Characteristic impedance in PCB

[joniengr081]

I am learning characteristic impedance on PCB traces. So far I have learned that characteristic impedance depend up on the width of the trace, height of the signal layer to the reference plane, and also on the dielectric constant. I don't see anywhere they said that characteristic impedance depends on the frequency of the signal travelling on the traces. Is that true characteristic impedance does not depend upon the frequency ?

[T3sl4co1l]

In an ideal transmission line, yes.  Varying Zo is called dispersion, and comes with losses or change in velocity factor.

Lossless stripline traces are such an example.  Practical coax is very close indeed.  (Note that coax and stripline are effectively the same thing, on a basic level: an inner conductor surrounded by an outer conductor, with dielectric between; the shapes of the conductors is irrelevant to propagation below waveguide cutoff.)  Practical stripline on FR-4 is pretty good up to a GHz or so, and notably lossy near or above there; special low-loss dielectrics are available to solve that if required.

Microstrip traces are a counterexample.  Even if the dielectric is lossless, there are two additional effects: 1. the wave partly propagates in air above the board, at higher velocity factor; 2. the wave has a nonzero component at infinity, i.e., it radiates (which is also a loss component with respect to the intended propagation along the trace).  The amount of radiation from practical microstrip is normally quite small (parts per thousand?), small enough we can ignore it for digital signal quality purposes (and that substrate and conductor losses are much worse than radiation), and small enough that, at typical signal levels (a few volts for single-ended CMOS, used usually below 100MHz or so; or fractional volts for differential e.g. LVDS and such, up to 10s of GHz), the radiation is near or below acceptable levels, even for a bare unshielded board.

Note that losses don't necessarily cause dispersion; when dielectric and conductor losses are balanced, a wave (e.g. step change in voltage) remains together, and just attenuates over distance.  Typically, conductor loss is worse, and dispersion does occur (consider coax, with the modestly-low resistance copper conductors, but extremely low loss PE dielectric, or even foamed PTFE, or (mostly) air for special hardline types); this can be balanced with loading coils at regular intervals (which reduce velocity and increase Zo, such that the reactive and resistive aspects of the line are brought into equal proportion), which is basically how the first transatlantic telegraph cables, and later for voice and data, were designed -- such a long route cannot preserve even slow (hand-tapped) Morse code with a plain coax design, but with loading coils integrated, bandwidth is extended to, ~kHz at least, with I think the last analog cables topping out at 10MHz or so.  (By the 1980s, only fiber-optic cables were being installed, which still contain repeater amplifiers and various frequency compensation tricks, but the fidelity is generally much better, and the bandwidth far greater of course.)

Tim

[joniengr081]

I also checked that characteristic impedance does not depend on length of traces and does not depend on the frequency of the signal. Interesting to know.

[joniengr081]

Regarding losses in transmission lines. There are two types of loses, one conductor losses and the other dielectric losses. They both are frequency dependent. IN FR4 these losses appear at GHz range. Below a certain frequency the conductor losses are more then dielectric losses but above that frequency, normally above 5 GHz in typical FR4, the dielectric losses dominates.

[ahbushnell]

The problem with FR-4 is the dielectric constant is not controlled.  So the impedance can change from board to board.  There are board materials that have controlled impedance.  They cost a little more then FR-4.  Note the cell phone in your pocket probably has this material. 

[joniengr081]

I have heard about Rogers and Magtron. I don't know how much expensive they are compared to FR4. Anyone has idea ? Which material is used in mobile phone PCB ? and whats the cost ?

[Doctorandus_P]

I also checked that characteristic impedance does not depend on length of traces and does not depend on the frequency of the signal. Interesting to know.

Transmission lines are generally much longer then the wavelength of your signals. They are often simulated as a lot of series inductors, combined with a lot of capacitors to GND. The signal energy is than transferred as a wave from capacitors to other capacitors  down the line though the inductors. That means that your signal only sees a very small portion of the transmission line at any given time. If you have fast digital signals, such as for example the (already slow to modern standards) 100Mbps Ethernet, then each bit is less then 3 meter long. This means you can hundredths of bits in a long cable before the first bit comes out the other end.

And about the prices of more exotic PCB materials. It's difficult to say anything decent about that. Price will change a lot combined with other factors such as amount of layers and the number of PCB's ordered. Just the simple fact that they do not fit in the cheap pooling services very likely makes them a lot more expensive for prototyping. Costs of PCB's goes way down when you start ordering in the multiple hundreds of PCB's.

A trick sometimes used for FR4 is to route signals slanted over the PCB. This way none of the tracks are exactly above or in between glass fibers, and this improves signal propagation delay uniformity.

[EEEnthusiast]

The value of Er itself is not constant across frequencies. So the Zo is also bound to vary with frequency. At very high frequencies, the surface roughness , conductor losses and the dielectric losses makes the Zo itself a complex number.
May be up to few 100MHz, the Zo can be assumed to be fairly constant.
As an example, have a look at the material properties of Isola 370HR, a popular FR4 variant.

https://www.isola-group.com/wp-content/uploads/data-sheets/370hr.pdf

[joniengr081]

Can we calculate at which clock frequency, the wavelength is smealler then 1, 5, or 10 inches long transmission line ? Then there would be several wavelength or cycles in the transmission line.

[nctnico]

The rule of thumb I learned is that if the length of a conductor is less than 1/10 of the wavelength, you don't have to consider it a transmission line.

[dietert1]

The FR4 dielectric constant is known to some degree and this should be good enough to do an estimate.  Recently i used a digi-key online calculator and tried to make the pair impedance about 100 Ohm. If it comes out as 80 Ohm or 120 Ohm, no problem. I mean if the leading edge of a digital signal overshoots 20 % that will work. Same if 20 % is missing.
I did the estimate to get it about right. At least it helped me to select one of two 4-layer stacks offered by the PCB house.

Regards, Dieter

[Doctorandus_P]

Can we calculate at which clock frequency, the wavelength is smealler then 1, 5, or 10 inches long transmission line ? Then there would be several wavelength or cycles in the transmission line.

Sure, there are formula's for that. I think it's between 50% and 80% of light speed (in vacuum) as a rule of thumb but it depends on dieelctric constant and maybe also on track geometry. I don't know the details, but I'm sure there are formula's for that kind of stuff.

[luudee]

Interesting thread ...

It just happens that we switched PCB houses, and are now using "WellPCB".
Since one of the PCBs we make uses Megtron-6, I asked our sales rep @WellPCB
for relative cost of the various materials that are recommended for "high-speed"
PCBs. I asked her to use FR-4 for as base.


normal FR4                                 1.00
Shengyi S1150G Halgon-free     1.36
Isola 370HR                                2.07
TU872 SLK                                 3.43
Megtron6_R-5775                       5.64


Hope this helps.


Best Regards,
rudi

[joniengr081]

I was reading a comment which says that one problem with FR4 is that the characteristic impedance is not constant which is due to change or un-stable in dielectric constant. What is the tolerance level of dielectric constant in FR4 ?

Second question regarding FR4 comparison cost wise with other dielectric for example Rogers, Isola, Megtron-6 etc. If the price of the dielectric is 2 or 3 times then it does not mean the overall cost of the PCB is 2 or 3 times, right ? because it's only the cost of dielectric.   

[luudee]

I was reading a comment which says that one problem with FR4 is that the characteristic impedance is not constant which is due to change or un-stable in dielectric constant. What is the tolerance level of dielectric constant in FR4 ?

Second question regarding FR4 comparison cost wise with other dielectric for example Rogers, Isola, Megtron-6 etc. If the price of the dielectric is 2 or 3 times then it does not mean the overall cost of the PCB is 2 or 3 times, right ? because it's only the cost of dielectric.   

Please see my post above.

Those are actual PCB prices. According to my rep, Megtron-6, is actually 5.6 times more expensive plain than FR-4.

Cheers,
rudi

[joniengr081]

Yes, I saw that it's the overall production cost. How do we compare their dielectric constant tolerances ? Which dielectric material has smaller tolerance of dielectric constant compared to FR4 ?

[nctnico]

I was reading a comment which says that one problem with FR4 is that the characteristic impedance is not constant which is due to change or un-stable in dielectric constant. What is the tolerance level of dielectric constant in FR4 ?

A much bigger problem with FR4 is that the glass weaving pattern isn't constants which results in changes of the Er. So if you need to route differential pairs which have signals over a couple of GHz, you better make sure to run them at a 45 degree angle in respect to the weave pattern to even out the influences of the weave pattern.

[rfclown]

You can Google and find the datasheets for Megtron 6 and Isola materials. We've used Megtron 6 and Isola 408HR at work. You are paying the price for a company (Panasonic or Isola) that is making a controlled material. Something like FR4 is not so controlled, and on top of that a PCB house may have a mix of material from different places. I you aren't paying for control, you don't get it.

I've used OSHPark for a board with Isola 408HR. They offer a 4 layer controlled impedance stackup for a low low cost (at least it seemed reasonable to me). Go to their site and compare prices of the various stackups. JCL does this as well. Both of these places are hobby friendly, and you can see the price differences.

[Doctorandus_P]

There are also quality differences for FR4.
Some 10+ years ago there were experiments with different sort of weaves and spreading (pressing) the weaves to make them more even. But I don't know where those experments went and whether the results were sufficient.

[T3sl4co1l]

AFAIK, they never rotate by fractional turns, and at that rarely if ever rotate at all.

Tim