Okay, here's a quick guide on how to create Supply Rail parts in Eagle. Please note that I am by no means an expert in Eagle - I learn as I go along, just like you probably are!
The brief tutorial is applicable to version 5.60 of Eagle on a Windows machine. Other versions may be similar.
I am assuming a basic knowledge of Eagle, otherwise I could be here all day. But if you have specific questions then post to this thread and I'll do my best to answer them - like I said I'm not an expert myself.
Supply Rail parts are useful because they allow you to connect various parts of your circuit to a supply rail symbol, which then automatically merges the nets concerned. This avoids the untidy alternative of physically connecting separated parts of a circuit to the same supply rail with a physical wire. The connection is instead implied by the connection of the supply rail part. This can also be used for ground rails, or in fact anything you want!
1. Okay. To create a Supply Rail Part, first you must open a library. I've previously created my own library called 'Brian Hoskins', and I'd advise you to create your own as well. The only footprints you can trust 100% in Eagle are the ones you've spent your own time perfecting!
2. Once you've opened your library, you need to create a new symbol. To do this, click 'symbol' from the toolbar
3. Then type your new symbol name into the dialogue box. (e.g. V1, V2, V_pos... whatever)
4. Click 'OK', and then you will be presented with the following dialogue box, asking if you're sure you want to create the new symbol. Click 'Yes'
5. Now type the command 'pin' into the command line. Choose your desired pin from the toolbar that appears (short, long, etc) and place it at the origin of your symbol diagram (marked by a cross).
6. Select the 'Change' button from the left hand toolbar (depicted by a spanner) then right-click your pin and select 'Properties' from the menu that appears. You will be presented with the properties dialogue box for your symbol. Change the standard pin name to something more descriptive (in this case best to make it your supply rail name) and change the type of the pin to Sup (short for supply). Then click OK. See below for details:
7. Now you need to draw your symbol. It's up to you what you want it to look like, but I always tend to stick to a "keep it simple, stupid" approach. Hence this is my symbol:
8. Now your Symbol is done. Select 'Device' from the top toolbar:
9. Type in your new Device name, like you did for the Symbol. Again - keep it simple, stupid. Use your supply rail name!
10. Just as with the new symbol creation, you will now be presented with a dialogue box asking if you're sure you want to create the new device. And we are sure, so click 'Yes'.
11. In the Device window that appears, you will see a button labeled 'Prefix'. Click it, and enter your Supply Rail name. Then, in the bottom left sub-window, click the 'Description' link and enter something descriptive for the device like I've done below. Note that you can use tags like <b> </b> etc:
12. Now type add in the command line, or select the add button from the left hand toolbar. This is where you add the symbol you created previously, to your new device. Select the correct symbol (hopefully you've called it something meaningful or this could be tricky!):
13. Now place your symbol in the top left sub-window. You may need to zoom in (tip:hold CTRL and use your scroll button on the mouse). It's best to place it on the origin I think, as it uses this to determine where to hold the symbol when you're placing it on your schematic.
15. That's it! You're done. You don't need a package (footprint) because this is just a supply rail connection on your schematic, not a physical part. If you save your work, you should now be able to add the supply rail you've created to your schematic. If you add multiple copies of your supply rail to your schematic and connect various parts of your circuit to them, then those parts of the circuit will automatically be connected without needing to draw physical connections between them. Much neater if you ask me.
Hope this helps!
Brian