USB differential routing - Page 1
Forum section: electronics / projects

author: shadewind
author_rank: Frequent Contributor
timestamp: September 05, 2011, 11:35:57 am
content: I'm using the FTDI FT232RQ (the QFN version of the FT232R) for a little USB-to-serial design I'm working on. I have some questions about the routing of the differential data lines:The characteristic impedance of each line is supposed to be 45 ? ohms if I understand correctly. My board is a two layer 1.6 mm FR4 board and using a line calculator (TXline) and assuming the dielectric constant for FR4 is 4.7, I calculate the micro strip width to 134.711 mil which must mean I'm doing something wrong. Or am I?For some reason, the pins on the FT232RQ are flipped with regards to the USB connector which means I must pass at least one of the traces down through a via and back up. According to most data sheets, this is very bad but according to most datahsheets but according to Lee W. Ritchie (http://www.speedingedge.com/PDF-Files/diffsig.pdf), it is not and he seems to know what he's talking about. What to do?

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: September 05, 2011, 11:52:14 am
content: This isn't an issue at USB low or full speed as data rate is only 12mbits/sec - it's only high-speed (480mbits) where you start needing to be more careful.

author: amspire
author_rank: Super Contributor
timestamp: September 05, 2011, 11:56:52 am
content: Mike is right.The FTDI FT232RQ is a USB 2.0Full Speeddevice which means the USB runs at 12MHz as apposed to aHigh Speeddevice running at 480MHz.So basically as long as the FTDI FT232RQ is close to the USB socket the tracks will be too short to behave like transmission lines.Richard

author: shadewind
author_rank: Frequent Contributor
timestamp: September 05, 2011, 12:17:22 pm
content: I figured as much but it would still be interesting to know what I would have done at high speed. Are my micro strip calculations wrong or is it just that my ground plane is too far away (1.6 mm)?

author: joelby
author_rank: Frequent Contributor
timestamp: September 05, 2011, 02:32:48 pm
content: Pretty much. As a rule of thumb, a 50 ohm microstrip trace width should be twice the thickness of the dielectric, or the same width as the thickness for 75 ohms.Your options could include using a 0.8 mm board, or a four layer board, where you could have a top-GND thickness of, say, 0.15mm.

author: shadewind
author_rank: Frequent Contributor
timestamp: September 05, 2011, 02:37:58 pm
content: Well, it feels good to know I'm doing it (at least somewhat) right at least and that it in this case doesn't really matter

author: ejeffrey
author_rank: Super Contributor
timestamp: September 05, 2011, 03:32:25 pm
content: Quote from: joelby on September 05, 2011, 02:32:48 pmOr use a coplanar waveguide.

author: plesa
author_rank: Frequent Contributor
timestamp: September 05, 2011, 03:44:08 pm
content: Quote from: amspire on September 05, 2011, 11:56:52 amThe USB 2.0 Full speed use the DDR signaling - 240 MHzMaybe you can find following document usefulUSB 2.0 Board Design and Layout Guidelineshttp://www.ti.com/lit/an/spraar7/spraar7.pdfAlso some useful information can be foundEMI Design Guidelines for USB Componentshttp://www.ti.com/sc/docs/apps/msp/intrface/usb/emitest.pdf

author: johnmx
author_rank: Frequent Contributor
timestamp: September 05, 2011, 11:54:33 pm
content: You only need to design a transmission line if the trace’s length is too long. When the trace is too short you don’t have to worry about signal reflections.The main question is: “How do I know when a trace is too long?”. Well, if the propagation time is more than one-half of the rise time, then the trace is too long.The rise time is given in the data sheet of the USB device (see note below for the Hub), and the propagation time is the trace’s length divided by the velocity of the electromagnetic wave. This velocity is the speed of light divided by the square root of the FR4’s relative permittivity (typically 4.0 to 4.5).Note: I read in previous posts that you don’t need to worry about transmission lines because this USB device works at 12MHz. Ok, but don’t forget that the USB Hub has very fast rise times even in full-speed, because it is a high-speed device.Modified:Actually the clock of the full-speed USB signal is 48MHz and not 12MHz as someone stated. 6MHz is for low-speed.You're right, 48MHz is the system clock and data clock is only 12MHz for full-speed.

author: seattle
author_rank: Contributor
timestamp: September 07, 2011, 05:49:28 am
content: I've done several boards now with Cypress USB 2.0 480Mbps controllers, and have never had a problem. I've done 4 layer boards with traces on the inner layers and outer layers, and double sided boards with traces above ground planes and above empty PCB. Short traces, long traces. In fact, I've never had trouble with USB integrity. Now, getting the USB to talk to the FPGABut that's another issue not related to integrity.I'd say lay it out as close as you can to vendor recommendations without going overboard and you'll be pleasantly surprised.PS. I am continually amazed at how well stuff works today. 20 years ago it was a chore to get 9600 baud working over more than 10 feet. These days, I've run ethernet 20 feet over twisted wire wrap wire and it never complained.PS. If you get a SW-based USB analyzer, you will be able to see problems related to signal integrity.

author: Bambur
author_rank: Regular Contributor
timestamp: September 09, 2011, 12:22:41 pm
content: Quote from: ejeffrey on September 05, 2011, 03:32:25 pmWhy not to use coupled microstrip lines?