Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

USB diffential line thickness confused

Status
Not open for further replies.

htekin42

Member level 2
Joined
Dec 10, 2012
Messages
45
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,286
Activity points
1,699
Dear All,
I am designing a board with FE1.1s and FTDI chips which are FT232RL and FT4232HL.

I am using 2 FE1.1s chip and get 4 usb port and different quantity serial port according to device model.

I have a question. I now that High Speed USB lines should be differential and they should be 90 ohm in differential. I am little bit confused. I used the saturn pcb tool to calculate impedance of lines.
I designed the board as 2 layer and top and bottom planes are Ground polygon. Gap is 0.245mm and PCB thickness is 1mm or 1.6mm, FR-4 standart and 1oz copper. When I calculate PCB tool, it gives me 1.2mm width of line. It is very bold line. How I can do correct line width. Also when I checked a few boards they have a line as seen in picture. What that is mean? I mean why designers make this kind of stuffs. pcb.JPG
Thanks
 

Hi,

How long are your traces?
Keep them short, then the two traces are not that critical.

Klaus
 

They lenght is around 80mm because of mini pci connector. We have a minipci gprs modem according to configuration of product. We have to keep that zone clear because of adding pci card in installation or in the future. I asked the question because we will going to use gprs modem in 3G band and it need to be full speed USB bus. Thanks
 

Hi,

For 90 Ohms differential impedance expect about 7.5 mil trace width and 7.5 mil spacing. But in detail it depends on PCB parameters.
I assume there is something wrong with your pcb tool data. Please check all values again.
Maybe crosscheck with another pcb tool.

Klaus
 

You must not make a right angle corner in your layout for the USB data lines, you must use a curved line. Also in the picture you showed the lines are made longer so that the propagation delay for all lines is the same, note no corners only curves.
 

For 90 Ohms differential impedance expect about 7.5 mil trace width and 7.5 mil spacing. But in detail it depends on PCB parameters.
True for a ground plane distance (substrate height) of 4 or 5 mils. The OP has the tenfold height.

Achieving small low impedance transmissions lines on a two layer PCB is difficult. The best solution is to make a (differential) coplanar waveguide with ground, I understand post #1 so that you already have it. Requires via fences for the ground pours. Use a smaller differential and ground separation gap according to the available technology, e.g. 150 µm. You won't get much below the reported trace width though.

You are asking about high speed in post #1 and full speed in post #3. Full speed doesn't require impedance matching for a 80 mm line, high speed does.
 

Hi,

True for a ground plane distance (substrate height) of 4 or 5 mils. The OP has the tenfold height.
True, Sorry. Somehow I thought of a 4 layer design and used my standard values...

Klaus
 

You must not make a right angle corner in your layout for the USB data lines, you must use a curved line. Also in the picture you showed the lines are made longer so that the propagation delay for all lines is the same, note no corners only curves.
Sorry but this is rubbish, you don't need curves, 90 or 45 deg corners will suffice.
The illustrated routes are not USB but length matched lines, USB lines should run adjacent to each other, broadside coupled. Similar to shown below.
 

Attachments

  • 8GT_Extreme.jpg
    8GT_Extreme.jpg
    79.2 KB · Views: 83

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top