Multilayer Laminated Structure
Single-point grounding means that in the entire system, only one physical point is defined as the ground reference point, and all other points that need to be grounded are connected to this point. It is suitable for circuits with lower frequency (below 1MHZ). If the operating frequency of the system is so high that the operating wavelength is comparable to the length of the system grounding lead, single-point grounding is a problem. When the length of the ground wire is close to 1/4 wavelength, it is like a short-circuited transmission line.
The current and voltage of the ground wire are distributed in a standing wave, and the ground wire becomes a radiating antenna and cannot function as a “ground”.
In order to reduce ground impedance and avoid radiation, the length of the ground wire should be less than 1/20 wavelength. In the treatment of the power supply circuit, single-point grounding can generally be considered. For PCBs with a large number of digital circuits, it is generally not recommended to use single-point grounding due to its rich high-order harmonics.
Multi-point grounding Multilayer Laminated Structure
Multi-point grounding means that each grounding point in the equipment is directly connected to the ground plane closest to it, so that the length of the grounding lead is the shortest.
The multi-point grounding circuit has a simple structure, and the high-frequency standing wave phenomenon that may appear on the grounding line is significantly reduced. It is suitable for occasions with higher operating frequencies (>10MHZ). However, multi-point grounding may cause many ground loops to form inside the device, thereby reducing the device’s resistance to external electromagnetic fields. In the case of multi-point grounding, pay attention to the ground loop problem, especially when networking between different modules and devices. Electromagnetic interference caused by ground loop:
The ideal ground should be a physical entity with zero potential and zero impedance. But the actual ground wire itself has both a resistance component and a reactance component. When a current flows through the ground wire, a voltage drop will occur. The ground wire will form a loop with other connections (signal, power cord, etc.). When the time-varying electromagnetic field is coupled to this loop, an induced electromotive force will be generated in the ground loop and coupled to the load by the ground loop, posing a potential EMI threat.
Floating ground Multilayer Laminated Structure
Floating refers to a grounding method in which the equipment grounding system is electrically insulated from the earth.
Due to some weaknesses of the floating ground itself, it is not suitable for general large-scale systems, and its grounding method is rarely used
General selection principles for grounding methods:
For a given device or system, at the highest frequency (corresponding wavelength) of interest, when the length of the transmission line L>in, it is regarded as a high-frequency circuit, otherwise, it is regarded as a low-frequency circuit. According to the rule of thumb, it is better to use single-point grounding for circuits lower than 1MHZ; for higher than 10MHZ, multi-point grounding is better. For frequencies between the two, as long as the length L of the longest transmission line is less than /20″, single-point grounding can be used to avoid common impedance coupling.
The general selection principle for grounding is as follows:
(1) Low-frequency circuit (<1MHZ), single-point grounding is recommended;
(2) High-frequency circuit (>10MHZ), it is recommended to use multi-point grounding;
(3) High and low frequency mixed circuit, mixed grounding.
Please contact us now for more details, or you can get support from HIEDESIGN as ODM & OEM.