I designed my own PCB and received it, but none of my pcb's can be found in the ports list or with the Ft_prog tool from ftdichip.com. Here is my schematic:
I saw that I had to connect pin 4 to pin 17, so I did but I don't have 3.3V coming out, I have 5V coming out of pin 17 and pin 4. I still can't detect the chip on my computer or with the Ft-Prog software. Does anyone have any ideas?
To answer to @Justme this is how i connect my usb 
As discussed in the comments, pins 7, 18, 21, 25 and 26 are drawn on your schematic as connected to the GND net, but they are clearly not connected to anything in the layout screenshot. Don't forget to run DRC before you finish the design! Perhaps you disabled the ratnest for this net and forgot, or it's possible the wires aren't correctly attached to the pin in the schematic (it looks fine though).
In addition to this... You are using a USB-C connector, and have not connected the CC1 / CC2 pins. If you are using a USB-C to USB-C cable, then no power will be provided. However, a USB-A (host-end) to USB-C cable (device-end), will likely give you 5v. To check this, measure the voltage between your GND net and TP2
In the future, it's important that you understand the role of the CC1 & CC2 pins - they help identify connector orientation, and are also used to negotiate power, among other things.
Many basic devices simply use a 5.1kΩ pull-down on each CC pin, which should negotiate / request a 1.5A limit (i.e: one 5.1kΩ pull-down on CC1, and second 5.1kΩ pull-down on CC2). This is a fairly high limit for a simple widget, so you might be interested to read up on the details of this further.
The chip should come up with default settings. You don’t need to use FT-Prog just to detect it. When you connect to the computer, the new device chime will sound. Just like if you plugged in a USB drive.
I have 5V coming out of pin 17 and pin 4
You have connected the VCCIO line to 5V on the schematic and on the PCB. That line should not be connected to anything else but the capacitor. The VCCIO net should have exactly 3 pads on it: pin 4, pint 17, capacitor. There is no 5V “coming out” - you are driving it with 5V.
Once 5V is driven into pin 17, the chip will be damaged and will not enumerate.
Remove the chip from the PCB, and make sure that when it is removed, the VCCIO net has only 3 pads connected and nothing else. Modify the PCB. Then reinstall a new chip.
There are many reasons why it does not work.
Due to the Type-C port implementation, the board does not even signal to the host computer Type-C port that anything is connected, so the host never turns on the 5V power supply to your board.
This is a common error in many devices and examples how to replace a device-end receptacle such as Type-B or MicroUSB. You can't simply directly replace those with a Type-C connector without further design of the Type-C interface properly.
Your device only powers up if you use an adapter cable which is allowed to provide 5V on a Type-C plug without negotiation.
Also the FTDI power supply connections do not match either bus-powered or self-powered configuration, but something invalid which leaves half of the chip unpowered and half of the chip powered when you disconnect USB where VBUS turns off or when you turn off the 5V supply.
And that PCB design reportedly omits ground connections, but it is unclear if the ground plane is really there but software just did not fill in the ground plane so it just looks like ground connections are omitted.
