LTspice model for LM317 and the calculators gives different output voltages for the same resistors values
The correct nominal voltage according to datasheet calculations is 9.138V (min 8.775, maximum 9.50 resulting from the reference voltage tolerance, ignoring resistor tolerances and adjust current tolerance) 

The equation is:  \$V_O = V_{REF} (1+R_2/R_1) + (I_{ADJ} R_2)\$

The 9.06V (nominal) calculator results from ignoring the effect of the 50uA nominal Iadj current.  



Edit: 

There are a number of LM317 models installed in LTSpice (at least in mine). The first one I tried (unknown source) yielded an output voltage of 9.125V, close enough. The second, a MOT model yielded 9.636V, which is a bit out of spec. The MOT-2 model oscillates (lol) with 100n or 1uF - supposedly not needed for stability- and yields 9.161V with 10uF. The TI and TI-2 models both give 9.467V- close to being out of spec. 

The 240 ohm resistor is really putting load that is less than it should be on the output (though you'll see it a lot), so might want to try again with a significant load on the regulator- nope with a 2K load in addition the voltage on MOT is 9.635V, pretty much as you'd expect with it being in regulation sans load. TI model similarly drops about 1 mV with the extra 5mA load.  

The results don't really engender a lot of confidence in the results being very accurate at DC.