Eagle cad dimension measurement showing on top and bottom layer when creating Gerber files
The "dimension" layer in Eagle is unfortunately named.  Other CAD/CAM programs might refer to this as a "routing layer".  It is intended to show the outer dimensions of the PCB. It basically shows where the PCB should be cut by a drill or router.

Some of the items in this layer must be placed manually. For example, you should draw your board outline on this layer.

Other features are added automatically. E.g. if you place a 125-mil non-plated drill hit on the board, there will be a 125-mil circle placed on the dimension layer.

One of the design rules sets the clearance distance from any feature on a copper layer to anything on the dimension layer.  This is very convenient with copper pours.  If you choose a 20-mil dimension clearance, the copper is "pulled back" 20-mils away from any cut edges of the board.  This prevents copper from being exposed on the edges of a multi-layer PCB, either on the outer periphery or on the inner edges of drill holes.

So now you see: When you drew lines on the dimension layer, Eagle "conveniently" removed copper from around those lines :)