How do I define a tented via-in-pad in Eagle?
If you're willing to live with octagonal soldermasks on your vias, then try the following:


Define the SMD ground pad, and disable the stop mask.
Place pads where you want your vias. Make the pads have the same characteristics as the vias you want. We will delete these pads later.
Show the soldermask layer (tStop)
Draw a polygon on the tStop layer in strips. This is to prevent your polygons from enclosing any area, and so that it's easier to draw. If you want a 3x3 grid of vias, then you would need four polygons.
Delete pads used as a template. The package is now done.
Place package in layout
Place vias
Use the "NAME" function to change the via net to the same net as the pad - probably "GND"
Route vias / add pour



After this, you will have the vias on the correct net, and your soldermask will come out as you wanted. The drawbacks that I see are:


The vias must be manually placed in the final board
Each via must be renamed to the target net (I couldn't get the GROUP function to work).
The soldermask is an octagon instead of a circle
There isn't an automatic way to draw the STOP mask for the package
Each via gives an overlap error in DRC (can be ignored).
No easy way for a STOP mask on the bottom side without drawing it manually


I was able to get this to work using Eagle 5.1 in about 15-20 minutes, so not too bad.