Propagation delay in PCB traces

The theory is easy; getting the numbers to plug into the theory isn't.

Your propagation speed would depend heavily on the material properties of the substrate, and those would depend on a bunch of variables that have little to do with basic physics.

Two ways that I can think of to approach this are to dig around and see if you can find expansion coefficients and permitivity variations with temperature for your brand of substrate then do some calculations (which you won't be able to believe until you do measurements), or see if you can get the specs relating to building microstrip filters on your PCB -- the microstrip filters are basically tuned by the filter dimensions and the propagation speed in the PCB, so you should be able to back velocity variation out of frequency variation fairly easily.

You can run something like Appcad and see how sensitive your traces are to various things: trace width, dielectric constant, dielectric thickness. You can get a PCB house to control these as needed, for money. You cpuld also get a good pcb house to control prop velocity itself, for more money.

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

John

Thanks John. It is on a Rogers material. I am looking at Appcad now, it is quite nice. Never heard of it before. A well kept secret of pros, I guess. I will read up on all relevant parameters of Rogers and see where this leads me.

And you're going to put 75A down a PCB track?

Uh, what? Wrong thread maybe?

RFSim99 is another freeware program that's useful for playing with things like this; it has a built-in microstip and stripline calculator.

You didn't elaborate on just why you care, but I'd suggest that for most things, it's not going to matter much at all, and if you want things to be seriously stable, you should probably in any event arrange to have board effects cancel out in some way: autocalibration, use of matched traces so it's the differential that matters, not the absolute propagation, or things like that.

But at the same time, the physics helps out some: propagation velocity depends on the effective permittivity that the fields are traveling through, and propagation velocity varies as the square root of that. Not only that, but the dielectric for microstrip is partially air, which doesn't vary much. 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

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" (for example) will get you much more consistent results, and you can search for substrate materials which are particularly stable and whose manufacture is well controlled. Consult with your board fab house about this!

Cheers, Tom

Thanks, in any case the widest swing seems to come from the variability of the Er of the material, which is 3.36 +- 0.05, about +-

Yes, that should be the case. If the transmission is embedded entirely in a dielectric of relative permittivity, Er, and the magnetic permeability is the same as freespace, and the line is run in TEM mode, then the propagation velocity is 1/sqrt(Er) times the freespace propagation velocity. It doesn't matter what the dimensions are (so thermal expansion has no direct effect), or what the line impedance is. For microstrip, the fields aren't completely inside the Er of the substrate; some are in the air above the board. Thus the propagation velocity is slightly faster, the mode isn't true TEM, and there's some dispersion. See, for example,

I'd expect Er to vary with temperature, with frequency, with absorbed moisture, ... (Note: Er of air is slightly greater than 1, and changes with pressure, temperature, humidity, ..., enough to be noticeable if you are monitoring part per million changes in capacitance of air-dielectric capacitors.)

Cheers, Tom

One tough application I ran into is doing PCB's for radar detectors, you know those do-dads speeders use to detect cop radar. In place of 90 degree track turns is a curved radius to prevent radiation. I suppose at a 1 cm wavelength track length needs to be accounted for too, because of phase.

I think I'd start with a computer (numerical analysis) sim, and see how it works. You can build in provision for slight tweaking to refine it. Ken

No theoretical base possible. Every company has their own manufacturing process in making a given board type/spec, and there are always process variations which may affect prop delay VS temperature, trace direction on PCB and certainly (by definition) batch. Impossible for generic modelling as seems to be given. Glass weaves will affect signal dispersion VS frequency, and that may quite different in different directions on the board due to the weave itself. Epoxy formulations have their own variations, so one must be rather eXplicit regarding a given manufacturer and type/formulation.

Also look at Matsushita Electronic Materials' Megtron products..some are variants of Getek that have been formulated to compete with the Rogers RF products (hint: Matrix).

Maybe via vapor phase electron transport, AKA plasma...

I suspect that the curved traces were perhaps more to prevent impedance bumps than to prevent radiation? 90 degree turns have excess capacitance on their corners... at microwave frequencies these are generally chamfered or rounded to remove this.

I'd be quite interested in knowing some cheap techniques for adjusting propgation delay along, e.g., a microstrip trace with the ability to tune a couple hundred ps or so over frequencies up to a handful of GHz. Possibly just having a "fat blob" on the trace that could be trimmed with a Dremel tool? I.e., it's small enough that it doesn't affect return loss much but the excess capacitance slows everything down a bit?

---Joel

On Aug 20, 9:40 am, "Joel Koltner" wrote: ...

Do you really think it's going to be practical to tune the equivalent of an inch or two of propagation with something like a "fat blob" that's small enough to not mess things up at a few GHz?

How about some line sections in a binary sequence of lengths that could be patched in or out, depending on where shorts were placed?

Or maybe just design things so the effect can be calibrated out...

Cheers, Tom

I'm not certain, but I do know that it's feasible to trim matching networks for GHz-range power amplifiers with well under 100fF "steps" using a Dremel tool to carefully eat away "chicken pads."

The problem is that getting adjustment down to, say, 5 degrees steps at 3GHz is under a millimeter -- hard to switch anything that short on a PCB (although on an IC, no problem). On the other hand, with some careful technique I imagine a Dremel tool can be used to eat off not more than, say, 100um at a time.

If you have control of the entire box, this is certainly the way to go.

---Joel

It's more "C" than "L". :-)

A pure LC circuit doesn't (can't) cause a resistive loss in power -- it causes a reflective loss due to an impedance bump; the energy is just reflected back towards the source.

I am being a little cavalier here in that, if you have an impedance discontinuity, in general you'd expect most of the power to keep flowing in the "forward" direction, some of it to reflect back to the source, and certainly some small bits will be either radiated and turned into heat via resistive losses. (There's also some "static" amount of power stored in the near field around the trace, as with any lumped capacior or inductor.) What I'm suggesting is that of reflected, radiated, and resistive losses the largest by far will be reflected.

I was actually trying to think of broadband solutions -- several orders of magnitude.

Check out the "Irish TV aerial splitter" at

Thanks for your input,

---Joel

OK, well, go and simulate the effect of what you're imagining as a blob. But note that the width of a microstrip trace has much greater effect on its impedance than on its velocity factor. Do you really want to keep reflections low??

If you really want to significantly affect the propagation delay, you should probably be milling out dielectric so it's replaced with air, and adjusting the trace width (widening it) to maintain constant impedance. It honestly doesn't sound very practical to me. I suppose if you want to electrically lengthen a trace, you could do it by milling out under it, narrowing the trace as well, and replace the board dielectric with something with a higher dielectric constant. (I'd be laughed out of here if I even hinted at putting something like that into production!)

Let's say you change the net er around a section of microstrip from

Thanks, I like this idea! It also seems as though this is amenable to a two-step procedure: Mill out enough dielectric to get the delay correct, and then go back and widen the stripline width (copper foil tape?) to correct the impedance. While the later will slightly alter the delay (since the effective permittivity will change with the small change in geometry), I expect it'd be a small enough effect that it could be ignored. I should try some simulations here...

Our techs love to cut stuff up with Dremel tools? :-)

I am thinking low-volume, high-dollar production here, though -- not $50 WiFi routers.

Didn't you guys used to make microwave cavity filters with all the inherent tuning slug adjustment/hacksawing/epoxying business? :-)

I'm thinking it's even a little worse than what you've calculated in that the change in the effective permittivity is going to be less than sqrt(8/2.5) (since half of it air...). However, I think I can live with a lot less than a

---Joel

...

Hmmmm...well, "us guys" here have always been into things like continuous autocalibration that happens in the background while measurements are running, and even very significantly improves the measurement beyond the calibration effects. ;-)

I was thinking er=10 alumina, and WAGging that it would give a net around er=8. If you're going to all that trouble, you _could_ pile alumina over the top of the trace, too, so it's embedded microstrip... (Eeeechhhh.) But you're right -- the effective er over er=10 alumina is only about 6.5. For plain microstrip over er=2.1 solid Teflon, ATLC tells me that a 50 ohm line will be about 3.1 times as wide as the substrate thickness and have net er=1.79 and 4.46ps/mm, and 50 ohms over er=10 alumina will be about .95 as wide as the substrate thickness, net er=6.52, and 8.52ps/mm. So to get 20ps adjustment and keep the impedance constant, you'd have to considerably narrow a 5mm length and completely fill under it with different dielectric. There's gotta be a lot easier way... And if you don't narrow the trace but leave it the same width that gives 50 ohms over er=2.1 substrate, you have a section of 25 ohm line...

And this doesn't all sound terribly impractical to you??? ;-)

Cheers, Tom