Modify Arduino micro library

[Thiird]

Hello,

new user of Eagle here.

Im designing a small keypad with an Arduino micro, in doing so I needed the arduino micro footprint which I found on Element14.com, the problem is that when I go to the board, given that the arduino is a component itself, instead of just having the holes for the pins on the main board I get the whole section cut out, see image.

What I would like to do is create a version of the same library that only includes the 2x17 rows of pins.

I tried to copy the library and modify it myself but being a new user I cant understand how to delete everything from all the layers except the two rows of pins.

Can you guide me through the procedure of creating such custom library?

Thanks

[one-of-the-robs]

The problem here, and it's unfortunately a very common one, is that the author of the library did not understand the difference between a board being designed and a module being included in a project.

You don't need (or probably want) to "delete everything". The simple fix is to open (a copy of) the library, go to the relevant footprint, and CHANGE LAYER everything that's on layer 20 "Dimension" to be 51 "tDocu". You can make that easy by:

- In the layers selection hide all except layer 20

- Use the group tool and pick everything (drag over the full window)

- Use the change->layer tool, pick 51, and ctrl-right-click anywhere on the editor

- reset the displayed layers to something more useful

[Thiird]

Thank you so much for the quick reply.

I understand the procedure but I cant do it: when I open an instance of the library I get another box along with it in the board, and if I delete it I cant properly select the arduino alone, what am I doing wrong? Selection settings?

Even if I manage to select only the Dimension layer the arduino wont be transferred (end of video).

Please refer to the video.

Video (2 min): https://www.youtube.com/watch?v=24pzErFvsUY&feature=youtu.be

Thanks.

[one-of-the-robs]

That's because you ignored my first instruction, namely

---

The simple fix is to open (a copy of) the library

---

Your video clearly shows you trying to make the changes in the board editor. The problem is that the library is broken so you need to fix the library by editing the footprint in the library. Once that's done you can update your existing board by doing an "update library" to fetch the corrected version.

[Thiird]

Oh I understand.

Im surry, but how do I modify the library? So far I've been using libraries to add components to my projects.

[one-of-the-robs]

---

@Thiird wrote:

Oh I understand.

Im surry, but how do I modify the library? So far I've been using libraries to add components to my projects.

---

If you navigate to the library in the control panel's left pane you can double click on it. Alternatively you can use "File->Open->Library" and navigate to it. That opens the library editor, a set of lists of content, from which you can double-click on the relevant footprint (since that's what you're wanting to edit).

The footprint editor looks and behaves quite a lot like the board editor but with obvious differences because you're editing one footprint with no defined nets, rather than lots of nets connecting lots of footprints.

[Thiird]

Ok I found it and moved the edges of the board to layer 51, but I cant select the four little circles.

Somehow they are part of Dimension but I cant select and move them.

Video: https://www.youtube.com/watch?v=wmCY-doJwFc&feature=youtu.be

Also I need to delete the 6 pins in the middle of the board, I tried deleting them from the board view but it says "Cant delete pin, connected to X", so I thought I first had to delete the pins from the schematic but it says the same thing.

How do I delete connected components?

Thanks.

[one-of-the-robs]

---

@Thiird wrote:

Ok I found it and moved the edges of the board to layer 51, but I cant select the four little circles.

Somehow they are part of Dimension but I cant select and move them.

---

OK, that's because the footprint has "holes" there. A hole is a non-PTH hole for mounting purposes. You may want them, in fact, so that your board has correctly aligned mounting holes to fix the module down onto. If you do want to remove them, get the "holes" layer up and you should be able to delete them at their centres.

---

@Thiird wrote:

Also I need to delete the 6 pins in the middle of the board, I tried deleting them from the board view but it says "Cant delete pin, connected to X", so I thought I first had to delete the pins from the schematic but it says the same thing.

How do I delete connected components?

---

That's because the library "device" associates the footprint with a "symbol" and connects schematic symbol pins to footprint pads. You can't remove either the pins or the pads while that connection exists.

I would suggest at this point that you probably want to make copies of both the symbol and the footprint, as what you're creating is a slightly-reduced version of the module and should therefore be a different device. Unless, of course, those six middle pads are guaranteed always irrelevant, pre-populated on the top side and only for in-circuit programming, or such like.

If you make copies, you can edit the new symbol and the new footprint to remove the pins, then create a new device using them and only connect what's there.

If you don't make copies, you need to edit the device first, break the connections involving those pins/pads, then you should be able to edit the symbol and footprint. You still need to do the symbol first, so that the device doesn't go through an invalid state of having too few pads for the pins that need to be allocated.

It's well worth having a good thorough read of the manual (installed as a PDF when you installed Eagle) section on library structure. Things make a lot more sense when you understand how the library works!

[Thiird]

I read a bit of the docs and after some effort I learned how to modify the library to came up with what I needed!!

Thank you so much for your time and patience.

Have a nice day.