Q:

Move silkscreen text from component on EAGLE CAD

How can I move a silk text from a component? I cant use the button move to the text and when I click smash nothing happend. I need to move the number 8 inside the board 

Edit1
I try to smash but when I press it, a new text appear and this I can delete it, but I cant move the numbers or delete them, how can I modify the footprint? or erase the numbers and add it manually?
(you see the opcion unsmash because I already smash it)

Edit2
I did it! Thanks all! I could modify the footprint going to library, then selecting the library, then package :)

A:

While @crasic's answer is correct for attribute labels, it does not work with regular text.
Basically when the component is designed, the name and value are added as a text label set to a special placeholder - >NAME and >VALUE to be precise. Other attributes can have similar placeholders. When you smash a component, it only allows free movement of any of these attribute labels (anything beginning with a >).
When you add other text like the number 8 you have there, they are not attributes, so you cannot move them after smashing. This is actually quite sensible as you could move that number 8 label to the other end of the connector which would mean as a reference it becomes useless.

The only way to move that label is to edit the footprint and either (a) delete it, (b) move it where you need it, or (c) move it to the References layer.

To elaborate on (c), you would normally not include the References layer when generating Gerber files, so if the label is on that layer it won't appear on your final PCB. What you can then do is in your board layout manually add a number 8 using the TEXT tool and place it where you want. 
By doing it this way it means that if you want to use the same footprint on another board you don't need to modify the footprint again for that new board. 
Furthermore, by leaving the label on the reference layer, if you move the component around you will be able to still see the reference as a reminder where pin 8 is. If the component is moved, you will have to move your added text label and place it in the correct place.

A:

Smash is a command, you need to select Smash tool (or type SMASH into the command interpreter) and then click on the part. 
There are some caveats - the part origin is either top or bottom, while the pads are on both sides, if you place the part on the bottom but hide the bOrigins layer you will not be able to select the part to smash but this is not obvious because you can still see the pads of the part
You can explicitly invoke smash on the part by typing SMASH JP1 in the command interpreter (replacing JP1 with whatever the reference designator for the part is) 

A:

I think, the 8 is the number of a pin, and its location is fixed in the footprint (unlike a component designator).  Two things could be done.

Change the footprint.  Move the 8 to the desired position.
[This is what I would do.]  Add another 8 as free text to the PCB.  Since it's not a part of a footprint, you can position it where you want.  You will end up with two 8s.  One inside of the board, another cut off by the board edge.  By the dame token, you could also add a 1 next to pin 1.

as an aside:
Smash un-docks the designator from the footprint.

Select the smash too on the toolbar.  
Click on the component you want to smash. (You can also do it from a command line, like @crasic had described above.)
The designator's own drag handle appears.

