PCB Technical - Impedance control of printed circuit boards

Without impedance control, considerable signal reflection and signal distortion will occur, leading to design failure. Common signals, such as PCI bus, PCI-E bus, USB, Ethernet, DDR memory, LVDS signals, etc., require impedance control. Impedance control ultimately needs to be realized through PCB design, and higher requirements are put forward on the PCB board process. After communication with the PCB factory, combined with the use of EDA software, the impedance of the trace is controlled in accordance with the signal integrity requirements.

Different wiring methods can be calculated to obtain the corresponding impedance value.

1. Microstrip line

It consists of a ribbon wire and a ground plane, with a dielectric in the middle. If the dielectric constant of the dielectric, the width of the line, and the distance from the ground plane are controllable, then its characteristic impedance is also controllable, and its accuracy will be within ±5%.

2. Stripline

A stripline is a copper tape placed in the middle of a dielectric between two conductive planes. If the thickness and width of the line, the dielectric constant of the medium, and the distance between the two ground planes are all controllable, the characteristic impedance of the line is also controllable, and the accuracy is within 10%.

Laminate structure

3. PCB parameters

Different PCB factories have slight differences in PCB parameters. Through communication with the circuit board factory technical support, some parameter data of the factory can be obtained:

Surface layer copper foil: There are three kinds of surface layer copper foil material thickness that can be used: 12um, 18um and 35um. The final thickness after processing is about 44um, 50um and 67um.

Core board: Our commonly used board is S1141A, standard FR-4, two copper breads, and the available specifications can be determined by contacting the PCB manufacturer.

4. The structure of the multilayer board

In order to control the impedance of the PCB well, we must first understand the structure of the PCB: usually what we call a multi-layer board is formed by laminating a core board and a prepreg. The core board is a kind of rigid and specific The thick, two-bread copper plate is the basic material that constitutes the printed board. The prepreg constitutes the so-called wetting layer, which plays the role of bonding the core board. Although it also has a certain initial thickness, its thickness will change during the pressing process. Baineng.com is a subsidiary of Qinji Group and is a leading domestic electronic industry service platform. It provides online components, sensor procurement, PCB customization, BOM distribution, material selection and other electronic industry supply chain complete solutions, one-stop to meet the electronics industry The overall needs of small and medium-sized customers in the industry.

Usually the two outermost dielectric layers of the multilayer board are both wetting layers, and a separate copper foil layer is used as the outer copper foil on the outside of the two layers. The original thickness specifications of the outer copper foil and inner copper foil are generally 0.5OZ, 1OZ, 2OZ (1OZ is about 35um or 1.4mil), but after a series of surface treatments, the final thickness of the outer copper foil is average It will increase by about 1OZ. The inner copper foil is the copper clad on both sides of the core board, and its final thickness is very small from the original thickness, but due to etching, it is generally reduced by a few um.

The outermost layer of the multilayer board is the solder mask, which is what we often call "green oil". Of course, it can also be yellow or other colors. The thickness of the solder mask is generally not easy to accurately determine. The area without copper foil on the surface is slightly thicker than the area with copper foil. However, because of the lack of copper foil thickness, the copper foil still appears more prominent. When we use You can feel it when your finger touches the surface of the printed board.

When making a printed board of a certain thickness, on the one hand, it is required to select the parameters of various materials reasonably. On the other hand, the final forming thickness of the prepreg will be smaller than the initial thickness. Below is a typical 6-layer

5. Semi-cured film

The specifications (original thickness) are 7628 (0.185mm), 2116 (0.105mm), 1080 (0.075mm), 3313 (0.095mm). The actual thickness after pressing is usually 10-15um smaller than the original value. Up to 3 prepregs can be used for the same wetting layer, and the thickness of the 3 prepregs cannot be the same. At least one prepreg can be used, but some manufacturers require at least two. If the thickness of the prepreg is not enough, the copper foils on both sides of the core board can be etched away, and then the prepregs can be used for adhesion on both sides, so that a thicker wetting layer can be achieved.

Solder mask: The thickness of the solder mask on the copper foil is C2≈8-10um, and the thickness of the solder mask on the surface without copper foil C1 varies according to the surface copper thickness. When the surface copper thickness is 45um, C1≈13-15um, When the surface copper thickness is 70um, C1≈17-18um.

Wire cross section: We would think that the cross section of the wire is a rectangle, but it is actually a trapezoid. Taking the TOP layer as an example, when the thickness of the copper foil is 1OZ, the upper base of the trapezoid is 1MIL shorter than the lower base. For example, the line width is 5MIL, then the top bottom is about 4MIL, and the bottom bottom is 5MIL. The difference between the upper and lower bases is related to the copper thickness. The following table shows the relationship between the upper and lower bases of the trapezoid under different conditions.

Dielectric constant: The dielectric constant of the prepreg is related to the thickness

The dielectric constant of the board is related to the resin material used. The dielectric constant of the FR4 board is 4.2-4.7, and it will decrease as the frequency increases.

Dielectric loss factor: Under the action of an alternating electric field, the energy consumed by heat generated by a dielectric material is called dielectric loss, which is usually expressed by the dielectric loss factor tanδ. The typical value of S1141A is 0.015. The minimum line width and line spacing that can be guaranteed for processing: 4mil/4mil.

Differential pair PCB trace requirements

(1) Determine the wiring mode, parameters and impedance calculation. Differential pair routing is divided into outer layer microstrip line differential mode and inner layer strip line differential mode. By setting the parameters reasonably, the impedance can be calculated by the relevant impedance calculation software (such as POLAR-SI9000) or the impedance calculation formula.

(2) Take parallel equidistant lines. Determine the width and spacing of the traces. When routing the traces, strictly follow the calculated line width and spacing. The spacing between the two traces must always remain the same, that is, they must be parallel. There are two parallel ways: one is that the two wires run side-by-side, and the other is that the two wires run over-under. Generally, try to avoid using the latter, that is, the inter-layer differential signal, because in the actual processing of the PCB board, the lamination alignment accuracy between the laminations is much lower than the etching accuracy of the same layer, and the medium loss during the lamination process cannot be used. Ensure that the distance between the differential lines is equal to the thickness of the interlayer dielectric, which will cause the differential impedance of the interlayer differential pair to change. It is recommended to use the difference in the same layer as much as possible.