Q regarding symbols

[Jonathon_Doran]

I started a new project, and decided that I want a USB-C receptacle.  There is a part USB_C_Receptacle_USB2.0_16P but it only has 11 pins shown.  How is this going to work when it comes time to route?

The part has the same basename for many pairs of pins.  May I assume they are on the same network and that I will be expected to route both later?

I have not fabricated a board before, so this is a new experience.  I am looking at the parts in stock at JLCPCB and see that the links for symbols/footprints are now EasyEDA links.  I am using KiCad.  So it doesn't look like it would be easy to just download the symbols/footprints for the parts that are in stock.

May I get some assurance/recommendations on how to proceed?

[janoc]

You need to create symbol and footprint for the part you want to use. It is completely normal that the vendor libraries don't contain everything that is available - that's why you have the symbol and footprint editor in KiCAD (and any other PCB editor worth its salt).

[selcuk]

Yes. Shielding pins all have the same name: S1. Schematic software thinks they are all the same. And you need to make sure each one of them are properly connected to a solid ground plane while routing, since schematics doesn't care about ground quality.

I recommend creating your own footprints and symbols to have a better control and high quality designs. Then you can download 3D step files from the Internet and validate with your footprints.

[ataradov]

Specifically 16P is a common name for a standard 12-pin connector. The ground and VBUS pins are tied inside the connector. Look at the pictures of those connectors and you will see the wider pins made out of two separate wires that will end up soldered to the same pad.

They use "16P" in the name because it exposes 16 pins from the USB side.

[Doctorandus_P]

For USB-C it's probably not needed to create your own schematic symbol. KiCad already has several symbols for USB-C connectors (depending on which pins you want to use). Pin numbers and naming on USB-C connectors is also standardized (A1 though A12 and B1 though B12) and this makes it a lot easier to make a "universal" symbol for it.

https://en.wikipedia.org/wiki/USB-C

KiCad uses "pin stacking" in a lot of it's default symbol libraries, as Ataradov already mentioned. You can easily se how that works by loading a schematic symbol in the symbol editor.

And another part of the puzzle was mentioned by Selcuk. If pads on in the footprint have the same padnumber, then KiCad interprets this as all those pads have to be connected together (when connected to a net).

And third.
USB-C is a bit of a complicated standard, and not all pins are always needed. If you want to use the connector for older USB standards, then only GND, Power, and D+ / D- may be enough.

For the footprint. As always with connectors, you have to be very careful here. The "mating part" of connectors is standardized but the footprint on the PCB is not. There can be hundreds of different footprints for the "same" connector. A quick count shows there are already 24 different "USB_C Receptacle" footprints in KiCad's default libraries.

[xvr]

I am looking at the parts in stock at JLCPCB and see that the links for symbols/footprints are now EasyEDA links.

There is Python script to download and install EasyEDA symbols to KiCAD. Just install Python and run pip install easyeda2kicad