Mapping error when replacing part on schematic

[Anonymous]

In the schematic I right click on  an LED and select REPLACE,  then select the new LED in the Library.

I get the error:  "Gate A in the old version of device set LED_VLM41 can't be mapped to any gate in the new version of this device set (neither by name nor by coordinates)."

Both LEDs have two pins.  Each LED device has its own symbol.

Looking at Properties of both Symbols the pin names are both A and C for the two symbols

Someone suggested I need to open the BRD and SCH XML files in Notepad do a search for the pin names edit the files and make the names match.  Is this really what I have to do to replace a component?

I don't see anywhere where the pin names are different.

Any help would be appreciated.

[one-of-the-robs]

You may get better answers if you can upload the offending library.

I think you posted this question before, with some screen-shots? The only thing I noticed in them was that the schematic symbol pins were not on a 0.1" grid. I don't know whether that's relevant to your replace problem but you need to ensure all schematic symbols have all their pins on that grid. The schematic editor doesn't like it if you place them off-grid.

[Anonymous]

Yes, I moved it because I thought it would not be viewed since I added to a solved question.

I shifted the symbols so the pins are on the grid.  Still get the error.

Old Symbol

New Symbol 

[Anonymous]

I attached the two LED libraries I am trying to swap.

[one-of-the-robs]

I've had a bit of a play. One of your devices has the LED symbol named as "G$1" while the other names it as "A". If you use the same name for both devices, the replace will work. If the names are not the same, I think the gates have to be at the same coordinates in the device, as well as the pins being at the same coordinates in the symbol. It may seem odd when both devices have only one gate but it does seem to be the case.

[Anonymous]

That sounds right!  Where do I find the Symbol Name?  I just see the name in the "Table of Contents"

[one-of-the-robs]

If you open the device in the editor, you will see the symbol on the page. Select the NAME tool and click on the symbol's origin point. You'll get a pop-up with the current name in it and you can type the new one.

Note that this is the name by which that "gate" (instance of a symbol) is known within that "device". It's independent of the symbol's name in the library. The tutorial on creating a 7400 quad-NAND device shows how these various names relate to each other.

[Anonymous]

That is what i suspected, but I cannot get the pop up window.   Click the Name button, then click the Symbols Origin... nothing. Left Click, right click...nothing.

Device Window

Symbol Window

[one-of-the-robs · Accepted solution]

I think you may be getting caught out by your origins. If you look at the two screen-shots you posted, the "origin" mark on the symbol editor is where the anode wire joins the triangle. Your annotations on the device editor suggest you're clicking on the little cross in the middle of the triangle. That's the origin of the device (the editor's origin) and not the origin of the symbol. Try clicking where the wire joins, i.e the position that you've marked in the symbol window, but in the device editor. I found that when testing your libraries earlier.

[Anonymous · Accepted solution]

That worked!  Thank you so much?  I feel silly, but I don't think I would have figured that out.  Eagle library has some obscure tricks.