At what frequencies does PCB design get tricky?

Question

I have designed many mixed-signal PCB's where the highest-frequency component is the microcontroller's crystal oscillator itself. I understand the standard best practices: short traces, ground planes, decoupling caps, guard rings, shielding traces, etc.

I've also put together a few RF circuits, at 2.4GHz and ~6.5GHz ultra-wide band. I have a working understanding of characteristic impedance, ground stitching, balanced vs unbalanced RF feed lines, and impedance matching. I've always contracted an RF engineer to analyze and fine-tune these designs.

What I don't understand is where one realm starts to cross over into the next. My current project has a 20MHz SPI bus shared between four devices, which has let me to this question. But, I'm really looking for general guidelines.

1. Are there guidelines as far as trace length vs frequency? I assume that ~3 inch traces are fine with 20MHz (15 meters), but what is the general case?

2. As frequencies increase, how to prevent long traces from radiating? Are striplines and coax the way to go?

3. What is the RF characteristic impedance of a typical microcontroller output stage, anyway?

4. etc.

Please feel free to tell me anything I'm missing :)

Answer 1

1. Trace length versus frequency - for sending data or carrier waves between one IC and another, the guidelines are fairly tolerant I'd say. The maximum frequency that could be generated in significant amounts (maybe up to several harmonics for a square wave) is the limiting factor and if your trace length is "less-than" one-tenth of the wavelength then you probably don't need to operate with a terminator. Even at slightly longer trace lengths you could terminate with a series combination of a few tens of pF and (say) 50 ohms. This avoids the problem of a 50 ohm terminator directly across a logic line. For different circuits the "rules" are more stringent for instance, a photodiode amplifier might have a 3dB bandwidth of 1 GHz (wavelength = 0.3 m) and one tenth would be 30 mm - a totally disastrous trace length on the input to a photodiode amplifier and also the inductance of the line would cause all sorts of hidden surprises when trying to get it working. So rules change depending on what you're trying to do.

So I'm making a distinction here between robust digital (or analogue) transmission, sensitive/feeble circuits like photodiode amplifiers and I'll use your 6.5 GHz UWB as an example - it may have had broad tuning across a couple of GHz but if you were trying to make a linear amplifier from the kHz to GHz range you will hit problems on trace length inductance resonating with parasitic transistor capacitance and sometimes you have to put resistors in very small tracks just avoid a circuit self-oscillating. With my "radio head" on what you can achieve at really high frequencies (but limited bandwidth) means you can utilize parasitics to your advantage but not so across a really wide bandwidth from DC to several GHz. That's how it tends to pan-out for me anyway.

1. Prevention of long traces radiating can be done with balanced traces - the far field is zero because the two EM fields cancel out (when done properly). Using striplines is a technique and doesn't itself stop a signal radiating. Coax does of course and so does balanced stripline.
2. Micro output impedance isn't as relevant as you think in a lot of examples - say it is 10 ohms at 100 MHz - your output goes down a 50 ohm stripline (or coax) and providing the termination at the receiving end is adequate, reflections are minimized. I know at college they say your output needs to be impedance controlled but in reality it doesn't.

Answer 2

1. Are there guidelines as far as trace length vs frequency? I assume that ~3 inch traces are fine with 20MHz (15 meters), but what is the general case?

At my work, the guideline is, if the electrical length of a trace is longer then 1/10 wavelength, you need to treat it as a transmission line. At a minimum, this means you must terminate with a resistor matched to the impedance of the line. How do you figure out what resistor value to use? You estimate what the impedance will be during design, and then you adjust the value to minimize ringing during DVT.

Now, there is some subtlety here about the true meaning of 1/10 wavelength. For a sinewave, this is straightforward. For a square wave, which is the sum of many sines, you must use highest frequency component as your estimator. As you sharpen the corners of the square with a faster slew rate, you increase the frequency of the fastest sine competent.

What this means is, for a digital signal, drive strength directly affects the electrical length of the line. Higher drive strength can easily turn a line that does not ring into one that does.

I learned this the hard way when a supplier made an "improvement" to a digital buffer without telling us. This change increased the slew rate, which caused ring so bad that the receiving chip started to latchup. A board we produced that had been working fine for years suddenly started randomly locking up.

Answer 3

You are asking a good question. In many ways the same question as this one: What types of signals should be considered to have a 50 Ω trace impedance?

I won't repeat my answer here, but suggest you go read it there. This should cover your 1).

2) Don't worry about traces radiating if you run over a reference plane. Worry instead about when the signal leaves the low impedance realm near the reference plane. Connectors, cables, etc.

3) Use your favorite IBIS simulator to find this. And it is important for termination. Most are in 10-25R range - but you may even find some that are asymmetric, so the high side and the low side output FETs are not giving you the same impedance.

Answer 4

1) Are there guidelines as far as trace length vs frequency? I assume that ~3 inch traces are fine with 20MHz (15 meters), but what is the general case?

Dimensions > 1/10 wavelength of the highest frequency or harmonic. That doesn't mean the circuit will stop working at 2/10 wavelength. It depends how sensitive the circuit is.

2) As frequencies increase, how to prevent long traces from radiating? Are striplines and coax the way to go?

There are different rules of thumb depending on what you're concerned the trace will radiate to. An RF circuit will always radiate. Picture the signal being guided by the trace, not existing inside the trace. The signal on one trace can jump onto another trace if they are close enough. Most people call this coupling. To minimize coupling, separate traces by at least 2*(distance to the reference plane). A wall of vias can be used to ensure two traces are isolated from each other.

There are a few rules of thumb to minimize how much a traces radiates out of the circuit and goes somewhere else. - Make sure all traces are terminated into something. A 1/4 wave trace makes a decent antenna, if one end is open-ended. - Avoid discontinuities. Think of a trace as a highway. If you're going 70mph and hit a 90deg turn, you're not going to be able to follow the road. The same is true with high frequency signals.

If a signal does radiate away from a circuit, it can be contained with a metal enclosure or absorbed. Stripline and coax both have metal that contain RF signals. Boards without a solid top metal layer are usually covered with a metal enclosure. The distance from the board to the metal enclosure is usually made less than 1/2 wavelength to attenuate radiated signals and avoid other weird things from happening. You can also buy materials designed to absorb RF signals, so they don't bounce all over the place.

4) etc. There are fun games you can play by changing the thickness of your traces or the distance to the reference. A wider line effectively looks shorter, but a narrow line looks inductive and can be used to cancel capacitive devices.