Hi Shadow,
If you look at the Maxim files, you'll see that the model .fam and Orcad .lib files are identicle and fully compatable with the LTSpice .sub subcircuit files. Save one or the other in the .sub directory in a new folder (with a general name of your choice for its type) so it can be sourced easily if necessary. Remember the full path, name and extention it is saved as for the .inc spice directive such as .inc {folder name}/MAX4173T.sub. You will have to built a 6 pin block if you use the include directive; I couldn't find one readily avalilable.
I went ahead and built a the block and edited it as a symbol file (.asy). If you would like that option, I'll post it below and you can put it in your symbol library. The Symbol Attribute line of SpiceModel may have to be edited since it's pathed to the location of my .sub MAX4173.
Version 4
SymbolType BLOCK
RECTANGLE Normal 112 96 -112 -96
TEXT -79 -64 Left 0 Gnd
TEXT -80 0 Left 0 Gnd
TEXT -79 65 Left 0 Vcc
TEXT 81 65 Right 0 Rs+
TEXT 81 0 Right 0 Rs-
TEXT 80 -64 Right 0 Out
PIN -112 -64 LEFT 8
SYMATTR Value MAX4173T
SYMATTR Prefix X
SYMATTR SpiceModel Misc\MAX4173T.sub
SYMATTR Value2 MAX4173T
SYMATTR Description SOT23, Voltage-Output, High-Side Current-Sense Amplifier
PINATTR PinName 1
PINATTR SpiceOrder 1
PIN -112 0 LEFT 8
PINATTR PinName 2
PINATTR SpiceOrder 2
PIN -112 64 LEFT 8
PINATTR PinName 3
PINATTR SpiceOrder 3
PIN 112 64 RIGHT 8
PINATTR PinName 4
PINATTR SpiceOrder 4
PIN 112 0 RIGHT 8
PINATTR PinName 5
PINATTR SpiceOrder 5
PIN 112 -64 RIGHT 8
PINATTR PinName 6
PINATTR SpiceOrder 6
I've attached a sim of the basic circuit with an input ramp from 3V to 28V and graphed the output voltage and load current to display the degree of error over the entire range. Rsense and Rload values were chosen arbitrarilary withing the ranges from the datasheet; your needs will likely differ.
Hope this helps you with your project.