USB diff pair impedance matching, connecting USB, Ethernet shielding

[jldesigns.eu]

Hello.

I'm currently designing a board with USB host support.

I've made some calculations regarding impedance matching for diff pair on the board, and got some quite thick tracks.

Board is standard Fr4 1.5mm thick 35um copper.

For polygons on the bottom + surrounding coplanar i've got
- trace width 0.6mm
- trace separation 0.23mm
- ground strip separation 0.23mm

And that gave me a differential impedance of 92.15Ohm (USB cable is suppose to be 90Ohm

Without coplanar the thicknes went to some silly 1.1mm

And I'm wondering... I've never saw tracks so thick on the PCB. I have a lot of dev kits, other devices, most of them double layers 1.5mm FR4, and never saw tracks thick. Most of the time its just normal 0.2 - 0.3mm track, with plane below and soround. Did i missed something, or its just not so important to fallow this rules. In my case overall length of the data liens is around 40mm.

The second question is about the USB shielding. I'm designing a host module. I've went through few doses of schematics and there are few routines there:
- direct connection to GND
- direct connection to GND trough thin track
- 100nF or similar cap to GND
- 1MOhm resistor in paraler to 100nF cap to GND
- Ferrite bed (600Ohm @100Mhz most of the time) to GND

Whats the best approach? Do the same rules apply to Ethernet?

Thanks in advance.
Kuba

[Dago]

Your board is way too thick for impedance matched traces.

Usually for such boards you use something like a 4-layer board where the top and bottom layers are usually 180um away from the internal planes. The much thinner board will result in much thinner track widths for the same impedance.

Also do notice that for USB there is a specified common-mode impedance of 30 ohms.

[jldesigns.eu]

Yep sure, I got that before.

But in the end there are hundreds of devices using a 1.5mm double layer boards using usb with thin tracks...

So I should just not care?

Any help with the shielding?

Take care

[wraper]

But in the end there are hundreds of devices using a 1.5mm double layer boards using usb with thin tracks...

Because they are either low speed USB devices where you basically don't care about impedance or some Chinese crap.

[free_electron]

But in the end there are hundreds of devices using a 1.5mm double layer boards using usb with thin tracks...

Because they are either low speed USB devices where you basically don't care about impedance or some Chinese crap.

<-the above ...

you really need a plane to do it properly.
you need to know the stackup as well

[jldesigns.eu]

Ok, any advice's on USB shielding and ethernet?

Also additional question whats is better for esd protection - 2xPGB1010603 for each data line or a single PRTR5V0U2X and why in few words.

[T3sl4co1l]

If your device enumerates Full Speed, it's not doing LVDS, it's doing 3.3V CMOS.  You can afford to filter this quite a bit (~30MHz lowpass?), and should, in combination with a TVS or clamp device to protect the chip.  Impedance doesn't matter much, at least until you have enough trace length to matter (a nanosecond or two worth, corresponding to the risetime).  If you have a long distance between PHY and filter or connector, you may want some RLC components to dampen the high impedance transmission line stub; values would be in the 50 ohm, 33pF range, and could be evaluated with the aid of simulation.

If it negotiates High Speed, it's doing LVDS and high bandwidth, and you don't get much bandwidth to filter (>300MHz), nor allowable capacitance to use clamp diodes, nor allowable unmatched transmission line length.

In both cases, you're probably fine if you keep the connector, protection/filter (if used) and PHY as close as possible.  It should be simple to maintain less than 1cm between all three, in which case the signal won't know the difference until GHz+.

Tim

[T3sl4co1l]

Ok, any advice's on USB shielding and ethernet?

Also additional question whats is better for esd protection - 2xPGB1010603 for each data line or a single PRTR5V0U2X and why in few words.

Shield directly to ground plane, and on to safety ground if mains connected.

Ethernet connectors, of the integrated variety, have everything inside for you, just add ground and PHY.  If you're building one up, you will need a jack, some chokes/transformers (available as a single component array), terminations for unused pairs or center taps, and a 1nF 1kV "ESD draining" capacitor.  Try to maintain characteristic impedance of the pairs, up to and through the transformer component.  These will likely be over bare board on the isolated area (which is fine, because they are separate pairs in the cable as well), and over inner layer ground plane between transformer and PHY.  The PHY also needs termination resistors, because ultimately Ethernet is a source-load terminated signaling method (whereas USB is source terminated only -- part of the reason its cable length is limited).

Ethernet signaling ranges from ~1V Manchester coding at 20Mbaud (10BASE-T) to slightly less signal amplitude and much higher baud rate for 100 and 1000 modes.  100BASE-T uses faster rate and adaptive filtering; 1000BASE-T uses only a slightly faster rate than 100, all four pairs, adaptive filtering, and multiple levels per symbol.

Layout between transformer and PHY should be 50 ohm per trace (differential doesn't matter), with a bandwidth typical of the desired operating range.  If 10 is fine, you can be pretty careless, as with USB Full Speed.  If 100 or more is required, you will need matching.

Tim

[jldesigns.eu]

Thanks for answers.

The device is build on top of Atheros AR9331 based WiFi module. The module features a 100Mbps Ethernet and USB 2.0 Full Speed. Ethernet is going trough a HR911105A mag jack, according to application schematic (4x49.9Ohms etc).

I would normally connect the shields directly to ground as well, but the thing is, every guidelines I read about USB says that the shielding should never be connected to signal ground...

My current layout is as attached.

J1 is USB and J2 is Ethernet. I had to route TX_N and RX_N for the Ethernet on the bottom (vias close to C1, C2 designators), except that, there is only GND poligon below the signal tracks for USB and Ethernet. I've planned to use some ferrite bead to connect the shielding to ground. I'm planing to short them out, and if need I can cut the trace and solder a resistor, cap, ferrite bead. Currently impedance for USB is matched, as in first post.

I'll number the issues:
1. D11 and D12 are for ESD on USB i've wanted to go for PGB1010603, should i change them for PRTR5V0U2X and if so, why?
2. Should i change anything with shielding of USB or Ethernet?
3. Should I change anything else in the layout?

[Jeroen3]

Fix your polygon, you have very thin lines under the components.
I do not see the USB ESD diodes. You can use the NXP ones you've named, or the ST USBLC6-2. Which is optimised for routing diff pairs.

Did you read this?
http://www.usb.org/developers/docs/hs_usb_pdg_r1_0.pdf

I never connect chassis to digital ground, but it might be wrong. This is because I never have any metal chassis, so there is nothing to shield anymore. Usually just a bare board or plastic case. I would connect it to mains earth, if I have that available. (Or power DC ground before the isolated supply) An 2 kV 1 nF cap (ethernet is 1.5kV by IEEE) will have similar effect of an isolated power supply.
You MUST connect chassis to earth if your casing is metal.
Also, shielded RJ45 plugs (and CAT cables) are quite rare and more expensive than "normal" ones. You only rarely find one, and if you do there is a special reason for it. So you'll probably have metal shielding case around your device. So the ethernet chassis is rarely used.

I've found this document. Looks like to have some extra why's.
http://www.micrel.com/_PDF/Ethernet/app-notes/an-139.pdf

[free_electron]

no t-stubs on the connectors !

the metal chassis of the ethernet and usb need to go to a chassis ground.
that chassis ground needs to be coupled using a ferrite bead with system ground.
NEVER make chassis ground a closed loop around system ground ( antenna effect )
end legs of chassis ground should be shunted for RF energy to system ground.

[jldesigns.eu]

I'm getting smarter thanks to You guys. Thanks.



The device wont be in metal case.

So the TODO list:
1. replace PGB1010603 with USBLC6-2SC6
2. Connect Ethernet and USB shields together, and in one place trough a ferrite bead to signal ground.

Questions:
1. What exacly are "t-stubs on connectors"? only thing that comes to mind are TVS, yes?
2. Should i pour a shield plane below connectors, or pour it with signal ground?

[T3sl4co1l]

I would normally connect the shields directly to ground as well, but the thing is, every guidelines I read about USB says that the shielding should never be connected to signal ground...

Just because they are guidelines or appnotes doesn't mean they can't be flat out wrong.  Sadly, manufacturers aren't very particular about what they publish in appnotes.

J1 is USB and J2 is Ethernet. I had to route TX_N and RX_N for the Ethernet on the bottom (vias close to C1, C2 designators), except that, there is only GND poligon below the signal tracks for USB and Ethernet. I've planned to use some ferrite bead to connect the shielding to ground. I'm planing to short them out, and if need I can cut the trace and solder a resistor, cap, ferrite bead. Currently impedance for USB is matched, as in first post.

A ferrite bead is the absolute worst possible grounding for the shield. 

Consider this situation: ESD on the connector, or RFI or something like that.  If the shield is not firmly grounded to circuit ground, it will have some voltage over ground.  At 100MHz, ferrite beads have, well, whatever impedance they're rated for, which is usually in the 100 ohm range.  Hardly a short circuit!

If "ground" is at some voltage, that means all the wires inside the cable are promoted to that voltage as well.  Okay, so you have one ground wire that's tied to circuit ground, but that has quite a bit higher impedance to the other wires than the shield does.  So it has essentially no effect, at all.

The result is, now your D+/- signals have whatever AC voltage on them.  And USB can only tolerate about 1.5V common mode error before it's completely wrecked.

A single ESD event might corrupt an unlucky packet, so that's not necessarily a bad thing.  But RFI from various sources (motors switching on and off, lamp dimmers, radio transmitters..) can disrupt things on a much more frequent basis.  A few keep-alive packets get toasted and your connection drops.

Whereas with shield tied directly into circuit ground, the RF energy is carried over the circuit, so that it all goes to that potential, and little or no RF gets coupled into logic signals and such.

As for "signal" ground -- what signal?  Is this just a digital board?  Then no, no problem!   Even if you had small signals, the fact that the RF is carried around the board by the grounding means you have very little to worry about, so long as sensitive traces are well isolated by proper design rules -- solid ground plane (or stitched pours), not crossing sensitive and noisy traces, keeping respective traces short, etc.

I'll number the issues:
1. D11 and D12 are for ESD on USB i've wanted to go for PGB1010603, should i change them for PRTR5V0U2X and if so, why?
2. Should i change anything with shielding of USB or Ethernet?
3. Should I change anything else in the layout?

1. Probably a good idea.  It's not obvious how much good either will do against the pins of a USB device (or what they're capable of handling), but the PRTR one seems better (lower voltage drop, still low enough capacitance).

2. Definitely!

3. No idea -- do you have bottom copper too?

Tim

[jldesigns.eu]

Thank you for Your answer.

I have only digital grounds, no any analog stuff.

The board is folded with ground on top and bottom.

Will the way VCC to USBLC6-2SC6 is router be a problem (its marked on the "top comment.png")

I will leave the footprint for the Ferrite Beads, and will short them with a solder or 0Ohm resistors.

Now there is a polygon for shield on the top layer under connectors? Is that OK, or I should use a GND polygon there?

[T3sl4co1l]

Thank you for Your answer.

I have only digital grounds, no any analog stuff.

The board is folded with ground on top and bottom.

Will the way VCC to USBLC6-2SC6 is router be a problem (its marked on the "top comment.png")

Umm, probably not but I'd like to see a fat trace (20 mil?) there too.  That can be routed on the bottom, since there isn't much room to get it out on the top layer.

I will leave the footprint for the Ferrite Beads, and will short them with a solder or 0Ohm resistors.

Now there is a polygon for shield on the top layer under connectors? Is that OK, or I should use a GND polygon there?

0 ohm jumpers are better, but you still have probably 10-20 ohms at certain RF frequencies, plus the ground area acts like a resonator against the board ground, so the problem will be much worse at some unlucky frequency -- even less likely to be excited at random, but when it does, on that random day an FM transmitter starts up nearby, or something... wham, like magic it's down!

GND it all!

I like that very little is routed on the bottom, so you get a huge, solid ground pour on that layer.  The traces running off to the top right are kind of derpy, not being 'supported' by any ground, but maybe they don't need it.  I take it, this is also just the corner of a larger board, so some of the things hanging around aren't supposed to make sense from this small view.

Tim