PCB Impedance Question

If a manufacturer prints the following regarding their PCB impedance data, what exactly do they mean? The trace length itself cannot be 50ohms, but why would it be 50ohms to ground? Would that mean through a via?

A layer (1) single free standing copper track (a micro-strip) of 0.40 mm width will have an impedance of 50 ohms with respect to a solid copper ground plane on layer (2).

Impedance means a complex value
Z = R + jX, where X could be capacitive or inductive reactance.
So "50 ohm" impedance does not mean "resistance" as you can measure with an ohmmeter.

Ah, of course - the joys of complex numbers :astonished:

Thanks!

The 50 ohms is the "characteristic impedance" of a transmission line. For digital computers, a square wave will travel on the PCB copper trace with a speed that is similar to a light beam in glass. It is slower than light in a vacuum

The impedance is determiined by the inductance per unit length and capacitance per unit length

Z = sqrt(L/C)

The speed of signals is

v = 1/sqrt(LC)
similar to speed of light
c = 1/sqrt(eu)
where e is permittivity and u is permeability

You may have a top pcb 20mil trace 5 mm long, shorted to bottom's ground plane via a single via, and its impedance could be 80ohm (at few GHz for example).
Z = 0.0000001 + j80
So the impedance is "inductive" - it means the "via" behaves as a small inductor - that is important when you want to ground a decoupling capacitor though a single via for example, thus you must consider the physical sizes and material properties as well..

Lots of things to consider at higher frequencies! Ran into this issue with a GPRS board I made... had to go to a thinner FRP design than usual (1mm vs. 1.6mm thickness) to accommodate the microstrip requirements of the cell phone antenna. Also consider grounding and EMI carefully - I tried and appear to have succeeded. It took a while, but the board has a almost continuous ground plane except for things like the SPI pin headers, for example.

pito:
You may have a top pcb 20mil trace 5 mm long, shorted to bottom's ground plane via a single via, and its impedance could be 80ohm (at few GHz for example).
Z = 0.0000001 + j80
So the impedance is "inductive" - it means the "via" behaves as a small inductor - that is important when you want to ground a decoupling capacitor though a single via for example, thus you must consider the physical sizes and material properties as well..

No, in this case, Amilobe is correct. The manufacturer is talking about a traces impedance as a section of a transmission line. This does depend on frequency (within limits), that trace should remain a 50 ohm impedance transmission line at 1MHz or 3GHz. It is called a stripline or microstrip.

http://www.ti.com/lit/an/scaa082/scaa082.pdf

So if you feed one end with a driver with a 50 ohm impedance, and the other end is connected to a receiver with 50 ohm input impedance, the result is no reflections and an SWR of 1:1, not dependent on frequency or length of transmission line trace.

TX-Line is a super handy free tool for calculating trace impedance…
http://www.awrcorp.com/products/optional-products/tx-line-transmission-line-calculator

And the solitary genius who first understood transmission lines (and many other implications of
Maxwell's equations) was Oliver Heaviside. He worked out that you could add regular load inductors
to telegraph wires to allow them to carry information much faster, invented the coaxial cable,
invented iron-cored copper wire for increasing distributed inductance, invented a practical
duplex telegraph circuit for long distance (IIRC), reformulated Maxwell's 20-or-so equations
into the modern 4 vector calculus equations (Hertz also did this independently I think), codiscovered
the Poynting vector...

He is much underrated in my opinion:

Note that he invented the terms impedance, reluctance, admittance, permeability, conductance, inductance....

A line characteristic impedance is a theorical impedance so it is always real.
If at one end an impedance controled line is correctly matched by is characteristic impedance , on the other end the actual impedance is also real.
It is for this property they were invented.

If it is not matched, the actual impedance could be complex, capacitive or inductive depending of the line lengh.
Unmatched a controled impedance line is also dangerous in analogic than in digital, depending of the higher frequency and the complexity of the design.

PCB
FR4 is a "Flame Retardant" norm, not an electronic norm, so with high frequency (>500 MHz) the same design will have different behavior with two PCB from two different FR4 manufacturers diffrence with epoxy resin).

"A line characteristic impedance is a theorical impedance so it is always real."

Nope, if the resistance or conductance per unit length are non zero, the characteristic impedance is complex.

While Heaviside's compensating inductors were good in the short term, they were real headaches and had to be removed when they wanted to extend the bandwith of the lines.

Nope, if the resistance or conductance per unit length are non zero

You are right if the line have big losses but everything is a matter of proportion.
Generally we use properly the materials and losses are sufficiently low so the line can be considered as perfect and Zc can be considered as real.
If losses are high, effectively there will be reactive term, but really what's the utility of using lines of poor quality?

There's a lot of very informative theory being described here. Makes me want to read Heaviside's biography, :-). But what are the practical implications for OP laying out a PCB? When should he worry about the effective impedance of his traces? Probably not of major concern on boards with Arduino chips. ????

I went to a talk once that talked about negative index of refraction materials, in other words, instead of a series-L, shunt-C it is a transmission line based on series C, shunt L:
http://www.mwlab.ee.ucla.edu/publications/2003c/FC3_01.pdf

oric_dan:
There’s a lot of very informative theory being described here. Makes me want to read Heaviside’s biography, :-). But what are the practical implications for OP laying out a PCB? When should he worry about the effective impedance of his traces? Probably not of major concern on boards with Arduino chips. ???

I guess high speed USB signals - ensuring equal length, number of vias and trace routing are the big issues for me.

Long PCB traces need termination for impedance matching. To define "long" see:
http://www.altera.com/literature/an/an315.pdf

see page 26
The designer should know the following :

risetime of signal (like 300ps) = Tr

bandwidth = 0.35/Tr = 1.16Ghz example frequency is bandwidth

speed of signal 5.5 Giga inches per second

wavelength = speed / frequency

if your PCB trace is longer than wavelength/10 use termination

CONCLUSION
For short traces, no termination is needed.