USB 3 Type C routing on small extension board

[Jackster]

I have a small PCB where we are extending out the USB Type C connection.

Require someone to route the trances from one Type C plug to a Type C socket.
Only need 5gbps and would prefer a 2 layer board to a 4 layer.



PM me with quotes.

[podericof]

Hi Jackster,
I strongly discourage to use 2 layers. I would use strip lines.

1. with microstrip you'll get an impedance error between 10% and 20%  from the expected value due to the fabrication process in PCB. while when you use stripline the error is usually around 5%
2. don't forget that during the EMC testing, you may be asked to do the radiated emission up to 6 GHz due to the high-frequency clock you are using. And stripline gives you a better EMC shield.


I had a quick look at your layout below and my suggestion is to increase the spacing between the GND copper and any controlled impedance traces.
For example, if you see your PCB, the first 2 differential tracks (from the top) you have one track near a large GND copper. You need to expect on that track to have a lower impedance of the nearby tracks.

also, don't forget that GND planes(or land) on different layers tends to oscillate if you don't have enough vias ( set the vias pitch at labda 4), in your case, at least one vias each 2.54 cm

Good luck,

[wraper]

2 layers won't fly. It will become a radio transmitter killing bluetooth, wifi and wireless mouses in close proximity. Not to say in will cause problems to signal integrity.

[Jackster]

Still searching for someone to re-design this PCB for me.

[rahandford]

May be able to help. 2 layer at your risk. rupert_handford@mr3design.net

[timgiles]

Set the gap between trace and ground to 5x trace width at least

The diff pairs should be length matched - but that is each pair not all pairs. Looks like you are trying to match all traces length.

4 layers. 2 will always have issues when you are low on routing area

Try to put the meanders after the traces have become mismatched in length. They are there to bring the transmissions back in sync.

Good luck

[thm_w]

Set the gap between trace and ground to 5x trace width at least

2x should be enough: https://leleivre.com/notes_microstripspacing.html

[pinkman]

+1 to everyone telling you to stay away from 2 layer.  Even with an optimal layout for USB C, signal reflections will be evident on the USB2 pair due to the host side data traces being routed to both sides of the connector. You will severely compound this without controlled impedance even on the short traces you show.  USB3 can be more forgiving but you will always have the USB2 pair there for backwards compatibility, initial attach/connect, etc...

Also... What are you trying to accomplish here?  Are you aware of the rules to achieve certification, and to make your design actually work with a wide range of type C devices on the market?  For instance, on the receptacle side, you will need to route your USB2 pair to both sides of the USBC connector; What you are showing in this picture is more or less a USB-C "extension" cable (in form of PCB) which is illegal per spec.  Look at 3.1.2 "Compliant Cable Assemblies".  You won't be able to receive any certfication with this and will certainly have significant compatibility issues unless you put a type C port controller + power switch on the receptacle side and properly terminate CC1 or CC2 (whichever is appropriate) on the plug side.