Electronics > Beginners

Mixed signal board: split or single ground polygon?

<< < (3/3)

Sparker:

--- Quote ---Seems not terrible.
--- End quote ---
:phew:

Thanks, Tim! That's an answer worth if not a textbook, but maybe one of these tutorials by AD/other companies discussing the ground separation topic!  :-+

What I didn't quite get is this (besides the 1 GHz magic, for which I don't have much experience to appreciate all of it yet  :)):

--- Quote ---break that ground bridge, and move the power trace over with the signals, so there is very little current imposed through the ADC area.
--- End quote ---
I assume you meant not breaking the bridge, but breaking the ground loop, so that it looks like at the attached picture, right? Or do you mean just pouring everything with the GND polygon (and thus, kind of, 'breaking' the bridge)? I intended to make that ground polygon on the left of the top layer as a separate return path for the analog power supply. Also J10 and J9 will not have any heavy currents run through them.


--- Quote ---The ethernet jack shield seems connected to the ground pour, along with the cap maybe C28.
--- End quote ---
Yes you are right.I have overlooked this problem. I don't quite understand though how it's going to affect my design if I am going to use unshielded Ethernet connectors with unshielded twisted pair.  ???
As for the case, this PCB will be in an underwater sealed metal tube with internal battery supply mounted on a dielectric platform. I will to connect the negative battery contact to the case. The Ethernet cable will only run for about 10...20 centimeters to another Ethernet switch.

T3sl4co1l:

--- Quote from: Sparker on November 14, 2018, 02:22:16 am ---What I didn't quite get is this (besides the 1 GHz magic, for which I don't have much experience to appreciate all of it yet  :)):
--- End quote ---

That's simple enough, just at a small enough scale that it ends up pretty high like that.

Consider the board as a single piece of copper.  Ignore the traces that are on it, ignore the functionality it has.  Consider all nets shorted together so it's basically a solid plane of copper.

The neck-down acts as an inductance, and the two full-pour areas act as capacitors (low frequency equivalents).  Thus you get a resonance between two capacitors in series with an inductor.

Given the dimensions, that resonance will come in the ~1GHz range, I would guess.

Frequency here is only a matter of scale.  A larger board might resonate in the 500MHz range, where a handheld FRS radio could interfere.  Or two boards joined by a short cable might resonate in the 200MHz range.  Or with short or long cables attached, 100MHz or less, where commercial broadcast radio, television and other sources would be a problem.

Now consider the board as it is.  There is ground providing such a path, but there are also traces routed in parallel with that bridging inductance, which will couple to it.  That coupling introduces some of the RF from that resonance.  Which means, equivalently: some RF at that frequency, if contained in the signals, can radiate out from that antenna structure; and external interference, if it happens to be strong enough and at an unlucky frequency (near the peak resonance), will couple into the traces.

You can draw an equivalent transformer circuit for this, representing what the signals will see, in terms of, say, a very small capacitor from a nearby noise source.

Well.  Maybe network synthesis is still a rather more advanced topic... :)

Speaking of cables, the same premise applies there, too: the longer they are, the more noise they can bring in, and they're bringing it right into the middle of the ADC area.  A better layout -- assuming you had the board area to accommodate it -- would have the cables near the slot/bridge, and the ADC stuff off to one side, so the noise currents do not cross the ADC section.  Also, RFI filtering on the analog signals is a must.

These are more considerations for proper commercial (CE approved) products, but you will find that practice very valuable if you go into (or are already!) design of such things.

For the amateur, if you don't mind occasional malfunction, or you are fine dealing with it in other ways (piles of ferrite beads on cables, wrapping the enclosure with tin foil, etc.), you don't need to worry about this.  Or, much of anything, really, just pour that board and route the traces however.  If it's not low noise in the 16+ bits range, I doubt it's going to matter much.



--- Quote ---I assume you meant not breaking the bridge, but breaking the ground loop, so that it looks like at the attached picture, right? Or do you mean just pouring everything with the GND polygon (and thus, kind of, 'breaking' the bridge)? I intended to make that ground polygon on the left of the top layer as a separate return path for the analog power supply. Also J10 and J9 will not have any heavy currents run through them.
--- End quote ---

Perfect!

Hey wait, if those don't carry heavy currents, and you're okay necking down the one trace... why do they need to be fat at all?  Just run a 0.25-0.5 mm trace up there and be done with it.  More space for ground fill!


--- Quote ---Yes you are right.I have overlooked this problem. I don't quite understand though how it's going to affect my design if I am going to use unshielded Ethernet connectors with unshielded twisted pair.  ???
As for the case, this PCB will be in an underwater sealed metal tube with internal battery supply mounted on a dielectric platform. I will to connect the negative battery contact to the case. The Ethernet cable will only run for about 10...20 centimeters to another Ethernet switch.

--- End quote ---

Oh neat, a submersible project. :popcorn:

Yeah, that's fine to ground anywhere.

Tim

floobydust:
It looks like the A/D's are exclusively powered off 3V3A. I can't tell where A/D VIO goes, it should run off 3V3D but I see no pcb trace.
I think RF return currents are going to make a mess of a split-plane as you have it.

If you want 16-bit or better performance, there are many things beyond pcb grounding to look after.
Missing any one design element will add noise to the A/D's and scuttle the best intentions.

Quiet rails are important, I don't see much for bulk capacitance or use of ferrite beads, or impedance-matching resistors on SPI to lower reflections.

Sparker:

--- Quote from: T3sl4co1l on November 14, 2018, 01:21:30 pm ---Well.  Maybe network synthesis is still a rather more advanced topic... :)

--- End quote ---
Allright, I think now I get the explanation!  :) If I get it right, the equivalent circuit should be something like this (the Paint drawing attached). If I understand correctly, that's also why they use differential I/O in high speed digital circuits, because the differential signals produce opposite coupling into these parasitic inductors.


--- Quote ---Speaking of cables, the same premise applies there, too: the longer they are, the more noise they can bring in, and they're bringing it right into the middle of the ADC area.
--- End quote ---
Do you mean the noise brought by a different level of ground at the other board I'm connecting? Actually this made me thinking, since my ADC is pseudo-differential, should I rather connect the external cable to the ground together with the negative ADC input, or connect the incoming cable's ground to the neg. input without connecting it to the ground?  I guess it would cancel out that imbalanced ground current between the board. FOr now I've put a jumper so that I can figure out what's better later.

floobydust, thanks for your further help with the ADCs!
Currently I am using the following schematic from the datasheet (see the attached picture). 3.3V analog supply is provided by a separate IFX117ME 3.3 regulator. I don't care about absolute reference tolerance for it, so the  power supply as reference is OK for me. The other IFX117ME powers the digital 3.3V bus, which powers the MCU and the Ethernet PHY. What do you think of it?

No, there are no ferrite beads, except for the Ethernet supply. There are also no resistors on the digital lines currently, but if these are so important, I will try to add them. By the way, I can also tweak the slew rate of the I/O of the MCU through its registers to address this issue.

T3sl4co1l:

--- Quote from: Sparker on November 14, 2018, 11:31:43 pm ---Allright, I think now I get the explanation!  :) If I get it right, the equivalent circuit should be something like this (the Paint drawing attached). If I understand correctly, that's also why they use differential I/O in high speed digital circuits, because the differential signals produce opposite coupling into these parasitic inductors.
--- End quote ---

Yes!  Precisely!  :clap: :clap: :clap:

Again, the coupling isn't very much, but it is nonzero, and this is how it happens.  :)



--- Quote ---Do you mean the noise brought by a different level of ground at the other board I'm connecting? Actually this made me thinking, since my ADC is pseudo-differential, should I rather connect the external cable to the ground together with the negative ADC input, or connect the incoming cable's ground to the neg. input without connecting it to the ground?  I guess it would cancel out that imbalanced ground current between the board. FOr now I've put a jumper so that I can figure out what's better later.
--- End quote ---

A differential pair isn't really needed if you use the cable in a differential manner.  Say it's coax (so, shielded to begin with), and isn't carrying much DC power, so the voltage drop along the shield is very small.  The voltage between signal and shield will be consistent along the cable.  Just make sure it's well grounded at both ends, and any (common mode) noise current will flow around and over circuit ground, rather than coupling into the signal.  (Again, we have that transformer action, primarily at the ends where the shield is broken -- and we must ensure it has low enough coupling so the signal stays clean.)

If it's screened multiconductor cable, the screen can be grounded (to enclosure or circuit ground), and the wires sensed differentially.  If unshielded... differential still helps, but you'll probably need filtering to be sure (which is fine if your ADC bandwidth is, say, 10s of kHz tops).

Tim

Navigation

[0] Message Index

[*] Previous page

There was an error while thanking
Thanking...
Go to full version
Powered by SMFPacks Advanced Attachments Uploader Mod