Topics

SD-24 differential TDR on USB cables

Gudjon Gudjonsson
 

Hi list

Hope the question is not out of the scope for the list but...
I want to do something useful with my CSA803c. A few years ago I made an
instrument with USB connection to a PC. The problem is that when the
USB packets are sent the instrument radiates above allowed levels. Luckily
there are USB cables available with ferrite rubber that fix the problem but
they
are expensive and may go out of production.

The problem irritates me and I want to understand it. My idea is to make
differential TDR measurements with my CSA803 and SD-24 into USB
cable and into the PCB.

Are there any SD-24 to USB connectors available?

Thanks for any suggestions.

Cheers
Gudjon

Leo Bodnar
 

Hope the question is not out of the scope for the list but...
Well punned!

My idea is to make differential TDR measurements with my CSA803 and SD-24 into USB
cable and into the PCB. Are there any SD-24 to USB connectors available?
You can buy surplus LeCroy or Agilent one https://www.ebay.com/sch/i.html?_nkw=USB%20test%20fixture
The easiest path is to just make one yourself. It's really just SMA or 2.92 to USB-A or USB-B. Single ended USB cable impedance should be 45R. Differential - 90R. But with TDR you don't need to do anything special to match the impedances - you will see the step.

It is tempting to make a PCB that fits directly over SD-24 connectors but I would expect their centres not guaranteed to be precisely spaced and axis parallel.

Something like this is easy to make: http://www.hyperlabsinc.com/datasheets/hl9801.pdf

Leo

Harvey White
 

On Mon, 5 Feb 2018 16:49:09 +0100, you wrote:

Hi list

Hope the question is not out of the scope for the list but...
I want to do something useful with my CSA803c. A few years ago I made an
instrument with USB connection to a PC. The problem is that when the
USB packets are sent the instrument radiates above allowed levels. Luckily
there are USB cables available with ferrite rubber that fix the problem but
they
are expensive and may go out of production.
I've seen clip on ferrite filters to reduce radiation. Had you
considered putting something like that on a conventional USB cable?

Harvey



The problem irritates me and I want to understand it. My idea is to make
differential TDR measurements with my CSA803 and SD-24 into USB
cable and into the PCB.

Are there any SD-24 to USB connectors available?

Thanks for any suggestions.

Cheers
Gudjon


Gudjon Gudjonsson
 

Hi Leo and Harvey

I will try to build something similar to HL9801 (and buy one if I fail).

I've seen clip on ferrite filters to reduce radiation. Had you
considered putting something like that on a conventional USB cable?
I tried with all kinds and nothing worked until I found these cables:
http://kgs-ind.com/wp-content/uploads/products/pdf/LNC-Noise-Suppression-USB20-Cable.pdf

But my question is more on how I can use my old Tek tools to do useful
measurements
to predict where the EMC problems are if they occur.
If I can characterise different USB cables and PCB's without having to
build a full
circuit and go to the EMC laboratory, I will say that my CSA803 investment
has paid back :)

/Gudjon

Leo Bodnar
 

Gudjon,
If your goal is to pass EMC test then my personal opinion is you are wasting your time starting with TDR - however fun it is.
I would try replicating the problem first before attempting to solve it. I don't know what you have failed on but you can do very basic troubleshooting with makeshift LISN for conducted and SDR with few DIY field probes for radiated. If you have your test house reports try to replicate the test results (at least roughly) and then do whatever necessary to suppress the peaks that are above the limit. If you can see the offending signal on your cheap receiver and you know that you have failed by 5dB try to reduce it by 10dB before going back to the test house.

Are you sure that the problem is caused by USB interconnects? You might have problems elsewhere but they coincide with bursts of USB traffic.

What speed is your USB bus running at? Place common mode chokes on the USB PCB traces and any other cables coming out of your product.
If you use FS or LS USB don't use measly HS choke, go for maximum impedance that still does not degrade the signal.

Leo

Gudjon Gudjonsson
 

Hi Leo


On Wed, Feb 7, 2018 at 9:53 PM, Leo Bodnar <leo@...> wrote:

Gudjon,
If your goal is to pass EMC test then my personal opinion is you are
wasting your time starting with TDR - however fun it is.
You are right, it is fun, I just made a connector and tested before anyone
could advice me not to :)

I would try replicating the problem first before attempting to solve it. I
don't know what you have failed on but you can do very basic
troubleshooting with makeshift LISN for conducted and SDR with few DIY
field probes for radiated. If you have your test house reports try to
replicate the test results (at least roughly) and then do whatever
necessary to suppress the peaks that are above the limit. If you can see
the offending signal on your cheap receiver and you know that you have
failed by 5dB try to reduce it by 10dB before going back to the test house.
Are you sure that the problem is caused by USB interconnects? You might
have problems elsewhere but they coincide with bursts of USB traffic.
I am pretty sure it is USB since the high quality USB cable solves the
problem.
Two design rule are broken on the PCB, the USB line is 110mm but should be
max 50mm however it is impedance matched.
It goes through the PCB two times but should stay on the same side.


What speed is your USB bus running at? Place common mode chokes on the
USB PCB traces and any other cables coming out of your product.
If you use FS or LS USB don't use measly HS choke, go for maximum
impedance that still does not degrade the signal.
I am running at high speed, 480 MBits.

I tried adding chokes, both on PCB and on cables but without success. The
only thing that works is the USB cable mentioned above.

You may be absolutely correct but I see some difference using different USB
cables and I want to correlate the results with EMI measurements.

If I can make tests on un- or partly populated PCB's I have gained a lot
and I hope to be able to do more general termination tests with the SD-24
TDR.

/Gudjon

Leo Bodnar
 

Gudjon,
Thanks for the information.
Please share the results when you get to the bottom of it. I am interested in both HS USB design and CSA803 TDR use.
From what I understand EMI problems from USB can come from either coupling to another signal or mismatched differential USB signal converting to common mode.
USB signal is not truly differential - each packet ends with SE0 state where both differential lines go to same level. SE0 = single-ended zero.
Leo

David Thomas
 

...pretty sure you have broken the 2 "fundamental rules" of high speed PCB design:

1) keep track lengths SHORT SHORT SHORT!

2) keep tracks on the SAME layer along the path (vias cause large impedance variations in the transmission line - which cause EM to be radiated...)

Think you should consider a board re-layout with those in mind - place the USB device RIGHT NEXT TO the connector and put the tracks on the UPPER layer with a signal ground plane on the NEXT layer beneath.


While you are at it, DONT let the tracks cross over any ground plane boundaries - if you do, the return path for the signal has to run around the edges of the ground planes to "get home", which forms a great loop antenna \ signal radiator, emitting loads of EM interference...

Other tips - maximise clearance from other parts of the circuit - and if you are using ground plane on top of the PCB too, "stitch through" to inner ground layers regularly (every 3-5mm?) with small vias to keep the ground impedance low... its just like laying out for RF (VHF\UHF?) , so you may pick up some tips from websites dealing with this too...

If you are using TDR I guess you have already done the track calcs to ensure the correct track impedance for that type \ thickness \ dielectric of PCB material?

Non-obvious one - if any SMD components on the tracks have large pads, REMOVE the ground plane under these, as this also causes track impedance variation...

Also, try to use small SMD components to reduce pad impedance effects (0603, or 0402 if you \ your board assembler can stand it...)

Haven't done <much> USB layout myself, but have done quite a bit of high-speed digital video (270 - 1485Mb/s) so I think the same ideas apply.... I wish someone had told me all this 25 years ago, as it would have saved me a ton of hair-tearing and ditched PCB versions...!


Some \ all of the above may already be known to you - but it may help other readers...

Anyone else have some experience of high-speed layout like this? I would be grateful for any comments \ corrections on the above, as we could all benefit from this kind of info...?


Good luck!

--
Best Regards

David Thomas

*Design Engineer
2T Communications*

Leo Bodnar
 

I would like to correct my mistake - common mode impedance of the full/high-speed USB 2.0 cable is 30 Ohms ±30%
Differential impedance is 90 Ω ±15%

This is from Table 7-12 in USB spec 2.0

Thanks
Leo