- +86-755-23012705
- Building 3, Jinfeng Industrial Park, Fuyong Street, Baoan District, Shenzhen ,China
- [email protected]

Menu

In PCB layout, it often happens that a thinner line has to be used to pass through an area due to limited wiring space, and then the line will be restored to its original width after passing through the area. The change of line width will cause the change of impedance, so the reflection occurs, which has an effect on the signal. Under what circumstances can we ignore this effect, and under what circumstances must we consider its effect?

Three factors are involved in this effect: **the size of the impedance change, the time of signal rise, and the delay of the signal on the narrow line.**

The magnitude of the impedance change is first discussed. Many circuits are designed to reflect noise less than 5% of the voltage swing (which is related to the noise budget on the signal). According to the reflection coefficient formula:

**ρ= (Z2-Z1)/(Z2+Z1) =△Z/(△Z+2Z1) ≤5%**

The approximate change rate of impedance can be calculated as follows: △Z/Z1≤10%

As you probably know, the typical impedance indicator on a circuit board is +/-10%, and this is the root cause.

If the impedance change occurs only once, such as when the line width changes from 8mil to 6mil and then remains 6mil wide, the impedance change must be less than 10% to meet the noise budget requirement that the signal reflected noise at the point of the sudden change does not exceed 5% of the voltage swing.

This is sometimes difficult to do. Take the case of microstrip lines on FR4 plates as an example.

Let’s calculate.

If the line width is 8mil, the thickness between the line and the reference plane is 4mil and the characteristic impedance is 46.5 ohm.

When the line width changes 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 limit.

As for the influence on the signal, it also depends on the signal rise time and the delay of the signal from the driving end to the reflection point. But at least that is a potential problem point. Fortunately, the problem can be solved by impedance matching terminations.

If the impedance changes twice, for example, after the line width changes from 8mil to 6mil, pull out 2cm and change back to 8mil. Then there will be a reflection at both ends of the 2cm long and 6mil wide line, once the impedance increases and positive reflection occurs, then the impedance decreases, and negative reflection occurs.

If the interval between the two reflections is short enough, it is possible for the two reflections to cancel each other out, thus reducing the effect.

Assuming that the transmission signal is 1V, 0.2V is reflected in the first positive reflection, 1.2V continues to transmit forward, and -0.2*1.2 = 0.24V is reflected back in the second reflection.

Assuming that the length of the 6mil line is extremely short, and the two reflections occur almost simultaneously, the total reflected voltage is only 0.04V, less than 5% of the noise budget requirement.

Therefore, whether and how much this reflection affects the signal depends on the time delay at which the impedance changes and the time of signal rise. As long as the delay at the impedance change is less than 20% of the time of signal rise, the reflected signal will not cause problems. If the signal rise time is 1ns, then the delay at the impedance change is less than 0.2ns for 1.2 inches, and reflection will not be a problem. That is to say, for this case, there will be no problem if the length of the 6mil wide trace is less than 3cm.

When the PCB line width changes, it should be carefully analyzed according to the actual situation to see if there is any influence. **There are three parameters to be concerned about: how much impedance changes, how long the signal rises, and how long the neck of the line width changes.**** **Roughly estimate according to the above method, appropriate to leave a certain margin. If possible, try to reduce the length of the neck.

It needs to be pointed out that in the actual PCB processing, the parameters can not be as accurate as of the theory, the theory can provide guidance for our design, but we can not copy, can not be dogmatic, after all, this is a practical science. The estimated value should be properly revised according to the actual situation, and then applied to the design.

XPCB Limited is a premium PCB & PCBA manufacturer based in China.

We specialize in multilayer flexible circuits, rigid-flex PCB, HDI PCB, and Rogers PCB.

Quick-turn PCB prototyping is our specialty. Demanding project is our advantage.

Building 3, JinFeng Industry Area, Fuyong Town, Baoan District, Shenzhen, Guangdong, 518103, China.

**Tel : **+86-136-3163-3671**Fax : **+86-755-2301 2705**Email : **[email protected]

© 2023 - XPCB Limited All Right Reserve