Hi,
I have a question regarding differential pair routing. I am using a USB connection in my board. There are differential pair called D+ & D- in USB connection.
The pin is connected from usb connector to the cp2102N type of chip which is usb-uart converter chip.
In between these connections there is a diode connected to the ground. This is creating an issue in pcb layout design. The differential pair can not be consistent from the start to the end(see pictures).
Is there a way to solve this problem without deleting the diode? Or can I change the ratsnest connections? or is it okey to route a single wire for a shorter distances?
The ratsnest keeps going until your connector, just continue the routing from the corners, I personally would route the tracks from the chip to the connector and then simply use single track routing to route the diodes.
There are a few protection diode arrays out there for USB ports. Check the parts datasheet for the recommended differential trace routing. There will generally be a change the pair spacing at the protection diodes. Just make sure the traces are symmetric and the deviations are as short as possible.
For example, this was routed as differential pairs in Kicad. I did a differential pair route from the connector to the pads on the protection IC, then another differential pair route from my USB IC to the protection IC from the other side:
Means there are kind of two ways to do this thing. One is to directly route the differential pair to the IC from the connector and then route separately for the diodes a single track. This is fast in my opinion.
Another is to look at the datasheet and tune the length of the diff. pair in kicad at near diode and route finally to the IC from the connector.
I will see which is in my case which helps more… Thanks…!
I am using LESD5D5.0CT1G diodes, these are used for ESD protection and transient voltage events.
There is no mention though in the datasheet about the diff. pair but the PCB design guide of my microcontroller has suggestion that the differential pair should be surrounded with GND pour and there should also be a ground layer below the copper layer.
My board design is almost finished accept that I have some difficulties in these diffrential pair routing which keeps popping up in different ways.
This time my question is that is it allowed to have a via between the pairs? the issue is that my D+ & D- lines from USB are flipped other way round at FT2232 kind of chip. Hence, I have to use at-least one via for the connection. (see picture below.)
The chip’s base is having ground pad so there is no way I can take a kind of U-Turn from the other side of the pad !!
I am using the Kicad’s inbuilt impedence calculator for the differential pair. It is recommended to have an impedance of about 90 ohms/-15%.
The thing is that I get around 110 ohms as an impedance with my current design. Other thing is that the with some parameters tuning like increasing the trace width, length etc, I can decrease it to nearly 90 ohms.
But my question is that is this method of counting an impedance theoretically really reliable?
Also, how much strictly the differential pair design recommendation should be followed?
Any online resource could help me on these. So do not hesitate to suggest.
Well, unfortunately the CP2102N-A02-GQFN28 has pinout where D+ comes before D- hence making diffpairs to cross when used with standard surface-mount USB connectors.
One way is to use the kind of connector you ended up with, another way is to put CP2102 on the bottom instead of top.
Its maximum data rate is 12 Mbit/s so from the signal integrity standpoint you most likely will get away with a sub-optimal routing. Though its electromagnetic emissions will be higher (if you care about that).
You could also do something like this. But you should have a good GND plane (best on a separate Layer). It is important to have a GND Via near each USB Via.
