Syntax: .include <filename>
This directive includes the named file as if that file had been typed into the netlist instead of the .include command. This is useful for including libraries of models or subcircuits.
An absolute path name may be entered for the filename. Otherwise LTspice looks first in the directory %HOMEPATH%\Documents\LTspiceXVII\lib\sub and then in the directory that contains the calling netlist and finally in the list of directories listed in the Library Search Path.
No file name extension is assumed. You must use ".inc myfile.lib" not ".inc myfile" if the file is called "myfile.lib"
It is possible to specify a url of the following form as a file name:
.inc http://www.company.com/models/library.lib
The file "library.lib" will be http-transferred to the circuit directory and included. For subsequence simulations, in the interest of avoiding downloading the file each time you run the simulation, you can edit the .inc statement to
.inc library.lib
Note that if the url you specify doesn't exist, most web servers don't return an error, but return a html web page to be displayed in your web browser that explains the error. LTspice can't always read these pages as error conditions so you may get some cryptic error message when the simulation tries to proceed with the included html language error page included in the simulation as valid SPICE syntax.