If this is a dual gang pot i.e. both pots are in the same mechanical housing - even if they are operated by separate, concentric shafts - and both pots have the same taper (i.e. both are linear or log pots) then if you want to split them across the schematic then you'll have to create your own symbol showing the two part separated by some (fixed by your own symbol) distance but still showing the two pots linked by the single shaft. If you just use two separate pots you'll end up with two components in th BoM. Please see: [https://easyeda\.com/andyfierman/Welcome\_to\_EasyEDA\-31e1288f882e49e582699b8eb7fe9b1f](https://easyeda.com/andyfierman/Welcome_to_EasyEDA-31e1288f882e49e582699b8eb7fe9b1f)

There is a way to do it. Create a new Schematic Symbol but just write on the Schematic Lib sheet that "This is the top level of a two part component". Set the component prefix attribute in the right hand panel to R? or VR? Save that sheet with the pot manufacturer's part number of the pot. Add a Description and links to the manufacturer's device page and to the manufactuter's datasheet. Add some tags (up to 5 are allowed) such as `pot; dual; gang; stereo` If you can't find a manufacturer page and datasheet then please source the part from a reputable supplier with good quality fully dimensioned datasheet(s) and quote their part number and datasheets. Go back to Shift+F search and search for you new part. Select it, right-click > Add Sub Part then draw one pot with the pin numbers as 1, 2, 3 (or whatever they are for the first gang in the manufacture's datasheet). Save it. Repeat the right-click > Add Sub Part on the top level part. Redraw or copy and paste your first pot symbol into this second sheet but number the pins 4, 5, and 6 (or whatever they are for the second gang in the manufacture's datasheet). Save it. You should end up with two pots each a subparts which you can place anywhere. If you have only one instanc of the dual pot in your schematic and you gave the top level the prefix of VR then one will be VR1.1 and the othe VR1.2 on the schematic.

There are some already in the library:  Just search for and assign a suitable PCB Footprint in the Footprint manager that opens when you click on the Package attribute of the Schematic Symbol when you place it into your schematic.

Many thanks Andy

You can create private library or go to library, pcb libs, user contribute, search. Good luck 

Great thanks.