PCB Impedance Design

It is suitable for most PCB suppliers’ process standards and PCB board design with impedance control requirements.

1). 2 Layers Impedance Design

100 ohm differential impedance recommended design

• Ground package design: line width/spacing 7/5/7mil ground wire width ≥20mil signal and ground wire distance 6mil, add ground vias every 400mil.
• Design without ground package: line width/spacing 10/5/10mil, the distance between the differential pair and the pairis ≥20mil (not less than 10mil in special cases). It is recommended that the entire group of differential signal lines is shielded with grounding, and the distance between the differential signal and the shielding ground ≥35mil (not less than 20mil in special cases).

90 ohm differential impedance recommended design

• Ground package design: line width, line spacing 10/5/10mil ground wire width ≥20mil signal and ground wire distance 6mil or 5mil, add ground vias every 400mil
• Design without ground package: line width, line spacing 16/5/16mil, the distance between the differential pair and the pairis ≥20mil, it is recommended that the entire group of differential signal lines should be shielded with ground, and the distance between the differential signal and the shielding ground ≥35mil (In special cases, it cannot be less than 20mil).

Note: Prioritize the use of package ground design. However, if the line is short and there is a complete ground plane, it can be designed without package ground.

Calculation parameters:

FR-4, thickness 1.6mm+/-10%, dielectric constant 4.4+/-0.2, copper thickness 1.0 oz (1.4mil), solder mask thickness 0.6±0.2mil, dielectric constant 3.5+/-0.3.

Fig.1 Design of ground package   Fig.2 Design without ground package

2) 4 Layers impedance design

100 ohm differential impedance recommended design

line width, spacing 5/7/5mil differential pair and the distance between the pair ≥ 14mil (3W criterion);

Note: It is recommended that the entire group of differential signal lines is shielded with ground, and the distance between the differential signal and the shielded ground line is ≥35mil (in special cases, it cannot be less than 20mil).

90 ohm differential impedance recommended design

line width, spacing 6/6/6mil differential pair, and the distance between the pair ≥12mil (3W criterion).

Note: In the case of a long differential pair trace, it is recommended that the USB differential line wrap the ground at a distance of 6 mils on both sides to reduce the risk of EMI (with and without ground, the line width and line spacing standards are consistent).

Calculation parameters:

FR-4, thickness 1.6mm+/-10%, dielectric constant 4.4+/-0.2, copper thickness 1.0 oz (1.4mil), copper clad substrate(PP) 2116 (4.0-5.0mil), dielectric constant 4.3+/-0.2, solder mask thickness 0.6±0.2mil, dielectric constant 3.5+/-0.3.

Stack-up:

3) 6 Layers impedance design

The impedance design of the outer trace is the same as that of the four layer board.

The inner trace is generally more plane layer than the surface trace, and the electromagnetic environment is different from the surface.

The following is the third layer trace impedance control recommendation.

100 ohm differential impedance recommended design

line width, spacing 6/10/6mil.

The distance between the differential pair is ≥20mil (3W criterion).

90 ohm differential impedance recommended design

line width,line spacing 8/10/8mil.

The distance between the differential pair is ≥20mil (3W criterion).

Calculation parameters:

FR-4, thickness 1.6mm+/-10%, dielectric constant 4.4+/-0.2, copper thickness 1.0 oz (1.4mil), copper clad substrate(PP) 2116 (4.0-5.0mil), dielectric constant 4.3+/-0.2, solder mask thickness 0.6±0.2mil, dielectric constant 3.5+/-0.3.

Stack-up:

2. For layersmore than six layers, please design by yourself according to relevant rules or consult relevant personnel to determine the stack-up and trace
3. If there are other impedance control requirementswith special circumstances, please calculate by yourself or consult relevant personnel for alternative design solutions.

Note:

• Many situationsaffect impedance, and PCBs that require impedance control still need to indicate impedance control requirements in the PCB design data.
• 100 ohm differential impedance is mainly used for HDMI and LVDS signals, among which HDMI mustpass relevant certification.
• 90 ohm differential impedance is mainly used for USB signals.
• Single-ended 50 ohm impedance is mainly used for some DDR signals. Giventhe large DDR particles, some adopt an internally adjusted matching impedance design. The design is based on the demo board provided by the solution company. This design guide is not recommended;
• Single-ended 75 ohm impedance is mainly used for analog video input and output. There is a 75 ohm resistor in the circuit design to match the ground resistance, so there is no need to perform an impedance matching design in the PCB Layout. Still,you need to pay attention to the 75 ohm grounding resistance in the circuit that should be placed close to the terminal pin.

PP types

Solder mask thickness: 0.6±0.2mil

Cer=3.5+/-0.3