Simple LED model for circuit simulation
If your circuit simulator support importing a SPICE model, you can use the models provided below for different colors of LEDs. 

*Typ RED GaAs LED: Vf=1.7V Vr=4V If=40mA trr=3uS
.MODEL LED1 D (IS=93.2P RS=42M N=3.73 BV=4 IBV=10U
+ CJO=2.97P VJ=.75 M=.333 TT=4.32U)

*Typ RED,GREEN,YELLOW,AMBER GaAs LED: Vf=2.1V Vr=4V If=40mA trr=3uS
.MODEL LED2 D (IS=93.1P RS=42M N=4.61 BV=4 IBV=10U
+ CJO=2.97P VJ=.75 M=.333 TT=4.32U)

*Typ BLUE SiC LED: Vf=3.4V Vr=5V If=40mA trr=3uS
.MODEL LED3 D (IS=93.1P RS=42M N=7.47 BV=5 IBV=30U
+ CJO=2.97P VJ=.75 M=.333 TT=4.32U) 


NOTE: There are three models available here since different LED colors have different characteristics. 
The lines starting with * are comments.

The following simulators support SPICE model importing to my knowledge.


Online e.g. PartSim
Installed e.g. Pulsonix


And since in your case the software has an interface to fill in the parameters just manually fill in the blanks using the models I mentioned. e.g. I_S = 93.1