Grounding scheme impact on LVDS impedance matching?

[bitbanger]

Hi Folks -

A fellow EE insists that a ground-based differential LVDS link (i.e. not opto/mag/cap coupled) which lacks a dedicated DGND reference between the two transcievers will cause impedance mismatching. That the ground is necessary for the "impedance reference", otherwise there will be "mismatch" causing reflections.

I do believe the units need to share a common ground, however only to guarantee that signal levels are within the common-mode limits of the receiving ends. I also believe this guy has some basis for his argument, I'm just trying to understand it.

What are your thoughts on this?  I purposefully excluded a ground connection between the two in this LVDS link to avoid common mode (and potential loop) currents in the same cable. The units' power supplies do share a common ground, outside of this link. Connection (10Mbps+) is via 15' or so of 100 ohm twisted shielded pair. Individual and overall braided shield. Transcievers in this case are pretty generic current-mode drivers, +/- 3.5mA, and tolerate I believe +/- 1Vdc of common mode difference between transcievers.

I really only have a basic understanding of transmission line theory so hope to learn from this. I tied overall shield together on both ends to chassis (not the same as DGND), but only grounded (again to chassis - DGND not available on both ends in this connection) the TX ends of the inner pairs. He wanted a discrete connection between DGNDS, even if it meant a single wire outside this quad-TSP cable.

Thanks for your thoughts.

[ConKbot]

I think the rub here is that your transmission line isn't a pure 2-wire pair.  On the PCB, I'll assume it's an edge-coupled microstrip. If your microstrips 50 strips are far apart (no edge coupling) you'll have a 100 ohm differential impedance, and a 25 ohm common mode impedance. Not too big of a stretch,  just the two impedances in series, and parallel.  The tighter you couple them, (closer together) the common mode impedance goes up as they have a mutual effect on each other, and differential impedance drops. you make your lines narrower, ground plane further away, and repeat until eventually you end up with a strongly coupled pair with no real influence from the ground.   

However, on a circuit board level, for typical multilayer construction, you can't get them very far from a reference plane, and you can't shrink your traces but so far, while maintaining a reasonable spacing. so you end up with two somewhat coupled lines and a ground plane making up the transmission line, not just the pair.

Since your ground isn't a nice short one, draw the loop from your connector, to the panel, to the standoff, to your DGND plane. Your nice big loop area makes for easy pickup of common mode interference.

When ethernet runs though the magnetics, on the phy side the center tap and it's termination allows the loop for the common mode currents to be closed in a small area, while the transformer and CMC isolates it from external common mode noise on the unshielded pairs.

[T3sl4co1l]

A few things.

1. Differential transmitters and receivers don't magically absolve you of the fact that you still have two, mostly independent transmission lines going over a (presumably dirty) board.

You still have the transmission line behavior of each trace.  Differential only works when the behaviors are matched, i.e., equal lengths from transmitter to noise sources (e.g., slot in ground plane) to receiver.

2. LVDS transmitters have a modest common mode resistance.  They aren't specified in this way (instead, they are described as pure current sources, a lie*), but it seems to be the case.  This will dampen common mode resonances, although not too well because of the mismatch.

*A sufficiently high resistance, in comparison to whatever impedance matters (in this case, the common mode impedance), looks constant-currenty.  It may be they are using that approximation, rather than outright lying.

In general, expect an LVDS pair to experience resonant common mode voltage at both ends.  The multiplication factor is the Q of that resonance, which can be quite unfavorable (probably less than 10x, but more than 1x).  This should be damped by terminating the common mode at one or both ends, but alas that is never recommended (possibly because the termination voltage is almost never going to match the common mode voltage the transmitter produces, and therefore it radiates every time the transmitter goes from Hi-Z to active; that could be addressed by terminating with an R+C, which charges to the transmitter's common mode level without drawing DC).

3. Wait, this isn't on a PCB, or over short distances?  And it's only ~10Mb?

Use RS-485 transceivers!  End of thread!

If you absolutely must, consider:
- LVDS bus driver (7mA)
- HDMI PHY or something along those lines (CML, basically LVDS; made for driving cables)
- Ethernet (an awfully heavy-weight step up, but will blast through any distance of UTP you hang off of it!)

You are quite correct that the signal needs to be grounded and shielded.  STP isn't bad for this, and 15' is probably not at all unreasonable.  Ground the shield to circuit ground at both ends.  I don't care what you call it, it's got to be RF-bypassed to the circuit ground plane, whatever that is.

If chassis GND is very close to DGND, then grounding the shield to chassis can be acceptable.  If not, you are making things very, very much worse, injecting exactly that common mode noise into the receiver!

Tim

[bitbanger]

Con -

I suspect this is his main rub as well, the fact that the differential pair of traces have a common mode element to the associated PCB's ground plane. I will give him that this will influence the controlled/matched impedance of the traces. What I don't understand is why this matters beyond that? Aren't the three "nodes" simply dealt with individually for sake of impedance matching? These are full duplex links but for example 1)TX PCB with controlled impedance traces 2)TSP cable, and 3) RX PCB with controlled impedance traces and term resistor. Driving factor for the characteristic impedance of the cable is physical properties, distance, permeability, not common mode capacitance, so again my potential ignorance fails to see how a discontinuity in DGND matters so long as comm mode input ranges are adhered to?

'Tesla:
This is an existing system, using an industry standard avionics link, "it is what it is".  Link starts at 10Mbps but can negotiate to 200Mbps (theoretically 400Mbps but not in this case). "TX" or host PCB was designed and routed in house for high reliability application so I'm confident it was done properly. Same goes for vendor "RX" unit.

Interesting discussion - wish I could comment more but for the moment 'thanks! One point to note is that this link spec has long called for overall shield connected on both ends, and TX ends' inner shields terminated to pin3 (PCB DGND) on that end (no through-cable connection between DGNDS). Draft spec is proposing ALL shields, inner and outer, connected to both shells (no connections to pin three on either end).