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.
Thanks
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
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.
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.
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.
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.