Open your copy of Eagle and in the main "Control Panel" window, use the File > Open > Schematic menu to open your copy of the schematic for the Trinket M0. The schematic file ends in .sch and when you open it, Eagle will ask if you want to open the board file as well. Say yes and select the schematic window if it isn't already selected.

The schematic will have different areas for the various parts of the board. In the case the Trinket M0, there sections for the SAMD21 microcontroller, USB connection, power regulation, and most importantly for this project are symbols to represent the rows of holes for mounting headers or other connections. 

To remove all the redundant pieces, we’ll have to use eagle’s group and delete modes to select and then delete all of the nets and components from the schematic except for the headers, shown here

With the schematic window open, select the group tool to select as much of the schematic as you can, except for the headers. Once selected, everything in the group will be highlighted. You can then select the delete tool, right click on the group and select delete group.

Repeat this process until the only thing left is the headers and the nets connected to them. We also want to remove the schematic frame and all the text in it because what we're left with will be pasted into another schematic, so this frame won't be needed.

You’ll want to make sure to keep the little pieces of nets that connect to the header as they have important information about what pins on the Trinket the headers pins go to.

Once you have removed everything in the schematic except for the headers and the nets connected to them, you should be left with a very sparse schematic:

Now that the schematic has what we want, switch to the board window by clicking the SCH/BRD button in the toolbar:

Now in the board window you should see a representation of the Trinket board but now it will be missing some pieces because we deleted them from the schematic. We want to delete everything from the board except for the headers and the outline, however It's possible that you don't have all the layers visible so we'll need to make all the layers visible for the things we want to delete. Additionally, we'll hide the layer with the outline (layer 20, Dimension) so that it won't be deleted.

Click on the Layer Settings tool, select Used Layers from the Filter dropdown, and click Show Layers.  Then de-select the Dimension layer and click OK to make the rest of the layers visible.

With all the layers visible you can see that there is a lot of information available in the board file, most of which we're not going to use. Among these are the Adafruit logo and any other branding on the board. Adafruit open-sources their designs but their name and logos are their trademarks and should not be used without their explicit permission.

Slimming down the board

Use the Group tool to select everything and then like with the schematic select the Delete tool, right click on one of the selected items and choose Delete Group. 

Eagle will pop up a warning saying that you're trying to delete elements that cannot be back annotated, in this case, it's talking about the headers and not deleting them is precisely what we want. Back annotation refers to Eagle's ability to keep the schematic and board in sync and will not allow you to remove the functional schematic elements from within the board window.

Click OK and you should be left with just the headers and the outline. If anything else is left over, go ahead and delete them as well.

You are now ready to save the headers as a design block.

Click the SCH/BRD button on the toolbar to switch back to the schematic view. In the schematic window's menu click  File > Save as Design Block

This will pop up the Generate Design Block window. If you wish, you can include a brief description of the part you’re working on however I honestly skip this step. Click “Save as…” and give the block a name. The window will allow you to select a different location to save the design block however I strongly recommend that you use the default location as it will make it easier to find later. Once you have chosen a name, click “Save” to create the design block.

You now have a Design Block that you will use later when we create a new schematic for the adapter board. Use the same process to create a Design Block for the header on the INA219 breakout and you'll be ready to create the schematic.

For the INA219 Breakout schematic, you'll need to delete the pull-up resistors from the header part of the schematic so you're left with just the header and the nets connected to it, leaving you with something like this: