Making your own parts on eaglecad and using I2C

Thread Starter


Joined Feb 10, 2012
Hi Everyone, im doing a project and need some advice if thats ok
Im designing a PCB on eaglecad and need to use a 28pin header. The header with the correct pitch is only 26 pin or 32 pin. How can I redesign the part so that it has a 28 pin header in the library? Is it a difficult and complicated processs?
Secondly, I will be interfacing a beagle board with an LCD so if anyone is able to provide me with some info on how to program that in c and how to use I2C it'd be great

thanks for the help, all the best


Joined Jul 17, 2007
You have two very different requests for your 1st post.

You have not mentioned what version of Cadsoft Eagle that you are using.
You didn't say which library has the headers with the correct pitch, or what the name of the 26-pin header is that has the right pitch. It helps if you post these things.

It's not too hard to copy an existing part, and make a few changes to wind up with a new part. You usually don't want to simply change the original part, unless it was in error.

You start by going to the Eagle control panel, and opening up the library that you'd like to edit. Find the device that is close to what you want by clicking the Device icon (looks like four AND gates, right below Draw on the top menu bar)

On the left side, you'll see the device more or less as it appears on the schematic. On the right up top, you'll see the package that's used on the PCB. Below that, you'll see the package name on the left. Remember that package name.

Then go edit a new package that has a name similar to that package, but with 28 in the name instead of 26. It'll ask you if you want to create a new package; click yes.

Then you can copy the previous package into the current package; this will save you lots of time, as you won't have to re-draw a whole new package, just stretch this one a bit, and add a couple of pins.

The command you'll use looks like:
COPY connector26.pac@libraryname.lbr connector28
of course replacing "connector" with the name of your source connector, and "libraryname" with the library to get it from.

Then you will find that new package in the list when you click the package button, to the right of the device button (it looks like an IC).

Then you edit the package to stretch it out and add the extra two pins. Make certain that you change the grid to some multiple or even fraction of the spacing of your pins.
For example, if your pin spacing is 2.5mm, then you would type:
GRID mm 2.5
- or -
GRID mm 1.25
If you don't adjust your grid before you start moving things, you will have problems getting things to line up.

Make sure that you don't goof up the order of the pins.

After you are done stretching the package and placing the pins, change the grid back to inch and 0.1, as:
- or -
(Just in case you didn't know, in this context, 1 mil = 0.001")
If you don't, you will have problems getting things (wires and pins) to connect in the schematic.

Now depending on how they defined your Symbols, you may or may not need to add a new one. Sometimes, connector libraries like this just have a couple of pin types for symbols, and they are simply copied as many times as necessary for the Device.

You'll need to use the NAME tool to edit the pin numbers in the Device and Symbol (if necessary). In the Device, you might start off by copying your 26-pin device to the 28 pin device just like I did with the package. You may need to disconnnect all of the currently connected pins from the package, and delete the existing package from the menu on the right - then add in your new package, and connect all of the pins up.


Joined Dec 10, 2011
To you all: Instructables .com And U-Tube both have a lot of help with this type of thread.
I use Eagle 5.11 with both to success.