I've some schematics with, for example, a power wire with name VCC. I need to change this name to USB_VCC on all wires which have by name VCC. Since I've a lot of wires with names to change, there is a function in EAGLE that allow me do somethig like: "Change all wire VCC to USB_VCC"? It'll save me much time and ensure to change all wires and to not do errors in rename.


1 Answer 1


You rename nets like anything else, using the Name tool. If you click on any section of a multi-section net, you get a slightly different window to if it is a single section:

Name window

Notice how there is a pair of radio buttons. If you want to rename just one section/segment, select this Segment, otherwise to rename the entire net, select every Segment of this Sheet. If the net spans multiple sheets, that second option will instead read all Segments on all Sheets.

This is fine for nets which you have named, i.e. ones that don't have a sup type pin on it, such as the GND symbols, VCC, V+ etc. symbols.

In the case which you net is named using a symbol from the supply1 or supply2 libraries, you should not use the name tool on this net. Why? because when you copy the supply symbol and place it on a new net segment, that segment will take the original name rather than the new one.

So how do you get USB_VCC?

Well, the simplest answer is to open the supply1 or supply2 (or any other) library and create a new supply symbol. In the library, draw out your symbol (or copy and paste from an existing one). The image below shows two key settings for the pin in that symbol - these settings govern the name of the net when the supply pin is connected.

Library Settings

Then create a device in the library with the name of your symbol (e.g. USB_VCC), and use your new supply symbol. You don't need a package, just the symbol.

You can then save the library and insert your new supply symbol.

You will have to replace the existing symbol on all segments of the net - e.g. using the replace tool.

If you already have the board routed, you may want to close the board file, replace all segments with the new symbol (to prevent wires being disconnected in the board), then save. Open the board back up - there will be forward/backward annotation errors now. Simply rename the net in the board file (it will rename the whole net), and this should bring the boards correctly back in sync. If they don't come back into sync, it actually nicely tells you that you missed a segment of the net when you were replacing symbols, and you can tell from the error which segment you missed (if any) and can then go correct it.


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.