Without impedance control, considerable signal reflection and distortion will be caused, resulting in design failure. Common signals, such as PCI bus, PCI-E bus, USB, Ethernet, DDR memory, LVDS signal, etc., all need impedance control. Impedance control ultimately needs to be realized through PCB design, which also puts forward higher requirements for PCB board technology. After communication with PCB factory and combined with the use of EDA software, the impedance of wiring is controlled according to the requirements of signal integrity.

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

Microstrip lines

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

How to control PCB wiring impedance

Stripline

A ribbon line is a strip of copper in the middle of the dielectric between two conducting planes. If the thickness and width of the line, the dielectric constant of the medium, and the distance between the ground planes of the two layers are controllable, the characteristic impedance of the line is controllable, and the accuracy is within 10%.

How to control PCB wiring impedance

The structure of multi-layer board:

In order to control PCB impedance well, it is necessary to understand the structure of PCB:

Usually what we call multilayer board is made up of core plate and semi-solidified sheet laminated together with each other. Core board is a hard, specific thickness, two bread copper plate, which is the basic material of the printed board. And the semi-cured piece constitutes the so-called infiltration layer, plays the role of bonding the core plate, although there is a certain initial thickness, but in the process of pressing its thickness will occur some changes.

Usually the outermost two dielectric layers of a multilayer are wetted layers, and separate copper foil layers are used on the outside of these two layers as the outer copper foil. The original thickness specification of outer copper foil and inner copper foil is generally 0.5oz, 1OZ, 2OZ (1OZ is about 35um or 1.4mil), but after a series of surface treatment, the final thickness of outer copper foil will generally increase by about 1OZ. The inner copper foil is the copper covering on both sides of the core plate. The final thickness differs little from the original thickness, but it is generally reduced by several um due to etching.

The outermost layer of the multilayer board is the welding resistance layer, which is what we often say “green oil”, of course, it can also be yellow or other colors. The thickness of the solder resistance layer is generally not easy to determine accurately. The area without copper foil on the surface is slightly thicker than the area with copper foil, but because of the lack of copper foil thickness, so the copper foil is still more prominent, when we touch the printed board surface with our fingers can feel.

When a particular thickness of the printed board is made, on the one hand, reasonable choice of material parameters is required, on the other hand, the final thickness of the semi-cured sheet will be smaller than the initial thickness. The following is a typical 6-layer laminated structure:

How to control PCB wiring impedance

PCB parameters:

Different PCB plants have slight differences in PCB parameters. Through communication with circuit board plant technical support, we obtained some parameter data of the plant:

Surface copper foil:

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

Core plate: S1141A, standard FR-4, two breaded copper plates are commonly used. The optional specifications can be determined by contacting the manufacturer.

Semi-cured tablet:

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 less than the original value. A maximum of 3 semi-cured tablets can be used for the same infiltration layer, and the thickness of 3 semi-cured tablets can not be the same, at least one half cured tablets can be used, but some manufacturers must use at least two. If the thickness of the semi-cured piece is not enough, the copper foil on both sides of the core plate can be etched off, and then the semi-cured piece can be bonded on both sides, so that a thicker infiltration layer can be achieved.

Resistance welding layer:

The thickness of the solder resist layer on the copper foil is C2≈8-10um. The thickness of the solder resist layer on the surface without copper foil is C1, which varies with the thickness of copper on the surface. When the thickness of copper on the surface is 45um, C1≈13-15um, and when the thickness of copper on the surface is 70um, C1≈17-18um.

Traverse section:

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

How to control PCB wiring impedance

Permittivity: The permittivity of semi-cured sheets is related to thickness. The following table shows the thickness and permittivity parameters of different types of semi-cured sheets:

How to control PCB wiring impedance

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

Dielectric loss factor: dielectric materials under the action of alternating electric field, due to heat and energy consumption is called dielectric loss, usually expressed by dielectric loss factor Tan δ. The typical value for S1141A is 0.015.

Minimum line width and line spacing to ensure machining: 4mil/4mil.

Impedance calculation tool introduction:

When we understand the structure of the multilayer board and master the required parameters, we can calculate the impedance through EDA software. You can use Allegro to do this, but I recommend Polar SI9000, which is a good tool for calculating characteristic impedance and is now used by many PCB factories.

When calculating the characteristic impedance of the inner signal of both the differential line and the single terminal line, you will find only a slight difference between Polar SI9000 and Allegro due to some details, such as the shape of the cross section of the wire. However, if it is to calculate the characteristic impedance of the Surface signal, I suggest you choose the Coated model instead of the Surface model, because such models take into account the existence of solder resistance layer, so the results will be more accurate. The following is a partial screenshot of the surface differential line impedance calculated with Polar SI9000 considering the solder resistance layer:

How to control PCB wiring impedance

Since the thickness of the solder resist layer is not easily controlled, an approximate approach can also be used, as recommended by the board manufacturer: subtract a specific value from the Surface model calculation. It is recommended that the differential impedance be minus 8 ohms and the single-end impedance be minus 2 ohms.

Differential PCB requirements for wiring

(1) Determine the wiring mode, parameters and impedance calculation. There are two kinds of difference modes for line routing: outer layer microstrip line difference mode and inner layer strip line difference mode. Impedance can be calculated by related impedance calculation software (such as POLAR-SI9000) or impedance calculation formula through reasonable parameter setting.

(2) Parallel isometric lines. Determine the line width and spacing, and strictly follow the calculated line width and spacing when routing. The spacing between two lines must always remain unchanged, that is, to keep parallel. There are two ways of parallelism: one is that the two lines walk in the same side-by-side layer, and the other is that the two lines walk in the over-under layer. Generally try to avoid using the difference signal between the layers, namely because in the actual processing of PCB in the process, due to the cascading laminated alignment accuracy is much lower than provided between the etching precision, and in the process of laminated dielectric loss, cannot guarantee difference line spacing is equal to the thickness of the interlayer dielectric, will cause the difference between the layers of the difference of impedance change. It is recommended to use the difference within the same layer as much as possible.