I am designing a PCB and having issue with the impedance matching of the differential pair. I am using the guidelines of the IC manufacture to design my PCB. Here is the link of:
According to this guidelines, the differential pair (DP and DM signals of the USB) must have 90 ohm impedance to each other. But I am not able to match this impedance. I tried using different line width (10mils,15mils,20mils,25mils,30mils) of the differential pair but it doesn’t help me. Also, I tried using 0 ohm resistor in between that didn’t help as well.
The specifications of my PCB are- the conductor thickness is 2oz(2.8mils) and the dielectric thickness is 63 mils (using FR-4 and dielectric constant is 4.5).
Can anyone please help me in resolving this issue ??
Let me understand, you are trying to get a controlled impedance of 90 Ohms diff and 45 Ohm single ended on 2 layer stack up?
Yes! I am trying to get a controlled impedance of 90 Ohms diff and 45 Ohm single ended on 2 layer stack up
On a 2 layer board to get a controlled impedance of 45 ohm per trace you are looking at a trace width of about 140 mil for that 45 ohm target. On a 2 layer board it is not possible to achieverealistic values for the trace width due to the height of the trace above a copper ground which would be on the back side of the board. A typical FR 4 board has a height of 59 mil for the fr4dielectric
It wont work !. The alternate is to use a 4 layer board instead. "most believe this to be true" :) and it is correct for a standard microstrip topology that alot of people use.
However using a standard 2 layer 62Mil board it is indeed possible to get your diff pair of 90 ohms with smaller traces. You would need what is called a "Coplanar WaaveGuide Coupler (2 Center Conductors)
Basically this is 2 parallel traces with a ground plane either side of the traces above a ground.
In such an arrangement for your target impedance the parallel traces would be 20 mil for 90 ohms diff. This would be more manageable. Going to 100 ohms diff you would belooking at 15 mil parallel traces.
All the best.
Just a follow up.
You need something like this
So this is a diff pair with a Z of 90 Ohms.
Layer topology is 2 layers FR4 0.62, ER 4.5. 1/2Oz copper 1.4 mil.
Trace to Trace spacing = 6MilTrace to Top Side Wall Ground-Plane spacing = 6MilTrace width = 13Mil.Below the dif-pair is a solid ground (Bottom side of board) The vias on the top side gnd seed to the bottom side ground.The variable is the ER constant of the board. ER4.5 = Better than -30db returnloss. ER4.3 = Better than -29dB returnloss. Line is good to 4 inches long, 100Mhz to 1Ghz.
BTW don't use 2oz copper if possible. Better to use 1/2 Oz instead to etch better lines.
The guidance is a bit misleading. You don't *require* 45 ohm single ended. You do need 90 ohm differential. The 90 ohm diff pair can be achieved with a tightly coupled pair on the top. You could do CPWG as suggested by excelon or you can widen slightly and do just an edge-coupled microstrip pair.
If you had a line which was 45 ohm single ended, and 90 ohm differential then that would suggest an uncoupled pair and those dimensions are not practical on a 2 layer board again as excelon has mentioned.
What tools were you using to check your impedance? The calculator in Allegro/Orcad will get you the right values assuming your stackup has been entered correctly.