Very long trace left unconnected at one end... is it bad?

[Saimoun]

Hello!

I'm kidding, I know it's bad 
But I'd like your help to find out how bad! The circuit is very simple:

MCU pin -> 1.8k res -> NPN -> Collector pulled up to 5V with a 820R res and emitter to ground.
(see attached picture as well)

Then MCU is used to switch the voltage between 0 and 5V to send a digital signal.

The problem is the signal is also routed to a very long trace (about 25cm), reading about it online it seems that with 25cm, only frequencies above 300MHz
will start to be an issue. Would you confirm or is there more to it even at low frequencies?

I'm trying to calculate the frequencies of the 5V signal. The MCU datasheet gives the max rise/fall time (see attached), say we estimate it at 20ns. Looking up online again, I found that the highest frequency is about 350/20 = 17.5MHz. This is probably slowed down by the 1.8k resistor at the base of the NPN anyways, so... it looks everything should be fine?

Thank you!

[themadhippy]

whats the point of the resistor if one ends unconnected?

[T3sl4co1l]

Where is the series 820R, is it by the transistor?  What transistor type, general purpose, so it probably turns on in a couple 10 ns?

What is the board design / layout?  Ground plane?  Is anything near the trace?

What criteria judge "badness"?  If emissions, to what standard?  Is the board naked (or in a plastic enclosure), shielded (or metal or conductive-coated plastic) enclosure, etc.?

Tim

[xvr]

Your one-side-unconnected trace is effectively an antenna. Will it be radiate or not mostly depends on geometry of it and environment.

[radiolistener]

reading about it online it seems that with 25cm, only frequencies above 300MHz
will start to be an issue. Would you confirm or is there more to it even at low frequencies?

No that is not true. I had issues with parallel bus running at 100 MHz clock with just 5-10 cm length, all wires was exactly the same length but when I tried to move wire position (for a clock wire and for data lines wires), it leads to transfer errors very easily.

Another example is interface between FPGA and GMII PHY chip. It running at 125 MHz but can leads to transfer errors even with millimeters wire length error with total wire length about 1-2 cm.

Even 50-100 MHz requires to be very careful with transmission line length and impedance.

In addition, GPIO has some capacitance load limit, and if you use long wires you can exceed it. So it may require to install buffer to amplify the signal.

[Saimoun]

Where is the series 820R, is it by the transistor?  What transistor type, general purpose, so it probably turns on in a couple 10 ns?

What is the board design / layout?  Ground plane?  Is anything near the trace?

What criteria judge "badness"?  If emissions, to what standard?  Is the board naked (or in a plastic enclosure), shielded (or metal or conductive-coated plastic) enclosure, etc.?

All very good questions, Tim!

* 820R is by the transistor
* Transistor is general purpose indeed, typical jelly bean NPN in a SOT23 package.
* Board layout is 2-layer, ground pour on both layers connected by many vias
* PCB is in a metal enclosure (not fully closed though, many apertures for connectors, displays, etc.)
* Is there anything near the trace? Not much, though it's not too far from the edge of the board (right by the metal enclosure), sometimes as close as 1-2 mm to the edge. Though there is always ground between the PCB edge and that long trace (not sure if that makes much of a difference?).
* The "badness" thing - say for example "will it be a major issue for EMI testing for FCC/CE certifications"? (I know this is still general - but my question is still quite general, to get an idea of how much of a problem this could be)

reading about it online it seems that with 25cm, only frequencies above 300MHz
will start to be an issue. Would you confirm or is there more to it even at low frequencies?

No that is not true. I had issues with parallel bus running at 100 MHz clock with just 5-10 cm length, all wires was exactly the same length but when I tried to move wire position (for a clock wire and for data lines wires), it leads to transfer errors very easily.

Another example is interface between FPGA and GMII PHY chip. It running at 125 MHz but can leads to transfer errors even with millimeters wire length error with total wire length about 1-2 cm.

Even 50-100 MHz requires to be very careful with transmission line length and impedance.

In addition, GPIO has some capacitance load limit, and if you use long wires you can exceed it. So it may require to install buffer to amplify the signal.

Ok interesting, thanks for the reply But you're speaking about signal speed, though? my signal speed is very very low, it's below 10kHz. So my only concern is more regarding the signal edges, hence looking at the rise/fall time.

[thermistor-guy]

Your one-side-unconnected trace is effectively an antenna. Will it be radiate or not mostly depends on geometry of it and environment.

In hot-insertion telecom equipment (my background), depending on where the trace is located, that trace could pick up +/-1kV impulses
during compliance testing, via capacitive coupling.

If the trace goes near connectors and the edge of the board, where installation personnel typically pick it up, the trace could serve
as a path for ESD, as installers pick up the board; insert it live into operating equipment; touch the trace as they do so; and discharge
into the trace. Over a 30-year nominal operating life, ESD events happen, as installers do upgrades, board swaps, and troubleshooting.

So, depending on circumstances, you could consider some ESD protection (e.g. diodes to GND and VCC) on the trace. May not be necessary.

[T3sl4co1l]

I'd still have to see where connectors and grounding and etc. is going on inside there, but 99.5% sure it's absolutely, positively no issue whatsoever.

Assuming that means FCC Part 15 compliance.  Or maybe even Part 18, even easier?

Ok interesting, thanks for the reply But you're speaking about signal speed, though? my signal speed is very very low, it's below 10kHz. So my only concern is more regarding the signal edges, hence looking at the rise/fall time.

Nonono-- your clock or bit rate might be 10kHz, the transition rate is on the order of 5ns from the MCU (as low as fractional ns for higher speed MCUs, up to maybe 20-30ns for old or slower ones, or slew-rate-limited settings), and probably a fall time of 10ns from the BJT.  That means harmonics all the way up to corresponding frequency scales, i.e. 50MHz.  Maybe not much, at the low rep rate, but you're also talking an electrically-short antenna so it has its own gain proportional to frequency characteristic that balances it out, and you get blips from it.

The kicker is:
1. Trace in PCB is poorly coupled to free space -- this is already enough to pass, e.g. on-board UART signals at 3.3/5V rarely if ever cause trouble;
2. Excessive source termination resistor means the leading edge is attenuated significantly to begin with (i.e. about 20dB);
3. Enclosure, assuming it's at least moderately well grounded to the board, and connectors aren't spreading around common-mode noise somehow coupled to the trace in question (but, coupling has been said to be very low, so that seems impossible), can easily knock that down another, say, anything from 20dB to over 100.

"Well grounded", at these edge rates, might be as simple as a single mounting screw; a great connection isn't really necessary.  Well, assuming the enclosure and board aren't massive or anything, but like palm sized.

More likely all the other connectors emit exponentially more noise, but you asked specifically with respect to one trace, and, it's one of the relatively rare cases, an EMC problem sufficiently well specified and constrained, that a more or less direct answer can be given.

Tim

[radiolistener]

But you're speaking about signal speed, though? my signal speed is very very low, it's below 10kHz. So my only concern is more regarding the signal edges, hence looking at the rise/fall time.

the shape of signal edges is what it is. More sharp and clean edge requires more high frequency bandwidth.
For example, if you're needs 10 kHz signal with 1 ns rise time, your transmission line needs more than 350 MHz bandwidth and it will be very sensitive to a proper termination.

So it all depends on your specification for "should be fine"... 

[MarkT]

The problem is the signal is also routed to a very long trace (about 25cm), reading about it online it seems that with 25cm, only frequencies above 300MHz
will start to be an issue. Would you confirm or is there more to it even at low frequencies?

Out by orders of magnitude, a 25cm stub although only resonant at 300MHz, is an bona-fide RF component well below that - at 10MHz it acts as maybe 30pF if over groundplane, that's an impedance of only a few hundred ohms, nothing like an open circuit.   And in the time-domain its a transmission line of about 4ns round-trip time on FR4 (if over an unbroken ground-plane).

So your 20ns switching signal might be affected by it - whether that matters depends on a lot of things, its quite likely not to matter unless the destination of that signal is sensitive to runt-pulses or double clocking, and if the signal is faster than your estimate of 20ns.  I suspect it won't be an issue in most circumstances, but if your board had to pass EMI compliance testing it might be an issue in that it could both emit EMI and receive EMI (most likely if its near a board edge).

[Saimoun]

Thank you very much all for your replies! Awesomely useful as always

Yes I'm aware about rise time being the part that matters, but @radiolistener you were speaking about a 100MHz signal, which will be hard to make with my 20ns rise/fall time

@Tim: very nice to hear, thanks for the thorough explanation!

"Well grounded", at these edge rates, might be as simple as a single mounting screw; a great connection isn't really necessary.  Well, assuming the enclosure and board aren't massive or anything, but like palm sized.

Yes the case has a single mounting screw, and yes the whole thing is about palm sized

Out by orders of magnitude, a 25cm stub although only resonant at 300MHz, is an bona-fide RF component well below that - at 10MHz it acts as maybe 30pF if over groundplane, that's an impedance of only a few hundred ohms, nothing like an open circuit.

I see, that makes sense. So, as Tim mentioned I have parts of my signal around 25-50MHz (because of the edge rates of 5-10ns). What would be the issues rising from this concretely? Ringing on the signal?

Thanks

[radiolistener]

What would be the issues rising from this concretely? Ringing on the signal?

it depends on how output is implemented. In some cases it can lead to heating or even burn out output driver or can affect power supply voltage due to higher power consumption. But usually it is critical for high power signals. For a usual logic it can leads to higher EMI or some undefined behavior for the chip if such load is out of specification.

[T3sl4co1l]

it depends on how output is implemented. In some cases it can lead to heating or even burn out output driver or can affect power supply voltage due to higher power consumption. But usually it is critical for high power signals. For a usual logic it can leads to higher EMI or some undefined behavior for the chip if such load is out of specification.

Since the circuit is given, and layout approximately given, we can be much more concrete than this.  There is no ringing on the signal, the edge rate is less than the electrical length of the line and the source impedance is much higher than the line impedance.  At best a little bit of steppiness might be visible on the falling edge (as the transmission line repeatedly charges, in steps, through the impedance mismatch), which can be read as the superposition of ringing on top of an RC rising edge, but again given the low edge rate, the mode is hardly excited.

If it were a 74LVC-class pin driver connected directly to a stub line of the given length, I might wonder if it would rise to the level of commercial (class B, maybe class A as well) radiation limits; or particularly if driven at some MHz.  I don't have a good feel for where what Fsw and trace length corresponds to what dB broadly speaking, but within orders of magnitude, that should be about right.

Tim

[Saimoun]

Thanks Tim again - very glad to hear! I'll confirm this with the oscilloscope when I get the PCBs