# Signal velocity in PCB traces

On what does the signal velocity depend for a signal traveling through a PCB trace?

According to Wikipedia, it depends exclusively on the relative permittivity (ε_r) of the medium (well, it also depends on c, but that one is a constant), under the approximation that for PCBs, the relative permeability of the medium is 1.

My question is: Shouldn't the signal velocity be a function of the characteristic impedance of the transmission line?

My thought process is: If I have a trace that has a width change, then there will be a characteristic impedance change, and that would cause partial reflection of the incoming wave. But there is no energy absorption anywhere, so the only cause for a partial reflection can be a change in the wave's propagation speed, right?

According to the equation in Wikipedia's signal velocity page, there would be no change in velocity, since the medium is the same, so the relative permittivity remains the same.

Can someone shed some light on this?

The rules of thumb given in the previous answer are good enough for many designs. But I want to add one additional thought.

The velocity factor is basically going to be the inverse square root of dielectric constant ($$\\varepsilon_R\$$ or $$\D_k\$$) of the material the electric field around the transmission line travels through.

For stripline, this means it's essentially the dielectric constant of the circuit board material.

But for microstrip, it will be an average of the board material's dielectric constant, and the surrounding material (usually air), weighted by the proportion of the electric field that travels in each medium.

That means that if your design has both microstrip and stripline, signals in the microstrip will travel at least slightly faster than signals in the stripline.

As pointed out in the comments, it's worth mentioning that the dielectric constant of PWB material can vary in service due to factors such as operating frequency, temperature change and moisture absorption. There can also be variation at manufacturing time due to factors such as etch-back of the traces and alignment of the traces relative to the glass fibers in the dielectric.

If I have a trace that has a width change, then there will be a characteristic impedance change, and that would cause partial reflection of the incoming wave. But there is no energy absorption anywhere, so the only cause for a partial reflection can be a change in the wave's propagation speed, right?

No, that doesn't follow.

If there's a discontinuity in the characteristic impedance, then you need a different ratio of current to voltage in the line for the incoming signal and the forward-propagating signal. That means to satisfy KCL and KVL (or, if you want a more mathematical explanation, to satisfy the boundary conditions) at the place the two geometries meet, a reverse travelling wave has to be generated. Then the current to voltage ratio on the incoming line at the junction can be made to match that on the outgoing line, and all is right with the universe.

The difference in propagation velocity on the two lines, if there is one, isn't important here.

• Good point about needing to weight the Dk's based on the materials. Apr 22 '20 at 21:27
• This is a really good answer. I would be pleased if a note could be added at the end saying that the dielectric constant is only constant at a particular temperature and frequency. Variations in temperature or frequency can cause the propagation speed and impedance to change also. Upvoted already though. Apr 22 '20 at 23:08
• @Cal-linux cool. But as you probably know, this site ranks high in search results. If someone typed in "what factors affect PCB trace impedance" and the number one accepted answer didn't mention temperature or frequency variations, even as a footnote, well, that is a disservice to the world. But I have harped on this issue enough. Don't want to become tedious. Good question and have a good day! Apr 23 '20 at 1:03
• " you need a different ratio of current to voltage in the line for the incoming signal and the forward-propagating signal" has made this a lot more intuitive for me, thanks! Apr 23 '20 at 8:14
• @mox, that's what I was alluding to when I mentioned " alignment of the traces relative to the glass fibers in the dielectric." Apr 23 '20 at 19:42

If you consider the PCB trace as a lossless transmission line, the characteristic impedance $$\Z_0 = \sqrt{\frac{L}{C}}\$$ but the velocity factor is inversely proportional to $$\\sqrt{L\cdot C}\$$ (where L & C are per unit length).

So it should be possible for the velocity to change without the characteristic impedance changing, but it would require two things to change simultaneously.

It is true that if you only change the capacitance (or permittivity) then $$\Z_0\$$ changes proportionally to velocity factor. More in this 1965 paper.

• The relative permittivity will be a function of signal frequency and material temperature also. So, speed will also be a function of those things. Then there is microstrip vs stripline to consider. Apr 22 '20 at 19:51
• @mkeith for sure, and it is anisotropic in general as well. Just trying to simplify it as far as possible without losing the principles. Apr 22 '20 at 19:56
• I know you know. My comment is for others. It is because the main question is "on what does the signal velocity depend for a signal traveling through a PCB trace?" By the way I didn't realize it was anisotropic to any degree. Interesting! Apr 22 '20 at 20:34
• Which one of reasons manufactures reference a frequency when they the specify relative permittivity/Dk for a material. Apr 22 '20 at 21:24

Electromagnetic waves travel in a dielectric medium. In theory, the propagation speed depends on the relative permittivity and the relative permeability of the dielectric medium that the wave is traveling in. For all practical materials, the relative permeability is 1 so typically we ignore that, and say that speed depends only on the permittivity of the dielectric.

The formula is V = C/sqrt(epsilon)

Where V is the propagation speed, C is the speed of light in a vacuum, and epsilon is the relative permittivity. Typical circuit boards are made from a glass fiber epoxy composite called FR4.

The relative permittivity of FR4 is around 4, but this can vary with frequency and temperature.

However, for a trace on an outer layer, the dielectric is partially air and partially FR4. So for traces on an outer layer, usually an effective permittivity is calculated that tries to average the effects of the two different dielectrics. Since air has a much lower permittivity, outer layer signals are faster than inner layer signals. You can say that they will be roughly 15% faster as a rule of thumb. A detailed calculation can be made using formulas developed specifically for this purpose. But all the details need to be supplied (trace width, thickness, distance to reference plane, exact permittivity of PCB material, etc).

For inner layer traces, the speed is approximately half the free space speed. As previously noted, the permittivity in circuit board is a function of temperature and signal frequency. This is something you have to get from the FR4 supplier or the board fabrication house if you want to be extremely accurate.

FR4 is not the only choice of material. There are others, some specialized for high heat and some specialized for high frequency, etc.

Outer layer traces are typically modeled as microstrip transmission lines. And inner traces are modeled as stripline transmission lines. Searching using those terms may be helpful in further research.

• microstip →microstrip Jun 7 at 7:59
• @PeterMortensen I fixed it. Feel free to fix typos any time on anyone's posts. Jun 7 at 8:16

Consider a 100 ohm trace.

Now parallel another 100 ohm trace with it.

You have a 50 ohm trace, with exactly the same speed of propagation as in either of the originals.

• True, but I don't see where this is relevant to the OP's questions. Apr 22 '20 at 21:25
• @SteveSh it is a thought experiment which allows you to see that impedance can be altered without any effect on propagation velocity. I think it is highly relevant. Kind of like a Zen koan. Make a trace what is the impedance? Make another trace and put in parallel. What is the impedance now? Did the speed change? Now you are enlightened. Apr 22 '20 at 23:04
• Didn't need to be - enlightened that is. You could have made the same point just by changing the geometry of a single trace. Apr 22 '20 at 23:41
• The answers are not written for you. You already know the answer. The answers are not exclusively for the original poster, either. The answers are for all the people who find this question by way of searching online. Some questions become very popular search results. Apr 23 '20 at 0:06
• "The answers are for all the people who find this question by way of searching online" ...... well, plus for the OP! :‒) Apr 23 '20 at 0:30

The following is excerpted fro Dr. Eric Bogatin's "Rule of Thumb#3 Signal Speed on an Interconnect", circa 2013.

The speed of light (any EM radiation for that matter) is 186,000 miles per second, or 300,000 km/sec in a vacuum, or air. A more useful form of this for our discussion is 12 inches per ns.

When an electric field [representing the signal] travels in a dielectric material, like a circuit board laminate, the speed of light slows down with the square root of the dielectric constant, Dk. For example, in FR4, the Dk is 4, so the speed of light in most laminate materials is Keep in mind the dielectric constant Dk is the same as Relative permittivity.

• I determined this rule of thumb in 1996 or so, and validated it on an actual PCB used in a real product ;-). Apr 22 '20 at 20:48
• I believe it would be worthwhile to devote at least one sentence to stripline/microstrip. Apr 23 '20 at 0:09
• ${12 in \over nsec} \approx {30 cm \over nsec}$ for $C$ in a vacuum. Apr 23 '20 at 0:50