2
\$\begingroup\$

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?

\$\endgroup\$
7
  • \$\begingroup\$ Is it just for schematic purposes or for board layout? You could use some headers as place holders in a schematic. Just label each pin. \$\endgroup\$
    – Passerby
    Aug 2, 2015 at 7:07
  • \$\begingroup\$ Do exactly what you'd do with any other part that isn't in the library: create the footprint yourself. \$\endgroup\$ Aug 2, 2015 at 8:59
  • \$\begingroup\$ The footprint is already done by Digispark, I wanted to reuse it as I have the actual controllers (unless I didn't quite get your point). Also @Passerby, it is for board layout as well. \$\endgroup\$
    – Heinzen
    Aug 2, 2015 at 19:50
  • \$\begingroup\$ So your essentially asking how to lock a set of items into a group. \$\endgroup\$
    – Passerby
    Aug 3, 2015 at 1:05
  • \$\begingroup\$ The problem is that I have the footprints and the schematics for the DigiSpark done and released by them. I need to use them in a different schematic/board with my own project, but if I export the DigiSpark as a library and use it in my own, I get a group of components rather than the actual board. On the schematic side it is expected to be like that, but if I switch to the board, the original footprints are not persistent, it gets messy and doesn't look like the original board at all. \$\endgroup\$
    – Heinzen
    Aug 3, 2015 at 18:12

1 Answer 1

1
\$\begingroup\$

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.

\$\endgroup\$

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.