Does Differential pair required ground plane ?

[Kabaleeswaran]

Hi Team,
i am new to Design.In My design, there is low speed Differential pair and High speed Differential pair available. Even i maintained 2W spacing between Diff pair to Diff pair. Some section ground trace running in between high speed differential pair to avoid the cross talk. low speed signal there is not need of ground plane for Diff pair.

the requirement are,
1.cross talk able to meet to provide proper spacing between differential pair 2W spacing .
2.EMI able to avoid ground trace between each differential pair.

So what is the major role for ground plane in high speed differential signal ?. or does differential pair need ground plane ? because one signal is reference for another signal .can you explain short answer for this query.( i red so many document. little bit confusion. ).



can any one explain is it possible to meet the requirement with out ground plane ? With out ground plane is not able to control the cross talk , EMI issue and other.

[robertferanec]

Some section ground trace running in between high speed differential pair to avoid the cross talk.

- did you include these GND tracks between pairs when you calculated impedance? also, I believe, if you use this kind of technique, you may need to place VIAs in more places, not just at the beginning and end.

1.cross talk able to meet to provide proper spacing between differential pair 2W spacing .

- bring the sold ground plane under the diff pairs close to them, that will help to eliminate crosstalk. Also, please keep in mind, when you see a recommendation such 2W these are usually done based on specific impedance. this video may help: https://youtu.be/Bu4MirknEvo

So what is the major role for ground plane in high speed differential signal ?. or does differential pair need ground plane ? because one signal is reference for another signal .can you explain short answer for this query.( i red so many document. little bit confusion. ).

- I have the same question what Paul van Avesaath asked: How did you calculate impedance if you don't have a reference plane?

Also, don't forget. In some cases / interfaces, differential pairs are just two single ended tracks with opposite signals running through them => e.g. even when routing these differential pairs, each track in pair needs to meet specific single ended requirements, for example they have to be routed by 50OHM impedance.

[Paul van Avesaath]

not 100% sure.. but technically you do not need the GND plane for a diffpair the GND plane is there for impedance. so how did you calculate the impedance without a reference plane?

for crosstalk i would go as wide as you can between the .. so 3 or 4 times the width if you can manage..
i do see some wierd openings in the GND traces you draw between the diffpairs (but that could also be a glitch in the screenshot)

in general you need a GND plane for the return current so i would highly advice adding it.. it will be better for the whole design.

[robertferanec]

Some section ground trace running in between high speed differential pair to avoid the cross talk.

- did you include these GND tracks between pairs when you calculated impedance? also, I believe, if you use this kind of technique, you may need to place VIAs in more places, not just at the beginning and end.

1.cross talk able to meet to provide proper spacing between differential pair 2W spacing .

- bring the sold ground plane under the diff pairs close to them, that will help to eliminate crosstalk. Also, please keep in mind, when you see a recommendation such 2W these are usually done based on specific impedance. this video may help: https://youtu.be/Bu4MirknEvo

So what is the major role for ground plane in high speed differential signal ?. or does differential pair need ground plane ? because one signal is reference for another signal .can you explain short answer for this query.( i red so many document. little bit confusion. ).

- I have the same question what Paul van Avesaath asked: How did you calculate impedance if you don't have a reference plane?

Also, don't forget. In some cases / interfaces, differential pairs are just two single ended tracks with opposite signals running through them => e.g. even when routing these differential pairs, each track in pair needs to meet specific single ended requirements, for example they have to be routed by 50OHM impedance.

[Kabaleeswaran]

Hi
paul and robert Thanks for your update. I agree with your point. I need one more clarification,
L1-Top
L2 -Ground plane ( number of signals are more so taken more signals in ground plane)
L3 -pwr
l4-Bottom

there is ground plane as your suggestion diff pair required ground plane to meet impedance so instead of ground plane shall i route ground trace in adjacent to diff pair which help to meet impedance ? due to space , density and cost and other .please guide me.

[robertferanec]

Did you try to check the price difference between 2 layer and 4 layer PCBs? These days 4 layer PCB is not expensive, but are much better. Solid GND has many advantages and it will make your PCB much more reliable and stable. Also solid GND saves a lot of space (you don't have to route GND tracks).

PS: routing gnd tracks is not as good as solid gnd plane. also you would need to calculate it differently, have a look at coplanar calculation.

[Kabaleeswaran]

Hi Robert,

Thanks for your answer. can you explain one more point too.

For differential pair underneath Ground required but Differential pair one signal is reference to other signals vice versa. so how ground loop short in Differential pair ?. Please explain shortly.

[robertferanec]

often differential signals are just two single ended outputs with opposite signals. this means, that for example for a specific differential pair you still need to route Positive track let's say as a 50OHM single ended signal (that is how you get width of the track), you still need to route negative signal as 50OHM and together they need to be 100OHM differential pair (that is how you get the gap with between them).

Also, PCB calculators almost always need distance from ground plane to be able to calculate differential pair impedance. Or what calculator do you use to calculate differential pair impedance without a reference plane? Can you add a screenshot?

[Kabaleeswaran]

Hi Robert,

I have not any calculator. I need to understand how ground is important for differential . i studied some document i could not get clarity. after discuss with you. i could understood. still i have some doubt in other interface. i will post it later. any way thanks for your support.

[Jere]

I have a quite similar question, I’ve read about this topic since I need to design PCB with some Ethernet Poe with differential paires.


1) My question is, What is best ? to not have a GND plane under Differential pairs ? or to have one, but the pairs need to cross a GND gap ? (The Magnetic Ehternet transformers guidelines, requires no ground plane underneath, so I I have a GND plane every where except under this component, and my diffrential pairs traces goes on layer above this GND gap, I have some trouble right ? (my guess is to have no GND plane under all of the Diffs pairs, to avoid impedance changes, but I need your help clarify that)



2) My second question is, what is best ? to keep the length equal between the 2 traces within a diff pair, or to keep them more symmetrical, with the gap in between strictly parralel ? Since, length should match, to avoid common mode noise, but the traces shoul be parralel to avoid impedance variations. If I choose to match length I loose some symmetry and introduce variance in impedance, and problem vice versa.

3) My third question : I understand that the length should match within the 2 traces of a diff pairs, but does it need to match with the length with other diff pairs ? (For example an Ethernet connector has 4 pairs, should all 4 pairs have same length ?

I’ve found an impedance calculator that does calculate differential impedance with no ground (iCD Design Integrity field solver)

So here, apparently with my Stack layer, with 14 mil trace width and 6 mil gap in between diff pairs, I should match the 100 Ohm Differential Impedance, with no ground plane underneath, isn’t it ?



As far as I understand, is that the diff pairs should be the most parrallel as possible to make the impedance the same all along the signal.

I found a Altium article about designing Differential pairs without a ground plane :

https://resources.altium.com/p/diffe...und-it-problem

[qdrives]

1a) What is the reference of those signals?
1b) If you cross a gap as the signal goes from referencing Earth to Gnd, place a capacitor there so that the high frequency signal can cross.
1c) If you should not place Gnd below the magnetics, then you should definitely not place any signal lines below it.

2) Do the length matching in the corners or close to the point where the mismatch would occur.

3) Take some memory with 8 data lines and a clock. If the clock is short compares to some data lines, what value would the chip see when the clock arrives?
However, with GB ethernet, as far as I know it is 2x Rx (+ & -) and 2x Tx (+ & -). Keep the Rx'es about the same length and the same for the Tx'es.

https://www.youtube.com/watch?v=QG0Apol-oj0

[Jere]

Thank you very much for your response !

1a) I’m not 100% sure, if I understood well. As far as I understood Diff paires, there are reference to each other within a diff pair TX (+ and -). But I use POE+, so the 48V injected is reffered to GND of the board. I show you a Schematic to show that :


1b) I think C9 from my shematic does this job
1C) it does makes sens, I didn’t realize that, thank you, So I will rethink the way I route, and place component, thank you for this !

2) Thank you, yes I read about that, I was wondering if by doing length matching, I loose some symmetry, soi t felt like I have to make a choice between keeping same length or keeping symetry. But Your answer give me a clue, that is prefferable to loose some symetry, but to better match length (I’ve read that 50 mils, length difference is acceptable)

3) Yes thank you, it makes a lot of sens as well. I will check length are quite similar for both Rx and both Tx.

Thank you a lot, it helps greatly !


Jere

[qdrives]

1a) I do not remember if it was the mentioned Rick Hartley video or another one were he states that most differential pairs are just two single ended ones. On a PC the signals reference the Gnd return plane and in the cable they reference each other. If you have a phy, the signals reference the Gnd (return) of the phy.

1b) No, C9 goes from "Earth" to the center taps of the transformers (via R+C). However, this schematic seems a bit different compared to the layout. The layout looks like RJ45 -> magnetics -> magnetics -> RJ45.

2) The amount of mismatch depends on the allowed skew the receiver can handle. Again, Rick Hartley explains (somewhere).