question about transmission line on PCB

[CQCQ]

Hi,If I have a PCB with 10cm long ， 8cm wide ,Working freq 200MHz.MUST I consider the track on the PCB as transmission line? If not can I make the track with any width dont care about the track's characteristic impedance(width，thickness）?

Thanks in Advance!

-CQCQ

 

[Yahia Muhammad]

200MHz is quiet low i think it should be considered above 300 MHz the wave length in your case is 1.5 meters
so in my opinion it's not necessary

 

[rfmw]

Operating frequency doesn't mean much if you have digital (squarewave) signal. What matters in this case is the rise/fall time of the digital signal.

If 10cm is still acceptable I think depends on your circuit and system...

 

[mfarhan1]

with Er of 2.2 and 10mil thickness the guided wave length would be about 1meter. so with 10cm the phase of signal would change only 36 degress approx if you are not concern with phase applications then you can ignore this and use the lumped equivalent instead of distributed.
for impedance it is changed with in few mm with different Z0, so i recommend you should measure the width of track equal to system impedance

 

[radiohead]

I agree, but all depends on the substrate material you use (FR4 or other), it's loss at higher frequencies, the thickness of the layer.

A general rule is that high-frequency interconnections should always be kept as short as possible, unless you want to add shielding and foresee physical separation for better isolation.

 

[madengr]

What is terminating either end? You don't want a high impedance output drive a wide, capactive line. Nor do you want a low impedance driving a thin, inductive line. I'll assume your source and load are 50 ohms. RF is not the only discipline affected by trace impedance. Precision, low noise analog design is affected too.

 

[House_Cat]

Hi,If I have a PCB with 10cm long ， 8cm wide ,Working freq 200MHz.MUST I consider the track on the PCB as transmission line? If not can I make the track with any width dont care about the track's characteristic impedance(width，thickness）

As you may have concluded from the "mishmash" of answers, your question doesn't include enough information about your application.

Every trace on a PCB is a transmission line. Each trace has inductance and capacitance. How significant to your problem that may be depends on the signal that will be present on the trace, and the proximity of the trace to other traces and/or a reference plane.

What is the nature of the signal on the specific trace(s) you are concerned with - i.e. is it a digital signal with a 200mhz clock rate, a sine wave, or...? If it is a digital signal, what is the edge rate? What two components are connected by the trace in question - what are the input/output impedances?

If your signal is audio, then the impedance of the trace is immaterial. You are concerned only with inductive or capacitive coupling to other traces and structures on the board. Make the trace any width you want as long as you keep in mind the issue of direct coupling and possible signal return coupling (so-called ground loops).

If your signal is DC, you are concerned with intermodulation of the DC between the different components supplied by the trace. Decoupling capacitors and trace width are used to treat that sort of problem.

If your signal is a digital signal, then the impedance of the trace matters. Mismatches cause reflections and energy loss in the signal edges. For a digital signal, the edge is where the information is carried. If you mess up the shape and amplitude of the edge, your data is messed up. Timing is also affected since the shape and amplitude of the edge determines when, or if, the next stage gets triggered.

If your signal is sinusoidal RF, then the impedance of the trace matters. Again, reflections affect the size and amplitude. In sinusoidal RF signals, the data is in the phase and/or amplitude of the signal. If you screw up the shape and amplitude, you have screwed up your data.

For both sinusoidal signals and digital signals, if you mismatch impedance you also run the risk of radiating directly from the trace to the surrounding environment. If the energy is not efficiently coupled from the source to the load, then the energy can be coupled to free space.

The only general answer that can be made to your question is that, usually, you want to match input and output impedances to give the best signal integrity. Impedance matching requires that you keep in mind the width of the trace, the dielectric properties of your board material, and the distance from your trace to the return path for the signal propagating on your trace (typically an underlying solid plane).

Supply more information about your signal(s) and a more specific answer can be given.