How to route this USB-C connector

[Jonathon_Doran]

I have this USB-C connector which I wish to use in a project.  I had a great deal of trouble finding a part and a footprint, but finally found this on JLCPCB (# C668624).

I have attached a close-up of the footprint below, as I started to route.  But then I see the differential signals are staggered.  I like puzzles as much as the next person, but this has me stumped.

As a differential pair, I want to keep the trace lengths the same.  But I believe I have to connect the B6/A6 and B7/A7 pads together.  One attempt is shown below (USB-1).  This is going to leave my lines a different length unless I do something funny.

So I figured I would just ask the community for advice.  Am I going about this entirely wrong?

I hope that I don't ask too many questions here, but this is my second board that I'm laying out and I'm still very much a beginner at this.

Edit:  I meant to also ask about another issue with this connector.  The minute I try to draw a trace from VBUS I get an error that it violates DRC.  The footprint has merged some pins (A12/B1 ground), (A9,B4 VBUS) and these are highlighted when it refuses to draw the trace.  What I am supposed to do here?

[Jonathon_Doran]

I believe I have solved the second issue.  The footprint that I obtained had drawn the pad as a polygon and not a pad.

I remade the symbol and the footprint so that there was a "A1/B12" pin and pad, and the same with "A9/B4" "A4/B9" and "A12/B1".  I also made the appropriate power flags on the symbol.  This passes ERC, and I can route out of the big pads now.

I still have the issue with how to route those D+/D- lines.  I might even have to drop them to the bottom layer using vias...

[ataradov]

For USB HS those things don't matter at all. Don't worry about length matching to a mm. What you did is what 100% of designs using this connector do and it works fine. And this is the most common and generic connector out there.

And for USB FS/LS it so does not matter that it is hard to describe. You can use coat hangers for wires and USB FS will work fine.

[SiliconWizard]

For USB HS those things don't matter at all. Don't worry about length matching to a mm. What you did is what 100% of designs using this connector do and it works fine. And this is the most common and generic connector out there.

And for USB FS/LS it so does not matter that it is hard to describe. You can use coat hangers for wires and USB FS will work fine.

Yep, this is exactly how I route those connectors and yes for USB FS and HS, this is absolutely fine.

[Jonathon_Doran]

Thanks to both of you.  How do I get the trace out of that mess?  Are you saying yes to the idea of using a via and dropping it to the bottom?  Or were you just commenting on the connecting of the pairs on the top (as shown in the screen capture)?

Based on the comment about being able to use coat hangers, I'm going with "use the vias".

This leaves me a little sad as I see folks routing those pairs out of USB-3.1 connectors with no trouble.

[ataradov]

What do you mean? You have both D+ and D- exposed on one side. And they connect in that pattern under the connector.

USB3.1 Type-C connectors have the same exact issue for the USB2.0 pins. USB3.0 pins are muxed using special ICs, since routing like that will not fly there.  Type-A connectors don't have this problem, since there are no orientation options. 

Attached picture.

[Jonathon_Doran]

Thanks for the picture, I'll think about this some more.

I boxed myself in with the VBUS lines.  You dropped them with vias.  I have plenty of space on the back copper for a VBUS pour, so I'll give that a shot.

This is a four layer board with Signal-GND-GND-Signal.  I debated using Signal-GND-Power-Signal, but wanted a good reference for any signals on the bottom.  I could use large pours for VBUS and 3.3V on the bottom though.

Sorry for all of the questions.  As I said, this is all new to me.  I'll make my mistakes, but I would prefer to mess up on paper.

[ataradov]

This design works fine on 2 layers. If you need signal integrity for something else on the board - prioritize that. USB HS does not care.

For VBUS you can route it on the back on the same layer and then do whatever you want with it. On smaller designs I put voltage regulator on the other side of the connector.

[SiliconWizard]

Yes you need zero via for D+/D-. For CCx and VBUS, you may, depending on your board. But that's absolutely not a problem. Just use the right size of via for VBUS depending on the max current you're going to draw.

[Jonathon_Doran]

Thanks for the advice on the via size.  My 0.7mm/0.3mm vias should be able to handle 1.5A (using the Saturn solver here).  The board can pull 170mA.

[bson]

This is a four layer board with Signal-GND-GND-Signal.  I debated using Signal-GND-Power-Signal, but wanted a good reference for any signals on the bottom.  I could use large pours for VBUS and 3.3V on the bottom though.

Any power plane will work just as well as a GND plane for a signal reference.  The key is the low impedance of the plane.  +5V, +3.3V, or 0V doesn't matter...

[Jonathon_Doran]

Thanks.

I hope that someone would be so kind as to take a moment and look over the entire design:

https://www.eevblog.com/forum/projects/request-review-of-project/

I'm afraid it has gotten buried.  I am almost to the point of giving up and just sending it off to be fabricated anyways.  This is my first board, and I'm really nervous about screwing things up to the point where the board cannot be saved.  I would prefer to put more work in up front rather than at the bench.

One change that I have planned that is not reflected on the design linked above is that I plan to extend the copper pours on the third layer to cover most of the board.

If I only had more experience with RGB LEDS I might be able to figure out how to get some on that key matrix within the power budget.  I really don't know how bright they are, or can be.

[ataradov]

This is my first board, and I'm really nervous about screwing things up

In that case it is a good idea to make a small board first with just the MCU and a few buttons. This way it will fit into the promotional tier of any cheap manufacturer. This way you will also figure out all the manufacturing issues and issues with your footprints.

I have a ton of experience, and I probably would not send a board like this for manufacturing without prototyping.

If I only had more experience with RGB LEDS I might be able to figure out how to get some on that key matrix within the power budget.  I really don't know how bright they are, or can be.

And this is why you prototype first.

[Jonathon_Doran]

In that case it is a good idea to make a small board first with just the MCU and a few buttons. This way it will fit into the promotional tier of any cheap manufacturer. This way you will also figure out all the manufacturing issues and issues with your footprints.

I have a ton of experience, and I probably would not send a board like this for manufacturing without prototyping.

Fair enough point, and one that I thought about.  But the high risk part of this would be needed on any prototype (at least I believe it would be).  The MCU would need power (from USB), and a crystal, and a regulator.  At this point, about 90% of everything is there.  I don't worry about the switches.

But I'll think this over for a bit.

[ataradov]

The point is that full size keyboard PCB would cost a lot compared to a $5 100x100 mm prototype. There is always a risk that it would not work, but small PCB is way cheaper for multiple iterations.

Plus you are worried about LEDs. Place however many LEDs you need on that test PCB and see how they behave. You can even add a connector for an external keyboard matrix.

[SiliconWizard]

The point is that full size keyboard PCB would cost a lot compared to a $5 100x100 mm prototype. There is always a risk that it would not work, but small PCB is way cheaper for multiple iterations.

Plus you are worried about LEDs. Place however many LEDs you need on that test PCB and see how they behave. You can even add a connector for an external keyboard matrix.

Yep. On a more general level, this raises an "interesting" point, as selecting either approach is something that also happens in a professional setting.

While many engineers are more in favor of intermediate prototyping first, as ataradov suggests, some do like the idea of designing the whole thing right off the bat, with the idea that if by any chance, everything works as expected, you'll have saved an iteration, and time. The second approach is also more likely to be seen among managers than among engineers themselves.

In particular, I've seen this latter approach promoted by "six-sigma" guys.

[ataradov]

Most involved projects I've seen would do a non-form factor version first anyway. This lets you break out the debugging pins and not worry about fitting into the final envelope. Plus you may not even know the final mechanical design at this point and it would be informed by the electronics after the firmware is (mostly) done. And the sooner you can get any boards, the sooner firmware people can start their work. After that hardware people have all the time in the world to massage their design into the final shape.

Of course in this specific case the firmware is likely going to be based on the existing keyboard firmware generators, so the development is not too involved. And there is also a ton of space anyway to break out whatever you need.

[Jonathon_Doran]

My keyboard is not a "full" keyboard.  It is a 6x6 grid which is about 120x130mm, so not that much bigger than that $5 special.

[ataradov]

Then just order it. JlcPcb shows $10 for 120x130 mm two layer PCB. It is not really worth it thinking twice about it at that price. Just order them and if there are issues - treat them as very specific prototyping boards. If issues are fixable, fix them by hand on the prototypes. If not - order a new set.

JlcPcb prices seem really sketchy at this point. No matter how optimized your process is, they are not that cheap to make. But I guess take advantage of this while it lasts.