In order to ensure the quality of signal transmission, reduce EMI interference and pass the relevant impedance test certification, it is necessary to design the impedance matching of PCB key signals. This design guide is a synthesis of commonly used calculation parameters, signal characteristics of TV products, actual requirements of PCB Layout, calculation of SI9000 software, feedback information from PCB suppliers, etc., and finally comes to this recommended design. It is suitable for most PCB suppliers’ process standards and PCB design with impedance control requirements.
I. impedance design of PCB double panels
Recommended design of 100 ohm differential impedance
① Package design: line width and spacing of 7/5/7 mil.
Ground wire width ≥20mil
The distance from the signal ground wire is 6mil, and a grounding via hole is added every 400mil;
② Design without package: line width and spacing of 10/5/10mil.
The distance between differential pairs is ≥20mil (in special cases, it should not be less than 10mil).
It is suggested that the whole set of differential signal lines should be shielded by the ground, and the distance between the differential signal and the shielded ground is ≥35mil.
(Special circumstances can’t be less than 20mil).
Recommended design of 90 ohm differential impedance
①. Land parcel design:
Line width, spacing 10/5/10mil
Ground wire width ≥20mil
The distance between the signal and the ground wire is 6mil or 5mil, and a grounding via hole is added every 400mil;
② Design without package:
Line width, spacing 16/5/16mil
Distance between differential pairs is ≥20mil.
It is suggested that the whole set of differential signal lines should be shielded by the ground, and the distance between the differential signal and the shielded ground is ≥35mil.
(Special circumstances can’t be less than 20mil).
Essentials: The package design is preferred; and the package design can be adopted if the route is short and the plane is complete.
Calculation parameters: sheet FR-4, sheet thickness 1.6mm+/-10%, sheet dielectric constant 4.4+/-0.2, copper thickness 1.0 oz (1.4mil)
The welding oil resistance thickness is 0.6±0.2mil, and the dielectric constant is 3.5+/-0.3.
Second, impedance design of PCB four-layer board
Recommended design of 100 ohm differential impedance
Line width and spacing of 5/7/5mil
Distance between differential pairs ≥14mil(3W criterion)
Note: It is recommended that the whole set of differential signal lines should be shielded by the ground, and the distance between the differential signal and the shielded ground wire should be ≥35mil (in special cases, it should not be less than 20mil).
Recommended design of 90 ohm differential impedance
Line width and spacing 6/6/6mil
Distance between differential pairs ≥12mil(3W criterion)
Essentials: When the differential pair wiring is long, it is recommended that the USB differential wiring be wrapped at a distance of 6mil on both sides to reduce the EMI risk (with and without wrapping, the line width and line spacing standards are the same).
Calculation parameters: sheet FR-4, sheet thickness 1.6mm+/-10%, sheet dielectric constant 4.4+/-0.2, copper thickness 1.0 oz (1.4mil)
Semi-cured sheet (PP) 2116(4.0-5.0mil) with dielectric constant of 4.3+/-0.2.
The welding oil resistance thickness is 0.6±0.2mil, and the dielectric constant is 3.5+/-0.3.
Laminated structure:
Screen printing layer
solder mask
Copper cortex
prepreg
Copper-clad substrate
prepreg
Copper cortex
solder mask
Screen printing layer
III. Impedance design of PCB six-layer board
The six-layer laminate structure will be different for different occasions. This guide only recommends the design of the common laminate (see Figure 2), and the later recommended designs are all based on the data obtained from the laminate in Figure 2.
The impedance design of the outer wiring is the same as that of the four-layer board. Generally, the inner wiring has one more plane layer than the surface wiring, and the electromagnetic environment is different from that of the surface wiring. Here are the suggestions for impedance control of the third wiring (refer to Figure 4 for lamination).
Recommended design of 100 ohm differential impedance
Line width and spacing 6/10/6 mil
Distance between differential pairs ≥20mil(3W criterion);
Recommended design of 90 ohm differential impedance
Line width, line spacing 8/10/8 mil
Distance between differential pairs ≥20mil(3W criterion);
Calculation parameters: sheet FR-4, sheet thickness 1.6mm+/-10%, sheet dielectric constant 4.4+/-0.2, copper thickness 1.0 oz (1.4mil)
Semi-cured sheet (PP) 2116(4.0-5.0mil) with dielectric constant of 4.3+/-0.2.
The welding oil resistance thickness is 0.6±0.2mil, and the dielectric constant is 3.5+/-0.3.
Laminated structure:
Top screen printing
solder mask
Copper cortex
prepreg
Copper-clad substrate
prepreg
Copper-clad substrate
prepreg
Copper cortex
solder mask
Bottom screen printing
For PCB boards with more than four or six layers, please design by yourself or consult relevant personnel to determine the laminated structure and routing scheme according to relevant rules.
5. If there are other impedance control requirements due to special circumstances, please calculate by yourself or consult relevant personnel to determine the design scheme.
Note: ① There are many situations that affect impedance, and the PCB that needs impedance control still needs to indicate impedance control requirements in PCB design data or sample sheet;
② 100 ohm differential impedance is mainly used for HDMI and LVDS signals, among which it is mandatory for HDMI to pass relevant certification;
③ 90 ohm differential impedance is mainly used for USB signals;
④ Single-ended 50 ohm impedance is mainly used for DDR signals. Since most DDR particles are designed with internal adjustment matching impedance, the design is based on the Demo board provided by the solution company, which is not recommended in this design guide.
⑤ Single-ended 75 ohm impedance is mainly used for analog video input and output. In the circuit design, a 75 ohm resistor matches the ground resistance, so there is no need for impedance matching design in PCB Layout. However, it should be noted that the 75 ohm ground resistance in the circuit should be placed close to the terminal pins.
Commonly used PP
Thickness of welding oil resistance: 0.6 0.2milcer = 3.5+/-0.3 If you need pcb layout design business, please contact customer service for specific design requirements.
