The problem is that you are using a schematic symbol contributed by one user (iJackBauer) and a PCB package contributed by another (memphis) and the two have used different pin numbering. There are two problems. 1\. the two contributors have used different pin numbering\. You have to make the pin numbering on the schematic symbol match the physical pin numbering on the PCB package\. 2\. memphis has mistakenly assigned net names to the pins on the package\. This \(a\) forces pins to be connected even if you put "no Connect" symbols on them and \(b\) if the netnames assigned to the pins are different from the netnames on the connections to them then they do not connect to the external nets\. The simplest and most reliable way to fix this is to clone memphis's package and save it with a unique name. Then SHIFT+F search for it again, select and **right-click > Modify** and then add a Description including links to the manufacturer's device page and to datasheet(s) showing pinout and PCB footprint. If you cannot find manufacturer's information then please include links to the information from a reputable supplier's pages and include supplier part number. Then open the new package and delete all the netnames (and the spice pin numbers as there is no spice model for this device) applied to each pin. Then renumber the pins to match the schematic symbol. Save it. Now clone the schematic symbol. Save it with the same name as your new package. Search for it and copy and paste the Description from the package into the description for the symbol. Open the symbol for editing. Change the "package" attribute to exactly the same name as that of your new package. Save it. * Please check the schematic symbol and your new part against the datasheets and correct any errors. When you next search for the symbol, it should appear together with your package.