1
\$\begingroup\$

on my project I'm using two PCA9615DPZ chips to extend an i2c bus between two boards.

The situation is:

PCA9615DPZ -> 15cm track -> connector -> 1m cable (CAT5) -> connector -> 15cm track -> PCA9615DPZ

But I have a couple of doubts:

1 - Do I have to use differential traces with controlled impedance? I didn't find a note about this in the datasheet, but is it necessary to use 100 ohm or 120 ohm differential traces?

2 - In case controlled impedance traces are needed, using a calculator I get that for a basic 4 layer stackup, the traces are about 0.1 mm, therefore very small. Could I have problems with my situation using such small traces? (I think they carry very little current)

3 - I have exactly the same problem with an RS-422 Transceivers MAX3077EASA+T, in which I find myself in exactly the same condition, are the same 1 & 2 considerations valid for this too?

In both cases I use a fairly low baud rate, but if it helps I can also go down to quite low baud rates.

\$\endgroup\$

2 Answers 2

0
\$\begingroup\$

For all questions, in theory, as you have a 100 ohm impedance cable for differential data and 100 ohm termination, you should also use 100 ohm differential pair for PCB tracks.

Another thing is what happens if you don't, as that is difficult to guess, as the PCB trace length is only 15cm. But any discontinuities in the impedance means that part of the signal gets reflected back.

And it does not depend on how fast the data rate is, but how fast the signal edges are. Of course even with fast edges, slowing the data rate helps.

Unfortunately the MAX3077E is intended for 16 Mbps and higher data rates so it has very fast edges. The slew rate is less than 15ns, while a 15cm PCB track has 1ns propagation time. It may work without issues.

The track width should handle any normal situation.

\$\endgroup\$
2
  • \$\begingroup\$ OK, I understand you need controlled impedance traces. But could I have problems with such small traces? Just over 0.1 mm in width. \$\endgroup\$ Mar 21, 2023 at 8:05
  • \$\begingroup\$ Have you researched how much current a 0.1mm trace can handle or how much resistance it has? It depends on how thick copper you intend to order. Then you can figure out how much current you need and if the trace resistance is a problem. \$\endgroup\$
    – Justme
    Mar 21, 2023 at 9:11
1
\$\begingroup\$

Compare bitrate to track length and rise time.

While a minimum risetime is not specified, it's unlikely to be much less than, say, 1/3 the maximum; the RS-422 transmitter's 15ns max. is the most critical in this regard. 5ns at 67% speed of light is 1m, and we should be less than 1/4th this to avoid transmission line effects, or 25cm.

It is highly unlikely that 15cm of mismatched or uncoupled traces will run afoul of either of these interfaces.

The worst mismatch you can get is probably downward, using an obnoxiously wide trace giving an impedance of, say, 10s of ohms; this will basically manifest as lumped equivalent capacitance, which will still have little effect on the system; but will reduce bandwidth and signal quality if many such stubs are connected to the bus. (You can't make trace impedances very high, even if removing ground plane and using minimum trace width; typical widths on 2 and 4 layer PCBs are in the 50 to 150 ohm range.)

Not to say you shouldn't; and you certainly can. Simply to say, the advantage at these frequencies will be marginal. But it is good practice for working with faster interfaces where it is critical, and a marginal advantage is still an advantage.

Or, to put it more generally: a differential interface must always use differential traces with controlled impedance; the question is, how tight the impedance matching and coupling distance should be, over what lengths. For these standards, those lengths are approximately the length of a whole board, so it would be hard to actively abuse the signals to a significant degree. Likewise the allowable mismatch within that length could easily be, say, ±50%, which basically means, use the default track width and you're set.

The signals should still be routed as a pair, just so they are exposed to similar noise environments -- any noise picked up along the route can subtract out at the receiver. They don't have to be particularly close.


Just a general comment about the dI2C chips: notice they specify a 0...VCCB common mode range only. (Compare with RS-422/485* which specifies -8...+12V, suitable for most industrial applications.) Compared to the ~1.5V signal level, this will offer enough range to deal with commercial level noise sources (a few volts conducted/radiated), but not transient interference such as EFT and ESD. I don't see mention of transient immunity in the datasheet, other than to claim that it exists (it's mentioned, but without specifying any level and test setup, this is meaningless). I would recommend shielded cable for this link, particularly if you need to withstand harsher (industrial or worse) environments. (The shield may in turn require some means of dealing with ground loop; the shield can be RF-bypassed with capacitors at one or both ends, for example.) Perhaps they have better immunity than this, I don't know, but it is unfortunate that they didn't design for a wider input range, or specify immunity directly.

*Curiously, I don't see an input common mode range specified for the MAX307x series. It's probably fine, but I would be tempted to shop around for an equivalent part that does specify this -- just to be sure.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.