topic Re: Routing "Superspeed" differential pairs in EAGLE Forum

Routing "Superspeed" differential pairs

Anonymous — Wed, 08 Jan 2020 22:41:29 GMT

I'm designing a product that includes a USB3 hub. Routing the "superspeed" signals is a difficult task in any case, but in addition to my own lack of experience & skill in this area, I'm wondering whether Eagle is really capable of this task. The pairs must be tightly length matched not just end-to-end, but at every point along the path. My experimentation with differential pair routing in Eagle suggests that it does not do such tight matching automatically, and it seems like an impossible task to do it manually.

Also, for the traces to escape from the hub IC they need to neck down to a smaller trace width to fit between pads. Is that possible? If so, how do you do it?

Re: Routing "Superspeed" differential pairs

jorge_garcia — Thu, 09 Jan 2020 18:12:20 GMT

Hello @Anonymous,

I hope you're having a great day. Thanks for visiting our forums! I'll try to answer your questions in order.

First, EAGLE can handle the tighter matching there's just a little bit of setup you need to do. Go to the DRC > Misc Tab. Set the max length difference to whatever is required by the USB3 spec. The default 10mm is not going to cut it. Additionally set the gap factor to 1, that way you'll be able to make tighter coils for length matching.

Second it is possible to neck down traces, just type the width in the Command line and press enter. You can do this at any point in time while routing the trace so it's very easy to drop down the width and then bring it back up.

Just a recommendation, because of how critical this component is you should probably route it first. You want to keep the traces as short, direct and symmetrical as possible. Once this is routed then you can move on to other components.

Let me know if there's anything else I can do for you.

Best Regards,

Re: Routing "Superspeed" differential pairs

Anonymous — Fri, 10 Jan 2020 04:01:31 GMT

Hello Jorge,

Thanks for this information. I'd like to know more about the "max length difference" parameter, but I think I have to start with a more basic problem: I think the pads on the IC are spaced closer than the spacing required to route the differential pair. I have observed in the past that when pads are farther apart than the required spacing they simply come together as quickly as possible, but in this case it seems like the router will not allow me to even start routing off these pads. It displays a yelloe semi-circle in whichever direction I try to pull it. How do I get around that?

Greg

Re: Routing "Superspeed" differential pairs

jorge_garcia — Fri, 10 Jan 2020 20:33:46 GMT

Hi @Anonymous,

I hope you're doing well. The yellow circle indicates that it can't move because DRC violations would be incurred. So the first thing you need to do is setup your DRC to match the requirements of your board manufacturer to make sure your board will be manufacturable. If you are just using the default DRC then it's not surprise that the routing is too tight.

Once you have the DRC setup properly if you continue to get the yellow circle then that would likely indicate that current manufacturing process you've chosen isn't suitable for the tight traces you need.

Let me know if there's anything else I can do for you.

Best Regards,

Re: Routing "Superspeed" differential pairs

engineeringNCMXB — Sat, 11 Jan 2020 20:06:47 GMT

@Anonymous On the best of days....differential routing with impedance control is a very thick topic. Eagle only helps you implement your own understanding of the topic. The geometry of the traces, ground planes, and the entire stackup will all contribute to the success or lack thereof. There are a lot of ways to control impedance of a differential pair along its entire route but there are a lot more ways you can disrupt the impedance. USB3 is no joke if you are hoping for reliability. Just measuring your success is a considerable challenge requiring a high-speed TDR or network analyzer along with skills to get useful data from them.
If you have never dealt with high-speed digital routing before, I would suggest that 90% of your efforts should be outside of learning how Eagle deals with differential routing which is the easiest part of designing a successful high-speed PCB.

Re: Routing "Superspeed" differential pairs

Anonymous — Sat, 11 Jan 2020 21:40:49 GMT

Carlos, thanks for the reply. I've dealt with high speed differential pairs before, but only as a design engineer reviewing the work of a layout designer, not doing it myself. So perhaps unlike many people on this forum, I have a pretty good understanding of the physics, but am a total newbie when it comes to using to using layout CAD tools.

Re: Routing "Superspeed" differential pairs

engineeringNCMXB — Sun, 12 Jan 2020 00:28:16 GMT

You are 100 steps ahead of most. 🙂

As for routing diff pairs in Eagle, there is modest support. You name the pair according to convention and route them together. Eagle will maintain the specified distance between the two. There is support for length matching, but I have found it to be difficult in tight routes. The biggest limitation I have seen is the when trying to adjust an existing differential route as the layout comes together. Especially when the diff routing uses curves instead of 45 deg turns.
As with many things in Eagle, it is possible but rarely easy.

With that said, I have had success with numerous high-speed designs. Most of the delicate work was manual and tedious compared to how Altium works but there is a $10k price difference so a little extra work is not too bad. I would like to see differential pairs improve the options of easier route adjustments as a pair. The concept of routing the high-speed stuff first and never changing it as the layout progresses is just no realistic. At some point....everything moves and routes need to follow along.