How does impedance control on a PCB track affects the components on the PCB ?

[indula]

I'm building a PCB which works in megahertz range that needs to be impedance matched with the measuring equipment. My question is if I added impedance control to every trace, for say 50 OHM, of the PCB will it affect the resistors and capacitors already in place and change the value seen by the other components since the traces are now 50 OHM ?
Sorry If I have misunderstood any theory behind what I'm asking since I'm newbie to the RF electronics.

 

[kubeek]

Would be best if you posted your circuit. Generally the transmission line should present itself to the other components as pure 50ohm resistive impedance above a certain frequency.

 

[ronsimpson]

Likely your PCB is not big enough to have a problem. Do you have a trace 1/10 wave length long?

All traces have a impedance. You probably have 200 ohm traces every where and don't know it.

If you tell the board house that you do not want " impedance control " they can make the board any way they want. When you specify impedance control then they must keep the capacitance between layers the same every time they make the board. The placement of the layers is controlled, the thickness of each layer is controlled. The board material controlled. They tell you "this wide = 50 ohms".

 

[RadioRon]

It depends a lot on the frequencies involved and the length of the traces. It also depends on how precise your impedance matching has to be for your application, so we would have to know more about the details. I have had to make adjustments to the value or size of resistors and capacitors at 1.8 GHz and up, but below 500 MHz the effects are very small and can be ignored with virtually any size of surface mount parts. For example, at 5.5GHz when we use discrete parts in an RF transmission line, we are careful to choose a size of component similar to the width of the trace. Often 0201 surface mount parts are used on boards with more than 6 layers where impedance control is important as the traces can be quite narrow.


Consider the pad size used for your existing components. If they are really wide compared to the 50 ohm trace, then they may have to be changed if the length of the pad is more than roughly one twentieth of a wavelength at, oh, lets' say the fifth harmonic if digital. For an electrically short pad length, the added reactance is like a point of shunt capacitance, and the amount is very small (like perhaps 1 pF) which can often be ignored at lower frequencies. But if your pad is long relative to the wavelength of the signals on it, then you have to consider it another piece of transmission line, which gets complicated. For this reason, you may have to choose surface mount components that are a similar width to the traces, but this problem can be ignored below, oh, I would say below 1 GHz.


On the other hand, if my fundamental frequencies are below 100 MHz, I would probably not care at all what affect the trace impedance control will have on my component values. I'm not sure if others would agree with me on that, but again, it depends on how precise your application is.

 

[crutschow]

to every trace, for say 50 OHM, of the PCB will it affect the resistors and capacitors already in place

In order for the trace to act as a 50 ohm transmission line without reflections, all the component impedances connected to the trace at the frequencies of interest must be much larger than that.
There should then be a 50 ohm resistive termination at the end of the trace.