# When does controlled impedance on a PCB matter?

Suppose I have a PCB that contains a microprocessor, or an FPGA (a "controller"). This "controller" drives a single-ended signal to an LVDS driver IC and a single-ended signal to a connector that goes out of the board. The output of the LVDS driver IC is then driven to the same connector that goes out of the board, as a differential pair.

If the board is specified as a board with controlled impedance, that is, 50ohms for single ended, and 100ohms for differential signals, does that specification only concern the signals going out of the board (single ended signal coming directly out of my controller and the output of the LVDS IC)? In other words, what significance does the characteristic impedance have for the signal that is not leaving my board (single ended signal going from the "controller" to the LVDS driver IC)?

-

It depends on how far the LVDS driver is from your FPGA and the rise time of the signal (note not the toggle rate)

If the trace is greater than ~1/10 of the electrical length (rise time / propagation delay) then you will probably need to look controlling impedance and termination with a trace of certain width above a ground plane (microstrip) or between planes (stripline)
If less than this (i.e. your LVDS driver is close enough to the FPGA) then you should be fine.

A typical propagation delay for microstrip (a trace above a ground plane) might be 150ps/in. So if your rise time is say, 1500ps then your electrical length is 1500/150 = 10in. So a trace longer than 1 inch will need consideration (some would say 1/6 of the electrical length or 1.6in, see the NI note)

Often just terminating at the source will do, as the reflections will only "bounce" once, and power consumption will be lower than with other techniques. You can do this with a series resistor equal to the difference between the output impedance of the driver and characteristic impedance of your trace. So if your driver has an output impedance of 20 ohms, them your series resistor will be 30 ohms (assuming a 50 ohm trace - note the impedance can change a bit depending on logic state)
IBIS models and simulation help, and SPICE can model a basic transmission line. You may want to play around with a simple setup based on the notes below in SPICE to get a feel for it.

There are many other ways to tackle this, and a lot more to it than outlined above - here are a few decent app notes on termination:
Transmission Line Terminations - UltraCAD
High Speed Layout Guidelines - TI
Proper Termination for High Speed Digital I/O - NI
FR4 propagation delay

-

PCB with controlled impedance allows you to make traces with specific impedance you need.

If you match driver, receiver and transmission line impedance, there will be no signal reflections, so this is very important when you have >10cm traces and >50-100Mhz frequencies.

Making trace with specific impedance without controlling it on the factory is impossible as different brands of FR4 would give you different impedance.

I.e. this is important even if signal never leaves your board.

-
 I understand. But for example, for the situation I described in the original post, the LVDS driver IC only specifies the impedance of its output, ie, it says that the IC is designed to drive a differential impedance of 100ohms. However, no specification is given for its input (the side that is connected to the microcontroller, or to the FPGA). Therefore, why would it make sense to drive the LVDS ICs input side with 50ohms impedance line? – SomethingBetter Sep 18 '11 at 15:25 @SomethingBetter What I said applies everywhere. The fact that it's not specified does not mean that it does not exist or it should not be concerned. I believe that it's not specified because signal integrity on the input side was not an issue (and probably is), so one might not care about impedance for inputs. – BarsMonster Sep 18 '11 at 19:26