4
\$\begingroup\$

For architectural reasons, we have a need to take a twisted pair (of an RS485 bus) into a PCB and then out. The PCB traces would add about 2 cm (just less than an inch) of length to the bus. The stubs connected to this differential trace pair in the PCB are very short (<1 cm).

Question: How to match the PCB differential trace pair impedance to that of the twisted pair cable (~120 Ohms)?

Given the low bit frequency (about 250kbits/s), the first answer that comes to mind is that the trace pair impedance does not really matter, since the shortest wavelength within the relevant bandwidth is so much larger than the trace pair on the PCB (say, a couple of meters vs. a couple of centimeters). This also appears to be true for CAN buses entering PCBs, given some of the discussions that I have seen in this site.

Having acknowledged that, if we still wanted to get as close to 120 Ohms differential impedance with the trace pair on the PCB, how can we compute the trace width and separation? Edge coupled micro strip calculations that one can find on web sites such as eeweb.com incorporate a reference ground plane on which the common-mode currents can return. In our case, it is just a twisted pair (no ground wire or shield) entering the PCB (i.e., no common-mode current return path on the wire), so should we even use a ground plane under the trace pair?

\$\endgroup\$
2
\$\begingroup\$

Yes, you do want to keep the trace impedance on the board as close to 120Ω as you can, mainly because this affects how the signal propagates on the cables attached to it. Presumably these devices are being daisy-chained together, and the reflections caused by impedance discontinuities will accumulate to reduce your overall signal integrity.

There are online calculators for controlled impedance traces that include your configuration with no ground plane, for example the one from Saturn PCB is particularly flexible.

You have some other design issues to consider, however. RS-485 receivers typically have a limited common-mode voltage range that they can handle, so you typically DO need a ground reference in your cable.

\$\endgroup\$
  • \$\begingroup\$ Very useful link, and helpful tips... thank you. Tried to match 120 Ohms on PCB using two parallel traces and no planes underneath. \$\endgroup\$ – benHur Sep 27 at 17:25
0
\$\begingroup\$

With such a small distance and baud rate, the matching will probably not matter because the speed is low, reflections and parasitic effects will be minimal. Parasitic effects start to take hold when you get into the 10's of MHz.

Because RS485 is differential, it does not need a ground plane, you could provide shielding if you like to minimize noise. You do need to worry about cross coupling from other signals, so keep that in mind on the PCB routing.

\$\endgroup\$
0
\$\begingroup\$

Impedance is always defined by geometry of conductors and dielectric with respect to (wrt) each other (DM) and wrt power ground and/or earth ground. (CM).

Saturn PCB design.exe. May tell you for a typ. Fibre/epoxy dielectric that 50 Ohms is somewhere between 0.5 to 1:1 diameter/gap and 120 Ohms is higher ratio.

A track pair or short wire pair may be 1nH/mm and 1pF/mm where the impedance is \$Z_o=\sqrt{L/C}\$. These geometric ratios define L,C which in turn defines the Zo. A long cable is closer to 0.5nH/mm and the capacitance varies significantly between a line and a plane — such as a a copper ground or a coaxial shield or a twisted pair with no shield.

Ideally the CM impedance if floating ought to be very high so stray capacitively coupled voltage creates very little current and thus any imbalanced impedance results in very low DM noise voltage. But that demands high inductive reactance and small shunt capacitance of the cable — and is risetime or frequency dependent. (Aka Balun). So you will find large Ferrite torroids on all VGA cables, and most high DC power charger cables and many microphone cables.

But often better immunity from stray inductive noise demands that the CM impedance be very low — so that the induced CM voltage is low and thus impedance imbalance further reduces the error induced as a DM noise voltage. This low CM impedance effectively better shunts stray motor current CM noise B fields for immunity.

Conclusion

For >20MBd 1cm stubs result in a negligible reduction of RS485 risetime or increase in ringing, so it may not ever cause bit errors to ignore impedance layouts at <250kBd 10ns=Tr. But for integrity it is always best to use the common ground path close to the data tracks 1:1 and choose that track gaps to match the track width. Yet Saturn will give you the optimal results.

\$\endgroup\$
0
\$\begingroup\$

Managing with Profibus over decades as field engineer, I had never found some exotic solution. It's always used with DB9 connectors with termination switches or pass through for daisy chaining. By the way, Profibus max. speed is 12 MBaud, RS485 physical layer.

The only weird part are PCB inductors, probably needed to limit \$\dfrac{di}{dt}\$ in case of ESD discharge through TVS. Have look at link Since your speed is relatively low, I don't see any need to calculate PCB impedance.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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