EAGLE detecting error at Copper Trace intersecting Dimension Outline
The problem is that SparkFun created the ARDUINO_MEGA device in the Eagle library with its own boarder using the Dimension layer. Eagle expects one single outline of your PCB using the Dimension layer. By including the ARDUINO_MEGA device in your design, you now have two independent board outlines in the same project.

In the DRC settings, one of the options defines the closest allowable distance between any copper and the board outline:

In this example, there must be a 15mil space between any copper on the board (traces, pours, vias, through holes) and the edge of the board. The "edge of the board" is defined by any lines in the Dimension layer. Obviously, if you intersect a line in the Dimension layer with a copper trace, you are violating this rule. Eagle isn't smart enough to realize that the outline of the ARDUINO_MEGA doesn't define the outline of your entire design. It just sees copper getting too close to a Dimension layer element and applies the DRC.

Here are two possible work-arounds:  


Approve the error in the DRC and don't worry about it. 

This is fine if you're making the PCB yourself or if you have a lot of control over the manufacturing process. However, if you're sending Gerber files to a board house or using a service like OSH Park, they may not like you having more than one complete outline in the Dimension layer.
Change which layer the outline of the ARDUINO_MEGA is in. I believe this is a better fix, as it "solves" the problem instead of sweeping it under the rug. First, open the SparkFun-Boards.lbr library in Eagle and click on the Package button.

Select the "ARDUINO_MEGA" package and open it. Click on the Change tool  on the toolbar and select the Layer option. Choose another layer you want the outline of the ARDUINO_MEGA to be in. If you want its outline printed on your PCB with ink, use the tPlace layer. Otherwise, use the tDocu layer. Select each of the line segments that make up the board outline, save it, and exit the library. Once you're back on your board design, click on Library->Update All to make the changes take affect. Run the DRC again and the problem should go away.