A brief discussion on PCB impedance control

As circuit design becomes increasingly complex and high-speed, how to ensure the integrity of various signals (especially high-speed signals), that is, to ensure signal quality, has become a difficult problem. At this time, it is necessary to use transmission line theory for analysis, and controlling the characteristic impedance matching of the signal line becomes the key. Inaccurate impedance control will cause considerable signal reflection and signal distortion, leading to design failure. Common signals, such as PCI bus, PCI-E bus, USB, Ethernet, DDR memory, LVDS signals, etc., all require impedance control. Impedance control ultimately needs to be implemented through PCB design, and higher requirements are also placed on PCB board technology. After communicating with PCB manufacturers and combining the use of EDA software, I have some superficial understanding of this issue and would like to share it with you.

The structure of multilayer board:

In order to control the impedance of PCB well, we must first understand the structure of PCB:

The multilayer boards we usually refer to are made of core boards and prepregs laminated on each other. The core board is a hard, copper-clad board with a specific thickness on both sides, which is the basic material for printed circuit boards. The prepregs constitute the so-called wetting layer, which plays the role of bonding the core board. Although they also have a certain initial thickness, their thickness will change during the pressing process.

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

The outermost layer of a 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, due to the lack of copper foil, the copper foil still appears more prominent, and we can feel it when we touch the surface of the printed circuit board with our fingers.

When making a printed circuit board of a certain thickness, on the one hand, it is required to reasonably select the parameters of various materials, and on the other hand, the final thickness of the prepreg will be smaller than the initial thickness. The following is a typical 6-layer stacking structure:

PCB parameters:

Different printed circuit board factories have slightly different PCB parameters. Through communication with the technical support of Shanghai Jiajietong Circuit Board Factory, we obtained some parameter data of the factory:

Surface copper foil:

There are three thicknesses of surface copper foil materials that can be used: 12um, 18um and 35um. The final thickness after processing is approximately 44um, 50um and 67um.

Core board: The board we commonly use is S1141A, standard FR-4, copper-clad on both sides. The optional specifications can be determined by contacting the manufacturer.

Prepreg:

The specifications (original thickness) are 7628 (0.185mm), 2116 (0.105mm), 1080 (0.075mm), 3313 (0.095mm). The actual thickness after pressing is usually about 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 foil on both sides of the core board can be etched off, and then the two sides are bonded with prepregs, so that a thicker wetting layer can be achieved.

Solder Mask:

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

Conductor cross section:

I used to think that the cross section of the wire was a rectangle, but it is actually a trapezoid. Take the TOP layer as an example. When the copper foil thickness is 1OZ, the upper base of the trapezoid is 1MIL shorter than the lower base. For example, if the line width is 5MIL, then its upper base is about 4MIL and the lower base 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 its thickness. The following table shows the thickness and dielectric constant parameters of prepregs of different models:

The dielectric constant of the board is related to the resin material used. The dielectric constant of FR4 board is 4.2-4.7, and it decreases with the increase of frequency.

Dielectric loss factor: The energy consumed by dielectric materials due to heat under the action of an alternating electric field is called dielectric loss, usually expressed as dielectric loss factor tanδ. The typical value of S1141A is 0.015.

The minimum line width and line spacing that can be ensured for processing is 4mil/4mil.