8-ch audio card USB Bus Problems

[hamtam]

Thank you for the advice.

The Part of the PCB now looks like:


In the datasheet of the xmos is only recommended to protect the VBUS and GND of the USB Bus. I hope it will be OK and the ESD will dischare at the USB shield and do not reach the D+ D- lines.
I give the ESD Protection on the data lines a try in the next development phase. Do you think it is necessary to have a copper keep out at the USB data lines on all layers?
The design is currently still a bit sensitive.

[hamtam]

Just for the nosy ones, after I cut and removed the copper the former design is also working with ESD protection as well.

It is easy to see where I did the cuts.

[mon2]

Excellent. Thanks for the updates and pics.

On the ground guard, the following is the best summary on this topic after some searches:

source:
https://www.quicklogic.com/assets/pdf/a ... P-RevC.pdf




Summary:

1) The ground guard is only on the surface (top side) layer.

2) For USB 2.0 HS support, you are required to keep the ground and power layers to be solid as shown in this and other documents.

3) 4L is recommended. 2L is too risky yet many low cost houses use this practice. Guessing they will also face some compatibility issues such as the quality and length of USB cables they can use, etc.

4) For proper support, recommend that you search out USB 2.0 HS compliant cables. If possible, ask the supplier if they have TDI # for the cable to confirm the cable has been properly tested. Most will offer a cable and say "it works". The formal test report, if real, will save you some headaches later on. As a general rule, if you purchase a true brand name cable (ie. Molex, etc.), you should be fine to know that the cable is ok @ HS on USB 2.0. Many vendors out there and pretty sure my mother is making them as well as they are so common.

5) The new layout looks great but please do insert proper ESD protection and if practical even EMI filter. We use Kingcore EMI filters which are a common footprint so you can use almost any other supplier to get started and then buy from Kingcore Taiwan at much lower costs.

USB 2.0 EMI filter (choke)

KC p/n.WCM-2012-900T
Price USD0.04/pc FOB Taiwan
SPQ=3000pcs/reel
MOQ=36000pcs per shipment
LT=30days


Rex Chen
Your Best EMI Solution Partner
鈞寶電子工業股份有限公司／King Core Electronics Inc.
O.Phone: +886-3-4698855#201
e-mail: rex@mail.kingcore.com.tw
Address: 台灣桃園市平鎮區南豐路269號／No.269, Nanfong Road, Pingjhen City, Taoyuan County 324, Taiwan

6) We use Socay ESD protection devices but use what works for you. The Socay device we use has the same footprint as the Littlefuse part but Littlefuse is much more expensive. As noted a few times in these forums, ESD is real and highly recommend to use such parts so you can enjoy selling and not hearing complaints from end users and negative reviews. Our philosophy, build a product that you would buy.


7) Finally, do submit your PCB files to a good PCB shop to request that they can support impedance control for this region of the design. Only then proceed with an order. Varying with costs, some PCB shops do not offer impedance control but will be much lower in costs. Ok if you are 100% sure that your gerbers are 100% ok to use as-is. For now, allow the PCB shop to control this area of the design with their laminate as required.

8) If you need some recommendations for good PCB shops, let us know or post back.

[hamtam]

Thank you for your advice it really helps ma a lot.
I use the USB 2-0 Design Guide from TI, which seems to be also reasonable.
http://www.ti.com/lit/an/spraar7g/spraar7g.pdf

After I modified a second card with the knife the card still produce only signal failures on the USB Bus. It enumerates but USB Audio is not possible.
I will check how I can add ESD protection on D+ and D- . But the card has a good ESD Protection for VBus already. I will ask our Manufacturer to test the Impedance of the PCB. I think this is a good Idea.

[hamtam]

In the next few days I will order the next Prototype PCB. I added EMI and ESD Protection. I used the Parts from wuerth elektronik http://www.we-online.de

[mon2]

Would you please supply the datasheet links for the EMI Wurth part that have been applied in this design?

Found the datasheet for the EMI filter from Wurth and that part looks suitable for your USB 2.0 HS use.

A few comments:

1) The Wurth EMI filter is 0603 footprint. When we did our USB designs, we found that 0603 footprint was not very common from our suppliers in Asia. Perhaps times have changed now.

2) For the above reason, we applied an 0805 footprint for the solder pads. Using an 0805 footprint, you can easily source a perfectly suitable emi filter from Asia for $ 0.04 USD each in T&R qty. Wurth is very good but they do purchase from other manufacturers in Asia under private label. If practical, consider to apply a landing PCB pattern that can be used for 0603 or 0805 footprints during assembly time. Not a PCB designer but our designer basically made the landing pads longer to allow for either version of the EMI filter to be used. Our current designs permit the use of 0805 or 0402 (for zero ohm bypass if required) of the EMI filter.

0805 footprint EMI filters for USB 2.0 are quite common:

For example, Bourns SRF2012-900YA looks like a competitive part in this footprint @ $ 0.10 USD in single T&R qty from Mouser which is not too bad.

https://www.mouser.com/ProductDetail/Bo ... pgtZJag%3d

Summary: Do not get locked down to a rare and unique footprint because it appears that you are paying a premium for this smaller footprint.


KC p/n.WCM-2012-900T
Price USD0.04/pc FOB Taiwan
SPQ=3000pcs/reel
MOQ=36000pcs per shipment
LT=30days

Above p/n. is for USB 2.0 application - datasheet is attached to this post.

Contact details:

Rex Chen
Your Best EMI Solution Partner
鈞寶電子工業股份有限公司／King Core Electronics Inc.
O.Phone: +886-3-4698855#201
e-mail: rex@mail.kingcore.com.tw
Address: 台灣桃園市平鎮區南豐路269號／No.269, Nanfong Road, Pingjhen City, Taoyuan County 324, Taiwan

[mon2]

Do you have the in-rush current protection on the Vbus rail? Please see the datasheets for the XMOS CPU and search for the following (taken from the XU208 datasheet):

(components highlighted in yellow) - without these parts or equivalent, the XMOS CPU may face permanent field damage upon docking for your device with a USB cable, etc.

A more elegant solution is to place a low cost USB load switch (Diodes Inc. offers some under $ 0.10 USD; AP2331 - models with higher current support are available) with more features than these parts.




The following traces under the ESD device should be straight from one pin to the other - as drawn now, the traces are not symmetric - we use straight lines in our PCB designs under our flow through TVS ESD devices:




From TI notes on USB PCB layout guidelines - the middle drawing is much like your PCB layout and is not recommended:



For a cost reduction on the TVS ESD devices, contact Socay (Shenzhen, CN). They should be able to supply a drop in replacement for this part.

Your new layout is much better than the first and should be fine. Given that your modified PCB is working ok, the USB spec is a bit tolerant to deviation.

[hamtam]

I still think, that the inrush part is not necessary on my board. Because it is a bus-powered Device and the Inrush Power control should be on the Host side?
I use a Buck Boost device (ADP2504) to maintain continuously 5V for my application. The IC has a soft start an the input Capacity on VBus is about 10µF which is within the USB spec.
Do you think that my consideration is reasonable?

[mon2]

The buck-boost regulator looks like an expensive part and solution. If you have this regulator mated with your Vbus of the XMOS device then you should be fine due to the soft start feature. Analog is usually very expensive but is good. A cost reduction would be to apply the network of parts recommended by XMOS instead of this regulator.

[hamtam]

It is really a pity.

• I now matched the impedance with the PCB manufacturer to 90 Ohms
  I add a transformer for EMI reduction
  the USB tracks differ less than 2mm

Unfortunately I still incur the USB signal problem! The XMOS Chip I use seems to be really susceptible on the USB Bus side.
When I force USB Full-Speed only 2 channels of 8 are available.

Code: Select all

            XUD_Manager(
                    c_xud_out,
                    ENDPOINT_COUNT_OUT,
                    c_xud_in,
                    ENDPOINT_COUNT_IN,
                    c_sof,
                    epTypeTableOut,
                    epTypeTableIn,
                    p_usb_rst,
                    clk,
                    1,
                    XUD_SPEED_FS, //instead of XUD_SPEED_HS
                    XUD_PWR_BUS
             );

Our current layout without the ESD protection but with the EMI transformer:


Do anyone know a consulter who can help us finxing the design?