How to measure propagation velocity through a trace on a pcb?

Question

With a pcb in hand, how to measure the propagation velocity of a path from point A to point B, with accuracy in the picoseconds range?

Answer 1

To do this measurement, there are two well-established methods:

TDR

Apply a pulse input (either the rising or falling edge of a square wave), and measure the time for the edge to propagate to the far end of the trace. The delay measurement is done with an oscilloscope, and high-end oscilloscopes have TDR plug-in modules available to automate this measurement.

Key requirements for your measurement equipment is that the pulse source should have a very fast rise time, and the cables connecting it to your system under test should not slow the edge down too much. The oscilloscope must have sufficient trigger accuracy and timebase resolution to measure the arrival time with the accuracy you want.

Group Delay

Use a vector network analyzer (VNA) to measure the phase response of your trace. The group delay (derivative of phase with respect to frequency) gives the propagation delay through the trace at each frequency. You'll be interested in all the frequencies contained in your signal under normal use, so for digital signals that would be from some low frequency determined by your coding scheme up to a high frequency determined by the rise and fall times of your edges.

In this case the quality of the stimulus is less critical than in the TDR case, but you do need to carefully calibrate the VNA and interconnecting cables on a daily or half-daily basis, using a quality calibration kit, to be sure of getting a meaningful measurement.

More difficulties

If your traces are layed out as tightly-coupled differential lines, you would want to do these measurements using differential stimulus and measurement. Unfortunately, appropriate gear to do the measurements differentially is not widely available. If your traces are single-ended, or differential but layed out as uncoupled lines, then a single-ended measurement is appropriate.

Also, as Mazurnification points out in his answer, how you connect your test gear to the traces is critical. If you can arrange to test between two connectorized ends of the trace, that's the best. If you are trying to test traces between chips on a populated board, that's almost impossible. If you have an un-stuffed board, you may be able to connect to it with some kind of probes. But more likely you will just build some test coupons onto the panel with your boards that let you connectorize traces of the same geometry as the ones you are worried about.

Answer 2

This answer is mainly re calculation.
Measuring is easier :-).

Any answers you get from anyone here will only be the first step on a highly technical journey. The basic answer is "about 6 inches or 150 mm per nanosecond. The longer answer is ...

In free space a nanosecond is close to a light foot or about 300mm, so a picosecond is about 0.3mm & 10 picoseconds is about 3mm. The word "about" tends to feature a lot in this sort of magic delvings so if any sentence doesn't have an "about" in it just assume it has been said. Depending on various factors such as those below and others, the on PCB propogation delay will be from 10% to 50 % to ???% slower so delays of say 1 to 2 times typically are seen compared to free space and longer would be no surprise.

There are tables available that give approximate propogationn delays (PDs) dfor various PCB materials and track topology so you can start with a rough guess of

• Delay = 3.5 x k x length_in_mm picoseconds.

  • Where k is a board-material / track / topology velocity factor.

If you have a PCB in hand as you say, them the very very best method available is to measure it under the real world conditions of your choice.

Failing that, the next best method is to use one of the available calculators which perform this task for you. As the answer depends on track width and to some extent, thickness, presence and relationship of other tracks (parallel on same plane, parallel on other side of this layer, nearby, crossing, ... and groundplanes, PCB material, vias and other structures, stubs and components along the way, .............. for a start, then a PCB design program that allows the actual circuit and environment to be modelled is desirable.
Programs like Altium's PCB suite include this capability as of right.

Finally, you can try to calculate it yourself after having done adequate study. Good luck.

Tracks at frequencies where picoseconds matter will act as "microstrips" - dielectric affected transmission lines. So ...
Wikipedia - Microstrips

Also Wikipedia - Transmission line

---

Useful Microstrip Propagation Times - Slower Than We Think - Excellent discussion. He wants to sell you UltraCad's services :-).

Ultracad home page

Various software PCB design tools from UltraCAD - some free, some not. Free ones are of limited use to you.

---

APPCAD - free ex Agilent RF & Microwave design program.

Well spoken of program - helps to thing your PCB is a bit of microwave circuitry - which it is.

APPCAD V3.02 here

Olde !!! APPCAD version that runs undr DOS and not windows {fwiw}

---

RFSIM99 S parameter simulator. When the easier magic doesn't work download here

---

Very good user discussion here

Some gems from above

• So for example, nominally 50 ohm microstrip on er=5.0 substrate yields about 1.56e8 m/sec propagation velocity; er=4.5 makes that 1.64e8, and 4.0 makes it 1.73e8. (Different calculators will yield slightly different answers, but the variation as a percentage should be very close.) So a 20% reduction in er made for about a 10.9% increase in velocity.

• That was for a trace width that stayed constant; if the trace width is adjusted to keep impedance constant, the percentage in propagation velocity is slightly less. For stripline (embedded in a constant er), the velocity variation over the same er range is about 11.8%.

• Note also that there is some variation in velocity as a function of frequency...it's not huge, but it's there.

• It will help a lot if you specify a particular substrate material. "FR4" doesn't cut it; "Isola 370HR"

&

• FRF-4 is pretty inconsistent, and its capacitance TC is remarkable, ballpark 950 PPM. If you need tight prop delay spread, you'll need a better laminate.

---

Useful Fundamentals of SI (Part 2) – Transmission lines
He essentially concludes that the rule of thumb speed is half light speed or K=2 in my formula.

---

Why you may care Interesting discussion of PD effect & design with high speed processors

---

EMC design for high speed PCBs. Related here

---

Some good refs in thus user discussion here

---

$40 book - but what a good title :-)
High Speed Digital Design: A Handbook of Black Magic - Howard W Johnson - author is an acknowledged grand master of the art.

Answer 3

Use good signal source (function generator) and good sampling or real time scope together with two good active, correctly calibrated, well matched to the trace probes and you are good to go. The precision that you are asking for is well within higher end test equipment capabilities (read as both relatively new and expensive).