Hello, and welcome to the TI Precision Labs video on PCB trace impedance matching. This is part of a larger series on PCB layout for good EMC. This series is specifically intended to cover mixed signal designs where the digital signals are less than 100 megahertz and the clock rise times are greater than 1 nanosecond. In this video, we will discuss how the PCB trace characteristic impedance is determined by its geometry.

We will see how matching the driver-to-trace impedance can impact the rise time, overshoot, and ringing on digital communication signals. This is important because overshoot and ringing can create noise problems that impact sensitive analog and, in some cases, even cause digital communications issues. The characteristic impedance of a line is the impedance seen by the wavefront traveling down the line. Impedance mismatches between the driver, transmission line, and load will cause reflections that translate into overshoot and ringing on the digital signals.

The geometry of a PCB trace relative to its ground return plane will determine its characteristic impedance. In this slide, you can see the micro strip and strip line configurations. The trace width, dielectric thickness, and dielectric constant can be used to calculate the characteristic impedance. Transmission line theory is a very deep subject, and we will only brush over it briefly in this section. The references provided at the end of this presentation provide a much more detailed coverage of the subject.

The analog engineer's calculator provides a simple way to find the characteristic impedance for a micro strip configuration. Simply enter the width, length, dielectric thickness, and dielectric coefficient to find the characteristic impedance. The most common characteristic impedance is 50 ohms. For most PC board traces, the characteristic impedance will range from 20 to 200 ohms. For this example, the characteristic impedance is 107 ohms. The link at the bottom of the page can be used to download the analog engineer's calculator.

This slide shows some very basic theory for transmitting a digital signal across a PC board transmission line. Transmission line reflections will happen whenever there's an impedance mismatch in the signal path. To avoid reflections, the driver impedance must match the PC board trace impedance and the load impedance. Generally, the load is the input impedance of a gate which is effectively an infinite input impedance. So this will always have a full reflection.

The driver will have an internal impedance RD and an external termination resistance Rterm. The external termination resistance is used to match the PC board trace impedance. If RD plus Rterm matches the PC board trace impedance, the signal delivered to the load will not have overshoot or undershoot. If RD plus Rterm is less than the trace impedance, there will be overshoot. And if it is greater than the trace impedance, there will be undershoot.

A bounce diagram is a method that's used to calculate the transmission line reflections so that we can predict the waveform that will be delivered to the load. Let's do a bounce diagram example for a system with overshoot. For this example, a 5-volt step is applied to the transmission line. And RD plus Rterm is 20 ohms. The reflection coefficient gamma is calculated on the driver's side as minus 0.429 and on the receiver side as 1.0. The receiver will generally have a reflection coefficient of 1.0, as it is effectively an open circuit and will completely reflect the waveform.

When a 5-volt step is first applied, a voltage divider forms between the driver impedance and the trace impedance so that the signal on the PCB trace is 3.75 volts. Based on the trace length, it will take some time for the signal to travel to the receiver. When the signal reaches the receiver, there will be 100% reflection. And the initial signal seen by the receiver is 7.14 volts. The reflected signal travels back to the driver where it is again reflected by minus 0.429 because of the impedance mismatch. This reflection travels back to the receiver and causes the signal to drop to 4.08 volts.

This process continues, and you see the output waveform shown. If you did the same calculation with a matched impedance, you would not see any overshoot. If you used a very large termination resistance, you would see undershoot. Now let's take a look at a simple calculator that can automatically perform this calculation. This slide shows how the analog engineer's calculator can be used to predict reflections. In this example, the length, dielectric constant, and dielectric thickness are entered. The signal frequency, amplitude, and termination impedance are also used to predict the reflections.

Adjusting the calculator parameters is a quick and easy way to get an intuitive feel on how transmission lines work. In this example, we use the calculator with real-world PC board specifications for a measured experiment. You can see that the measured results look very similar to the predicted results but do not match perfectly. In the next few slides, we'll look at a summary of multiple experiments related to adjusting the termination impedance.

This slide shows measured results for a termination line, where the termination resistance is adjusted across a wide range. The schematic of the circuit tested is shown in the lower-left side. A 74LVC1G38 gate is used as the transmitter and receiver. One line, called the aggressor, is driven with a 3.3-volt, 10-megahertz square wave. The other line, called the victim, is driven with a logic low. The aggressor will cause crosstalk on the victim. For the experiment, we will look at overshoot and crosstalk between the two traces.

Theoretically, the overshoot will be 0 when the termination resistance plus the driver impedance is equal to the trace impedance. The calculated impedance for this trace is approximately 66 ohms. Assuming the drive impedance is 10 ohms, the termination resistance should be 56 ohms. Looking at the oscilloscope waveforms, you can see that for a 0 ohm termination resistance, there's a great deal of overshoot and ringing. The 50-ohm termination has a very fast rise time but no significant overshoot. The 100-ohm termination has a slow rise time.

The graph summarizes the experimental results over a wide range of termination resistance. The experimental results show that the calculated trace impedance is approximately correct, as a 50-ohm termination produces optimal results. Earlier in the presentation, we mentioned that rise time is important to RF systems, as it determines how much high-frequency noise the square wave generates. The termination resistance will directly impact the signal rise time. For small termination resistances, the signal will rise rapidly, and there will be overshoot and ringing.

For this circuit, the 0-ohm impedance has a rise time of about 1 nanosecond. When the termination resistance matches the characteristic impedance as well, the rise time will be fast, but there will be no overshoot and ringing. For this circuit, the 50-ohm impedance has a rise time of about two nanoseconds. For very large impedances, the undershoot decreases the rise time. In this case, a 100-ohm impedance has a 6-nanosecond rise time. In the next slide, we will see how rise time relates to RF emissions.

Here are the radiated emissions measured with RF sniffer probes. The emissions for the circuit on the last page were measured with 0-ohm, 50-ohm, and 100-ohm terminations. Increasing the termination resistance will increase the rise time, which will decrease the RF emissions. The rise time is 1 nanosecond, 2.2 nanosecond, and 6 nanosecond, for 0 ohm, 50 ohm, and 100 ohm, respectively. For a 1-nanosecond rise time, the peak is minus 15 dBm. For a 2.2-nanosecond rise time, the noise decreases to minus 20 dBm, and for a 6-nanosecond rise time, the noise decreases further to minus 35 dBm. Thus, the overall noise decreased by 20 dB or a factor of 10 by simply changing the termination.

One last thing to consider regarding termination impedances-- the termination impedance should be near the driver for best impact. The goal is to match the impedance discontinuity at the output of the gate, not at the end of the transmission line. Remember, the receiver is a high impedance. So placing a termination in series with an open circuit isn't helpful. In this experiment, we compare the overshoot and ringing when the termination is placed on the correct and wrong side of the line. The measured results show that placing the termination on the wrong side of the line more than doubles the overshoot. So please be careful to place the termination near the driver.

That concludes this video. Thanks for watching. Please take the quiz to check your understanding of this video's content. Question 1-- which is not a factor in determining PCB trace impedance? The correct answer is a-- trace length. The trace with dielectric thickness and dielectric materials are the only factors that are needed to set the impedance. Question 2-- what problem will occur if a transmission impedance is too small?

The correct answer is b. The signal will have overshoot and ringing. Question 3-- what are some issues that you would expect from mismatched impedances? The correct answer is e-- all of the above. Impedance mismatching can cause overshoot, crosstalk, RF emissions, and data communications errors. Question 4-- true or false? The termination resistance can be placed anywhere on the line for impedance matching. The correct answer is b-- false. The termination resistor needs to be placed near the driving gate. That's all for today's video. Thanks for watching.