Is there a potentiometer model for LTspice?

...has anyone done this already?

Yes, someone has already done this. (I believe his name is Helmut Sennewald).

The Yahoo LTSpice group has a set of potentiometers that work very well. You will have to register a Yahoo account and join the group to download them (by the way, I highly recommend doing this if you want to pursue LTSpice, the Yahoo group has one of the larger collection of third-party LTSpice models).

The relevant files are potentiometer_standard.lib and potentiometer_standard.asy, as well as some other supporting files.

The models provide linear, log, and other models, as well as a potentiometer symbol. The following is an excerpt from the readme file.

pot_lin : ideal linear resistance dependency
pot_pow : ideal power function resistance dependency
pot_plog : ideal positive logarithm function resistance dependency
pot_nlog : ideal negative logarithm function resistance dependency
potr_tab: arbitrary(table) based resistance dependency
pot_piher_plog : pseudo logarithm function resistance dependency, Piher
pot_radiohm_plog : measured pseudo logarithm fucntion resistance dependency, Radiohm

How would this taper be "controlled" during simulation?

These pots have a wiper property which can be easily parameterized as a regular LTSpice parameter. For example, you might say wiper={GAIN}, and then add a directive such as .step param GAIN 0 1.0 0.25.

Tried to follow the suggestions above but took me a awfully long time to create a potentiometer that looks like a potentiometer and that can be instantiated from the main schematic. So, for the benefit of anyone that may be as dumb as me...

Just copy these 3 files to a directory in the LTspice search path (erase any initial spaces in every line). Hope the names are self-explanatory.

potentiometer_test.asc

    Version 4
    SHEET 1 880 680
    WIRE 272 48 0 48
    WIRE 528 48 272 48
    WIRE 272 80 272 48
    WIRE 528 80 528 48
    WIRE 0 96 0 48
    WIRE 0 192 0 176
    WIRE 272 208 272 176
    WIRE 528 208 528 176
    FLAG 272 208 0
    FLAG 0 192 0
    FLAG 320 128 out1
    FLAG 528 208 0
    FLAG 576 128 out2
    SYMBOL voltage 0 80 R0
    SYMATTR InstName V1
    SYMATTR Value 10
    SYMBOL potentiometer 272 176 M0
    SYMATTR InstName U1
    SYMATTR SpiceLine2 wiper=0.2
    SYMBOL potentiometer 528 176 M0
    SYMATTR InstName U2
    SYMATTR SpiceLine R=1
    SYMATTR SpiceLine2 wiper=0.8
    TEXT 140 228 Left 2 !.op

potentiometer.asy

    Version 4
    SymbolType BLOCK
    LINE Normal 16 -31 -15 -16
    LINE Normal -16 -48 16 -31
    LINE Normal 16 -64 -16 -48
    LINE Normal 1 -9 -15 -16
    LINE Normal 1 0 1 -9
    LINE Normal 1 -94 1 -87
    LINE Normal -24 -56 -16 -48
    LINE Normal -24 -40 -15 -48
    LINE Normal -47 -48 -15 -48
    LINE Normal -16 -80 16 -64
    LINE Normal 1 -87 -16 -80
    WINDOW 0 30 -90 Left 2
    WINDOW 39 30 -50 Left 2
    WINDOW 40 31 -23 Left 2
    SYMATTR Prefix X
    SYMATTR ModelFile potentiometer.lib
    SYMATTR SpiceLine R=1k
    SYMATTR SpiceLine2 wiper=0.5
    SYMATTR Value2 potentiometer
    PIN 0 -96 NONE 8
    PINATTR PinName 1
    PINATTR SpiceOrder 1
    PIN 0 0 NONE 8
    PINATTR PinName 2
    PINATTR SpiceOrder 2
    PIN -48 -48 NONE 8
    PINATTR PinName 3
    PINATTR SpiceOrder 3

potentiometer.lib

    * This is the potentiometer
    *      _____
    *  1--|_____|--2
    *        |
    *        3
    *
    .SUBCKT potentiometer 1 2 3
    .param w=limit(wiper,1m,.999)
    R0 1 3 {R*(1-w)}
    R1 3 2 {R*(w)}
    .ENDS

Google LTSpice potentiometer, there are lots of examples with varying degrees of complexity. Most use a sub-circuit along these lines:

* This is the potentiometer
*      _____
*  1--|_____|--2
*        |
*        3
*
.SUBCKT potentiometer 1 2 3
.param w=limit(wiper,1m,.999)
R0 1 3 {Rtot*(1-w)}
R1 3 2 {Rtot*(w)}
.ENDS