Impedance control on PCB

[neutrino]

pcb impedance

Hi,
i have some questions:
1) what is the limit over is necessary consider a trace of PCB as trasmission line??
2) Usually length > lambda/10 is a usefull formula. Is correct?? For example, if i have to project PCB with RAM,FPGA...with 50-100MHz digital signal, is necessary control impedance??
3) What is a maximum length for route that nets in multilayer FR4 dielectric? About 2 inches length is critical for 70 MHz digital trasmission data?

Regards

 

[House_Cat]

impedance control

It isn't the frequency of the digital signal that matters on a PCB - it's the risetime (or fall time) of the edge because that's where the data is contained. The critical length is approximately where the roundtrip propagation delay on the trace equals the risetime. For FR4 with a typical Er that works out to about 3 inches for a one nanosecond risetime. Beyond that critical length, it is essential to use transmission line design considerations, including impedance matching and termination.

The maximum trace length can be approximated as Lmax <= Risetime/(safety factor - propagation time). The propagation time is dependent on the board materials, and the safety factor is just an arbitrary design margin that you, the designer chooses. It typically varies between 2 and 4 to account for external "noise" from power supplies, external EMI, etc. You can also use Lmax <= (c x Risetime)/(3.5sqrt(Er)) for a very rough maximum trace length estimate. As the ristime increases, that estimation gets less accurate because the shape of the trace begins to enter into consideration for the field behaviour around the trace.

 

[neutrino]

pcb impedance control

Thanks for this perfect answer House_cat

This is about trace length, but i think even for impedance matching. With my collegues, i discuss many times if use or not a impedance control, even when trace are short. Recently, i posted in this forum a trouble with radiated emission about multilayer PCB. Trace length are electrically short (rise time 2ns, trace length about 1.5 inches on FR4, 6 layers). PCB AC cable, measured with capacitive clamp, radiate very much (60dBpW @ 60MHz). I suppose is necessary impedance matching even if trace are electrically short...

Is correct?

 

[House_Cat]

pcb impedance matching

Yes, that's correct. If you want maximum energy transfer from the source to the sink, you want the impedance matched along the entire signal path. If you don't do that, you can expect reflections (signal distortion) and radiated energy. In the case you mention, you probably had an unterminated trace, or some other mismatch between source and sink impedance.

 

[FvM]

impedance vontrol

Although impedance matching is related to EMC in several regards, it's not generally sufficient to achieve low emission designs. There are many other aspects involved, particularly power supply decoupling and filtering, also ground and power plane current distribution.

A radiating supply cable should be mainly considered as case of conducted emissions, I think.

 

[pcbdesigner34]

impedance pcb

The return path of the high speed signal is important in case the trace length is very short. If the return path is not an undereground trace, for example a ground slot, then it can lead to several secondary issue incluing EMI.

If however, the return path is continuous, changes in impedance should have small effect in quality of signal for length lambda/10. It is however, better to keep the impedance defined - to simplify the design rules.

For PCB designers I recommend the book "Signal Integrity for PCB Designers" available at amazon for 35 bucks or so.