Using USB-C connector on PCB?

[grandaspanna]

I've just done my first PCB with a USB-C connector and have a question...

USB-C cables should be able to be plugged in either orientation. On my board, power works with both, but data only works in one orientation. I'm using a Molex 105450-0101 which breaks out each side of the connector as a row, so D- and D+ appear in both rows of pins mated to the PCB. Now, this is probably the source of my problem, I've only used one pair.

The question relates to convention and practice here - should the USB cable connect both sides? It looks like it doesn't - are cables different? Should I always connect both sides of the PCB socket, or maybe there are different USB-C sockets out there that join them internally?

Note that I don't really need USB-C features (power or fast data), but the reversible plug-in is a convenience. I've used mini and micro USB connectors before, but thought I'd dip my toe :-)

The board implements an RP2040 so it it's pretty close to a Raspberry Pi Pico, but I've added some additional I/O and LED bling.
" alt="" class="bbc_img" />

[SiliconWizard]

You should definitely route both pairs on PCB to have a fully compliant USB-C connection. I've never seen any USB-C connector with both pairs already internally connected together. But there are various USB-C connectors out there with a different footprint, and some are easier to route (when you don't need USB SuperSpeed) than others.

As it happens, I've seen some USB-C cables that had both pairs connected internally, and some not. No guarantee. And no mention of this on the cable either. SO don't count on that.

[grandaspanna]

Thanks. I'll update the board.

[oPossum]

Both sets of data and power pins should be connected.

This is how I usually route it....

[grandaspanna]

That's cool - what connector is that? The Molex I'm using features two rows of 0.5mm pins.

[oPossum]

That is the common 12/16 pin connector made by several manufactures. I have been using the low cost generic ones purchased on aliexpress.

It looks like you don't have any 5k1 resistors on the CC lines. That may be a problem when using a USB C to USB C cable.

[grandaspanna]

You're right, I don't have the CC resistors - I'll add those too. It was a quick retrofit to a design for a micro USB socket.

The connector I have is a 24-pin one and the main reason I grabbed it was because it was in stock locally. Now that I've got a bit more time, I might move to one with an easier footprint.

[oPossum]

Molex 217179-0001 has the same footprint.

https://www.molex.com/pdm_docs/sd/2171790001_sd.pdf

There are many others.

[grandaspanna]

Thanks - it's now dawning on me that there's quite a range out there. The 24-pin ones seem to be a bit more expensive and not necessarily useful to me, but I was impatient :-)

[grandaspanna]

Actually, one more question: what are the issues/consequences of connecting the shell to ground?

[ajb]

Yes, there are a number of different connector options that bring out different sets of pins.  Some only bring out power and CC (for devices that only need to charge), some bring out power, CC, and D+/D- for USB2.0 devices, others bring out all 24 pins for full functionality.  Unless you're building a USB3.x device, you don't need all 24 pins and selecting a connector that only brings out what you need will make things much easier to route and assemble. 

As far as the shield/shell, in general you should solidly connect it to your device's ground unless you have a specific reason not to.  Some devices need additional care, but something like that board which just has one USB connection and then what looks like some GPIO should be fine with a solid connection.  There are numerous threads here on the subject, pay particular attention to any of the replies where user T3sl4co1l has provided a wall of text, those are typically very helpful and insightful.  Even if you have a specific reason to NOT do a direct connection to the circuit ground, generally you still want a mechanically solid connection to the board, so designing in some previsions for that are especially important on SMT connectors.  SMT mechanical pads with no additional anchoring to the board will rip off very easily, so expanding the pad with a bit of a fill around it and putting some vias in/directly around the pad will help strengthen it.