After having my first board im tempted to try the SeeedStudio Fusion pcb service, and I don't know how to define my board size, is there some specific layer for that or some special trace?
First, I do recommend SeeedStudio's Fusion. Been happy each time I get boards back from them. On the Fusion page, there is a link to Eagle DRC rules and CAM files. Make sure you have those and run it often. (If the DRC is loaded and you use Eagle's auto-router, the auto-router will automatically follow the design rules...)
http://www.seeedstudio.com/depot/datasheet/Fusion%20eagle.zip
There are calculators on web to help with trace width. In general I have found even the smallest widths that services like SeeedStudio support are large enough for most hobby-electronics class projects. Their minimum is 6mil, but I tend to use 8 or 10mil. If I am routing large amounts of power and have space, I'll go to 12. Similar with minimum spacing, even though they allow 6mil I bump the DRC up to 8 for extra margin.
When editing schematics in Eagle it is important not to change the grid size from 0.1in. Otherwise, the editor will not detect connections properly.
On PCBs, I tend to switch between inches and mils when I'm drawing traces. I try to use multiples of 0.025inch. I will generally set my "Alt" grid spacing 2-3 times more fine than the "Size" value. (The "Alt" grid is enabled anytime you press the Alt-key. So while placing a part or text label, you can get a finer grid.)
The dimension layer (20) is the best place to draw the outline of your board, and I think that is the default layer. For text I use (21) tPlace and (22) bPlace for silk screening.
Before running the CAM processor, I like to turn off ALL the layers, except (19) Unrouted. Sometimes it is hard to miss a connection you though you made.