cancel
Showing results for
Did you mean:

# What do the following symbols mean in the NUCLEO-F429ZI circuit diagram?

Associate

This is a part of the circuit diagram of NUCLEO-F429ZI.

What do the symbols in the picture below mean? is the inductance ohm value?

thank you.

1 ACCEPTED SOLUTION

Accepted Solutions
Evangelist III

As @Tesla DeLorean said, "Diff Pair 90-ohm" means a differential pair with a characteristic impedance of 90 ohms.

With high-speed signals like USB, PCB traces need to be treated as transmission lines.

https://circuitdigest.com/article/understanding-impedance-matching-in-pcb-design-with-example-and-calculation

@happyojj wrote:

is the inductance ohm value?

No - inductance would be in henrieshttps://en.wikipedia.org/wiki/Henry_(unit)

8 REPLIES 8
Guru

Traces routed as a differential pair with matching length and impedence?

So together, side by side, same length, direct.

Tips, Buy me a coffee, or three.. PayPal Venmo
Up vote any posts that you find helpful, it shows what's working..
Evangelist III

As @Tesla DeLorean said, "Diff Pair 90-ohm" means a differential pair with a characteristic impedance of 90 ohms.

With high-speed signals like USB, PCB traces need to be treated as transmission lines.

https://circuitdigest.com/article/understanding-impedance-matching-in-pcb-design-with-example-and-calculation

@happyojj wrote:

is the inductance ohm value?

No - inductance would be in henrieshttps://en.wikipedia.org/wiki/Henry_(unit)

Senior III

> So together, side by side

Oh no you didn't.

Differential pairs are defined by how the signal is represented electrically (as the difference of two signals), not by how you lay out the traces.

You can keep the differential pair uncoupled (far apart) and route each as a single-ended line. The "odd impedance" is then zero which means the differential impedance is simply twice the characteristic impedance of each. You can maintain a constant differential impedance by controlling the impedance of each of each separatly, as you would with a single-ended signal.

In that case, you can absolutely route each on opposite sides of the board. As long as the differential signal wherete they converge at the receiver is not corrupted, it will work just fine. They are usually routed together for convenience and to simplify delay-matching when it is required. But this is not strictly necessary. Even if they are very far apart, they can still be a differential pair.

Another common argument for routing them together is supposedly common-mode rejection. CMR in differential pairs on a PCB does exist, but it's not as effective as it is in twister-pair cables (due to the fundamental difference in geometry between the two). This benefit on its own does not necessarily justify routing the diffpair physically close to one another. (Update: because this also forces you to reduce their width to achieve desired impedance. For very high digital signals, this increases ohmic loses and closes the eye diagram, so the design might simply not work).

(Update: but there may also be EMI considerations)

There are several talks by the regular "SI expert" grifter crowd, on all this.

Pardon my fervor. SI myths are a pet peeve of mine, since I'm constantly being tormented by the gobs of bad and conflicting information out there.

- If someone's post helped resolve your issue, please thank them by clicking "Accept as Solution".
- Please post an update with details once you've solved your issue. Your experience may help others.
Principal

To the original question: these are markers / directives from schematics to PCB layout in Altium Designer.

As long as the differential signal when the converge at the receiver is clean,
> it will work just fine.

> They are usually routed together for convenience and to
> simplify delay-matching when it is required.

My 2 cents:

As the differential receiver should have some common mode rejection (CMR) (even at high frequencies) there's also the advantage of routing the signals together so they might pick up the same noise, which might then be attenuated by the receiver's CMR.

Senior III

@LCE, I was just updating my answer in anticipation of this common argument. Only to find out you almost immediately made it  😀.  Please see the additions and let me know if you disagree.

- If someone's post helped resolve your issue, please thank them by clicking "Accept as Solution".
- Please post an update with details once you've solved your issue. Your experience may help others.
Principal

As I'm doing a lot of audio stuff, I'd say CMR is more relevant for LF audio signals in mixed signal boards.

But okay, usually good anti-aliasing filters are the safer way in that case.

To be honest, I have limited HF-CMR hands-on experience, mostly due to lack of proper equipment.
But just in case, I like to keep differential pairs together.

Senior III

As I'm doing a lot of audio stuff, I'd say CMR is more relevant for LF audio signals in mixed signal boards.

And I don't have much experience in that area.

I have no problem accepting that for LF signals, and in particular audio, every bit of extra CMR you can get, for example by routing traces close together - is better than nothing. And of course, since you don't care about losses (as you would in very high speed digital), there is no downside to doing so.

But just in case, I like to keep differential pairs together.

Hey... we all like something or another. 👍

- If someone's post helped resolve your issue, please thank them by clicking "Accept as Solution".
- Please post an update with details once you've solved your issue. Your experience may help others.
Senior III

"Diff Pair 90-ohm" means a differential pair with a characteristic impedance of 90 ohms.

actually, that's not quite correct. 90-ohm is the nominal Differential Impedance for the diff pair that carries data in USB 2.0 (The DP/DM signals). You sometimes also encounter the equivalent term "Differential Characteristic Impedance". But the term "characteristic impedance" is usually applied only to a single-ended line (a single transmission line).

Here they placed the diff impedance annotation twice, once for each half of the pair. That's not a good way to do it.

- If someone's post helped resolve your issue, please thank them by clicking "Accept as Solution".
- Please post an update with details once you've solved your issue. Your experience may help others.