After some trouble I figured out how to use a vendor-supplied SPICE module in LTSPICE. I think this is it:

1. Find the LTSPICE library directory. On my computer it is in

~/.wine/drive_c/Program Files (x86)/LTC/LTspiceIV/lib

2. Get the SPICE model you want, e.g.

​http://www.nxp.com/products/rf/transistors/bipolar/oscillators/6_ghz_gt_12_ghz_x_ku_low_band/BFG425W.html

In the "All Models (zip)" archive find the file "BFG425W_SPICE.PRM" and save it.

Rename it to e.g. BFG425W.lib and put it in the .../lib/sub directory.

Edit it like so:

    * Filename:  BFG425W.lib
    .SUBCKT BFG425W 1 2 3

The filename probably is just a comment, but the SUBCKT name must match what's in the .asy file below

3. Go to the .../lib/sym directory. Copy a symbol which matches your model, e.g.

     $ cp npn.asy BFG425W.asy
   

4. Edit e.g. BFG425W.asy like so:

       SYMATTR Value BFG425W
       SYMATTR Prefix X
       SYMATTR SpiceModel BFG425W.lib
       SYMATTR Value2 BFG425W
   

The prefix "X" specifies a spice subcircuit invocation. The "Value2" property is the subcircuit name.

Now you should find a new component BFG425W when you use the place component function.