The role of USB2.0 data transmission on PCB design

The role of USB2.0 data transmission on PCB design

USB is a fast, bidirectional, isochronous transfer, inexpensive, easy-to-use, hot-swappable serial interface. Due to the advantages of fast data transmission, convenient interface, and support for hot swapping, USB devices are widely used. At present, most of the products on the market use USB2.0 as the interface, but many hardware novices encounter a lot of troubles in the USB application, often after the PCB is assembled, there are various problems with the USB interface

For example, the communication is unstable or unable to communicate, and there is no problem in checking the schematic diagram and soldering. Perhaps at this time, it is necessary to suspect that the PCB design is unreasonable. Drawing a PCB that meets the requirements of USB2.0 data transmission plays an extremely important role in the performance and reliability of the product.

The USB protocol defines that digital signals are transmitted by two differential signal lines (D+, D-). If the USB device is to work stably, the differential signal line must be laid out in strict accordance with the rules of differential signaling. Based on the author's years of experience in designing and debugging USB-related products, the following points of attention are summarized:

1. When laying out components, try to keep the differential line as short as possible to shorten the distance between the differential lines (√ is a reasonable way, × is an unreasonable way);

2. The differential line should be drawn first, and a pair of differential lines should not exceed two pairs of vias as far as possible (vias will increase the parasitic inductance of the line, thereby affecting the signal integrity of the line), and should be placed symmetrically (√ is a reasonable way, × unreasonable way)

3. Symmetrical parallel routing, which can ensure the tight coupling of the two wires, avoid 90° routing, arc or 45° are better routing methods (√ is a reasonable method, × is an unreasonable method)

4. Differential series connection resistance and capacitance, test points, placement of pull-up and pull-down resistors (√ is a reasonable way, × is an unreasonable way)

5. Due to factors such as pin distribution, vias, and wiring space, the differential line lengths are prone to mismatch. Once the line lengths do not match, the timing will shift, and common mode interference will be introduced, reducing signal quality. Therefore, the corresponding compensation should be made for the mismatch of the differential pair to match the line length. The length difference is usually controlled within 5 mil. The compensation principle is where the length difference occurs and where to compensate.

6. In order to reduce crosstalk, if space allows, the distance between other signal networks and the ground is at least 20 mil (20 mil is an empirical value) from the differential line. If the distance between the ground and the differential line is too close, it will affect the impedance of the differential line.

7. The output current of USB is 500mA. Pay attention to the line width of VBUS and GND. If 1Oz copper foil is used, the line width is greater than 20mil to meet the current-carrying requirements. Of course, the wider the line width, the better the integrity of the power supply.

Ordinary USB device differential line signal line width and line spacing can be consistent with the entire board signal line width and line spacing. However, when the operating speed of the USB device is 480 Mbits/s, it is not enough to only do the above points. We also need to control the impedance of the differential signal. Controlling the impedance of the differential signal line is very important to the integrity of the high-speed digital signal.

Because the differential impedance affects the eye diagram, signal bandwidth, signal jitter and interference voltage on the signal line of the differential signal. The differential line impedance is generally controlled at 90 (±10%) ohms (refer to the chip manual for specific values). The differential line impedance is inversely proportional to the line widths W1, W2, and T1, inversely proportional to the dielectric constant Er1, and proportional to the line spacing S1. , which is proportional to the distance H1 of the reference layer. The following figure is a cross-sectional view of the differential line.

The following figure shows the reference stack of a four-layer board. The middle two layers are reference layers. The reference layer is usually GND or Power. The reference layer corresponding to the differential line must be complete and cannot be divided. Otherwise, the impedance of the differential line will be discontinuous. . If the four-layer board is designed by stacking as shown in Figure 2, the differential line width of 4.5mil and the line spacing of 5.5mil can meet the differential impedance of 90Ω.

However, the 4.5mil line width and 5.5mil line spacing are only our theoretical design values. In the end, the circuit board factory will make appropriate adjustments to the line width and line spacing and the distance to the reference layer according to the required impedance value and combined with the actual production situation and the board.

The wiring rules described above are based on USB2.0 devices. In the process of USB wiring, grasp the shortest differential line, tight coupling, equal length, consistent impedance, and pay attention to the current-carrying capacity of the USB power cable. Master the above principles. The basic operation of USB devices no problem.