2022-04-28

View：702

Author：pcb

When conducting **PCB board** wiring, it often happens that when the traces pass through a certain area, due to the limited wiring space in this area, thinner lines have to be used. After passing through this area, the lines return to their original widths. Changes in trace width cause impedance changes and therefore reflections, affecting the signal. So under what circumstances can this effect be ignored, and under what circumstances do we have to consider its effect? Three factors are involved in this effect: the magnitude of the impedance change, the rise time of the signal, and the delay of the signal on the narrow line.

The magnitude of the impedance change is discussed first. The design of many circuits requires that the reflected noise is less than 5% of the voltage swing (this is related to the noise budget on the signal). The approximate rate of change of impedance can be calculated as: △Z/Z1 ≤ 10%. As you probably know, the typical specification for impedance on a circuit board is +/-10%, and that's the root cause.

If the impedance change only occurs, for example, after the line width is changed from 8 mil to 6 mil, and the width remains 6 mil, to achieve the noise budget requirement that the signal reflection noise at the sudden change does not exceed 5% of the voltage swing, the impedance change must be less than 10 %. This is sometimes difficult to do. Take the microstrip line on the FR4 board as an example, let's calculate it. If the line width is 8 mil, the thickness between the line and the reference plane is 4 mil, and the characteristic impedance is 46.5 ohms. After the line width is changed to 6mil, the characteristic impedance becomes 54.2 ohms, and the impedance change rate reaches 20%. The amplitude of the reflected signal must exceed the standard. As for how much it affects the signal, it is also related to the rise time of the signal and the delay from the driving end to the signal at the reflection point. But at least this is a potential problem point. Fortunately, impedance matching termination can solve the problem at this time.

If the impedance changes twice, for example, the line width changes from 8 mil to 6 mil, and then changes back to 8 mil after pulling out 2 cm. Then reflection will occur at both ends of the 2cm long and 6mil wide line. The impedance becomes larger and positive reflection occurs, and then the impedance becomes smaller and negative reflection occurs. If the interval between the two reflections is short enough, the two reflections may cancel each other out, thereby reducing the impact. Assuming that the transmission signal is 1V, 0.2V is reflected in the second regular reflection, 1.2V continues to transmit forward, and -0.2*1.2 = 0.24v is reflected back in the second reflection. Assuming that the 6mil line is extremely short and the two reflections occur almost simultaneously, the total reflected voltage is only 0.04V, which is less than the 5% noise budget requirement. Therefore, whether this reflection affects the signal, and how much, is related to the delay at the impedance change and the rise time of the signal. Research and experiments have shown that as long as the delay at the impedance change is less than 20% of the rise time of the signal, the reflected signal will not cause a problem. If the signal rise time is 1ns, then the delay at the impedance change is less than 0.2ns corresponding to 1.2 inches, and reflections will not cause problems. That is to say, for this case, there is no problem as long as the length of the 6mil wide trace is less than 3cm.

When the trace width of the PCB board changes, it should be carefully analyzed according to the actual situation to see if it will affect it. There are three parameters to be concerned about: how large is the impedance change, what is the signal rise time, and how long is the neck of the line width change. Roughly estimate according to the above method, and leave a certain margin appropriately. If possible, try to reduce the length of the neck. It should be pointed out that in the actual PCB board processing, the parameters cannot be as in the theory. The theory can provide guidance for our design, but it cannot be copied or dogmatic. After all, this is a practical science. The estimated value should be revised appropriately according to the actual situation, and then applied to the design. If you feel inexperienced, be conservative first, and then adjust according to the manufacturing cost on **PCB board**.