Is it important to design to 50 ohm even the digital lines (for example SPI lines)?
on my RF board there are both analogue lines and digital lines.
On analogue lines there is a RF carrier. That lines have been designed to have 50 ohm characteristic impedance.
Regarding digital lines, what should I do? In my case, there is a SPI to program a PLL. Do these lines have to be designed to have 50 ohm characteristc impedance?
Thanks and best regard.
Antonio
Only your RF lines need to be 50 ohms (if that is their characteristic impedance). Make the digital lines large enough to do their job, but no larger.
Hi,
I can′t remeber that I′ve ever seen a SPI line designed as 50 Ohms line. Did you?
Generally this depends on frequency, trace length and so on.
--> give SCK frequency and trace length.
But let′s say you have a 20MHz SPI clock, then the 20MHz wavelength is about 20m... for sure there are overtones, but i don′t think your SPI trace come somehow near to some meters.
And below that length you have reduced reflections, reduced influence on the signal and thus less benefit in creating a 50 Ohms line.
Additionally when you use a 50 Ohms line, then your driver (SPI signal) needs to be able to drive this 50 Ohms signals and you need a 50 Ohms termination... and for sure a suitable HF feedback path.
On the other hand I already transferred SPI over 120 Ohms lines. Over several meters, differential signalling with RS485/RS422 drivers. Mainly to maintain signal integrity over some meters in noisy environment. Also to suppress GND bounce problems when communication between two different PCB.
Klaus
I agree with Klaus, for the most part you can forget the impedance of digital lines, especially for fairly low speed comms like SPI. Do be careful though when it comes to high speed USB, Ethernet and HDMI where the impedance starts to become relevant although trace length rather than impedance is more important.
Brian.
A frequently used termination scheme for fast digital signals is source side series termination with unterminated load side. Impedance of single ended lines is rather 70 than 50 ohms.
Source side series termination is partly provide by digital IC output impedance and may be supplemented by additional series resistors in the 20 to 50 ohms range. It becomes relevant above 50 or 100 MHz signal frequency.
depending on the clock rate, it MAY be an issue. But most SPI interfaces are pretty slow.
I HAVE seen some issues related to ringing on such lines, but that is more related to the poor job the chip vendor did than the line impedance.
Yes, this might be good to add in pads for, just in case
The sorts of problems i have seen are more ringing related.
If THIS is you clock waveform at the chip, and the ringing is big enough in amplitude, the chip might think the rising edge of the clock pulse is two separate clock events, and try to load the data twice...which of course screws everything up royally
Dear Antonio,
even if you design all of your digital PCB traces at 50 Ohm, they will be terminated to a load which is the GATE of the MOSFET of the integrated circuit.
That GATE is a capacitor of a few pico Farads.
That means that you have a 50 Ohm line terminated to a capacitor and not to a 50 Ohm resistor.
That means that you will always have some sort of signal reflection because of the impedance mismatch: 50 Ohm terminated to a capacitor.
Just design your PCB digital (SPI, UART, ADDRESS BUS, DATA BUS) traces as short as possible in order not irradiate or pick-up noise.
Enrico Migliore