Electronic – How to add the board of a pre-existing controller to the project

cadeaglelibrary

I have a DigiSpark board that has the schematics and board files released in their website. I am making a PCB where I need to have that part in my circuit.

Right now I have tried editing the DigiSpark's schematic and add the components I need and work on the board but that doesn't work properly.

Tried exporting the DigiSpark board as a library but it adds every component (as in: resistor, capacitor…) rather than the actual board to the files.

Is there any practical way of making my own project and when I am done with it, import the schematics and wire things up and then work on the board while keeping the original DigiSpark board design?

Best Answer

As you have both the Schematic and Board files for the existing design, then it is indeed possible to import it into a new design. There are two options.

Option 1

Rename the existing files and start working from there. This is useful if you are just starting out, but not if you are already a long way into a design.

Option 2

If you have an existing design you want to import a second existing design into, then these steps will allow an existing schematic and layout to be imported in.

  1. Open the design you want to insert into (not the DigiSpark one, your design). Make sure both the schematic and layout are open.

  2. In the schematic editor, go to File->Import->Eagle Drawing...

  3. In the window that opens, select the DigiSpark schematic file. Make sure that the DigiSpark board design is in the same folder and has the same name as the schematic else this won't work.

  4. Another window appears which gives you a list of nets in the design you are trying to import. It will tell you the name of the net in the design (old name) and give you an option to change the name in the new design (new name). If there are no conflicts then by default the new name and old name will be the same (though you can change them if you want). If there are any conflicts, i.e. nets in both designs that have the same name, it will do one of two things, either (a) give them a different default name, or (b) give them the same name and show a little yellow [+] symbol at the end of the line indicating they will connect. You should verify the net names to make sure only things you want to connect (e.g. ground) have the [+].

  5. Click ok.

You should find that the schematic is imported into your existing one, and if you look in the layout you should also find that the fully routed layout has been imported into your design as well.

I should note that I have a non-free license of Eagle which allows multiple sheets. When I do the import the imported schematic appears as a new sheet. For the freeware versions multiple sheets is not included in the license, so I am not entirely sure where it will be imported. It is entirely possible you will get another sheet regardless, or it may import into the existing sheet, or not at all. You'll have to test it.

Related Topic