Sometimes printers can scale things. I had trouble with my printer 'shrinking' designs, but not as much as 1/8th.
If the length and width are the same scale (as in reduced by the same percentage) then you can decrease the border width in eagle.
The only way I could effectively print out to scale was to scale my design up to counter-act the shrinkage from my printer.
go to 'print setup -> page -> calibrate'
Values greater than 1.000 will increase the size, values < 1.000 will obviously shrink. It is best to create a test design, full size (as large as eagle will allow, 3"x4" if its freeware)
With lines, and pads spaced apart by a KNOWN amount. On the design, mark the length and distance between these lines...then when you print it out, measure their actual values. The amount you must scale is the value its meant to be, divided by the actual value.
Example: your PCB design in eagle had dimensions 4"x3". But your print out measured 3.875 x 2.91. Length (x): 4/3.875 = 1.032 - Width (y) = 3/2.91 = 1.031.
You can of course use the same value for X and Y, but, printers generally are less accurate in a certain axis. So you can scale each axis individually. On mine the length was less accurate (shrunk more) than the width...and it also wasn't very accurate towards the edges of the page..so print your design in the centre of it rather than top left or bottom right.
About pads in eagle library:
I haven't found a 'good' way to increase the size of pads for a ready-made component using a user-language-script (ULP). I'm sure they do exist but the best, and unfortunately, most time consuming method is to create your own package for a certain component. Say you have a DIP16 chip, in an eagle library, and you wish to make its pads larger. Instead of completely remaking the 'device' this is how I do it.
1. In the main eagle window, open the library and find the component of interest (click 'device'), make a note of its package.
2. Now click 'package' and look for the package the component uses.
3. Highlight the whole thing with 'group', then click 'cut', and right click on the package.
4. Make a new package (package -> new) click paste. Then use the change button on the left pane to change the size of the pads. (Diemeter, and shape).
5. Save it.
6. Go to the device again (device), at the bottom right where it has the package, click 'new', give it a random extension like 'mod', and choose the package you just created. Then it'll appear in the bottom right window with a yellow exclaimation mark next to it, indicating you haven't link its pads to pins on the symbol.
7. Click 'connect' then 'copy from' the drop down menu and pick an existing package., then 'ok.
And thats it, you've added a new package to that component. When you choose it in a schematic it'll give two options, the original package, and your own.
It's a really long way of doing it, but you are right, some components like double pin headers, have really small pads, leaving only a tiny ring of copper around them after drilling.
I hope that helps in 'some' way. I've been meaning to make a tutorial for eagle for a while if anyone else is interested in it.
Buriedcode.