XHRA-2HPA USB termination

Technical discussions around xCORE processors (e.g. General Purpose (L/G), xCORE-USB, xCORE-Analog, xCORE-XA).
Hello
New User
Posts: 2
Joined: Sat Mar 11, 2017 11:31 pm

XHRA-2HPA USB termination

Postby Hello » Sat Mar 11, 2017 11:38 pm

Hi,

i have a question about XHRA-2HPA USB connection.

1) Are serial resiitors in DP DM signal lines required? Or they are included in XHRA-2HPA?

2) What is USB Rtune resistor?

Thanks for answers.
User avatar
mon2
XCore Expert
Posts: 743
Joined: Thu Jun 10, 2010 11:43 am
Contact:

Postby mon2 » Mon Mar 13, 2017 1:31 pm

Hi. The series resistors are usually applied into USB designs to allow for tweaks for the impedance controlled traces. Being a USB 2.0 design, you must design these USB traces to be impedance controlled @ 90 ohms. When submitting your PCB fileset to your production shop, highlight these pair of lines and alert the shop that you require the traces to be impedance controlled @ 90 ohms for USB 2.0 speed. The shop in return will then adjust the same traces to meet this request based on the laminate used for your PCB. A good PCB shop will also offer test reports using TDR equipment to confirm that the finished PCB is able to meet the requested impedance (our shop charges + $10 for this report). We use Tiefa Circuits in Shenzhen, CN for such prototypes.

http://www.tiefapcb.com

Contact: Chantal

Suggestions:

1) allow for an EMI filter for USB 2.0 support using an industry wide 0805 footprint. You can source this EMI filter from assorted vendors including Bourns, etc. but the cost savings are best from offshore suppliers like Kingcore.

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

rex@mail.kingcore.com.tw

Above p/n. is for USB 2.0 application. They also offer USB 3.0 / USB 3.1 EMI filters and manufacturer for many of the big brands. We specifically selected this vendor for the referenced parts due to the common footprint shared by many local suppliers shown on Digikey and Mouser websites. Often, we found others to have a unique and single sourced footprint which is too risky for production.

We created a footprint for this part that allows for either assembly using the above EMI filter or can be bypassed using a standard 0402 resistor. The 0402 resistor can now be 0 ohms or 22-33 ohms, etc. if you wish to bypass the component. The 0402 pad is directly under the 0805 EMI filter footprint so there are no EMI stubs. Can share more details if there is an interest. We have done the same with our USB 3.1 Gen 1 designs and have working products based on this idea. The end product was tested to run for days non-stop with zero errors in our gigabit USB dongle design.

2) do add support for EMI ESD protection onto the USB connector - this is mandatory unless you are ok with RMA of field damaged products. RMA will lead to a poor end user experience and will quickly tarnish your reputation. We throw the kitchen sink into our designs and can sleep at night knowing we have designed a product that is of quality. For ESD protection, review the devices from Bourns, etc. and use a common footprint from Socay (Shenzhen, CN). They are a leader in the ESD protection business.

ULC0524P is a device we use for our USB 2.0 designs for ESD protection

http://www.socay.com/upfile/201407020248027678.pdf

Part Number: ULC0524P
Unit Price: 0.042 USD/ pc

3) The Rtune resistor is usually for an internal USB / Ethernet / PCI Express PHY and is specified by the silicon supplier to be 1% in accuracy. It is required and should be the value shown in the XMOS reference schematics.

Summary: If you design with the proper impedance controlled traces then the series resistors are not required. However, if the traces are not correct on the PCB design or during the PCB production ( the laminate used can throw off the impedance so the PCB shop must be involved to support this request ), the USB design will face problems. Seriously consider to insert the EMI filter with the 0402 bypass pads into your design. The EMI support is in our opinion mandatory, as ESD does kill. Just review this forum about ghost stories of dead XMOS designs.

Be cautious about how you will program the flash memory device for this controller. You must do this initial programming:

a) out of circuit before soldering the flash onto the PCB or
b) consider a method by which you will place the XMOS CPU into reset (ie. will tri-state the QSPI flash pins) and then use an external SPI flash programmer to inject the XMOS binary code
c) only once the factory code is uploaded will you be able to use the USB interface to maintain the XMOS code out in the field

Feel free to post your final schematic and PCB layout for a review before building the bare PCBs. Can share the footprint for the same EMI filter on request - need to find the related project upon reaching the office.
Hello
New User
Posts: 2
Joined: Sat Mar 11, 2017 11:31 pm

Postby Hello » Mon Mar 13, 2017 7:59 pm

Hi!
Thanks for answer very much! it was really very usefull.
It's my old design (prototype), it works, but I want to improve it.
Image

Can share more details if there is an interest.

Sure!

The end product was tested to run for days non-stop with zero errors in our gigabit USB dongle design

How you check usb conection for errors?
User avatar
mon2
XCore Expert
Posts: 743
Joined: Thu Jun 10, 2010 11:43 am
Contact:

Postby mon2 » Tue Mar 14, 2017 9:33 pm

Here is the suggestion we are making for the EMI filter / 0402 resistor bypass PCB landing pattern which should meet your requirements. We are doing the same for the USB 3.1 Gen 1 (aka USB 3.0) and USB 2.0 lines on this gigabit ethernet dongle design.


Image

Image

Using this idea, you can stuff the Kingcore EMI filter (common to other brands from Digikey / Mouser) or series resistors to suit or bypass with 0 ohms @ 0402 footprint.

Return to “Processors”

Who is online

Users browsing this forum: No registered users and 8 guests