[UPDATED, not solved]Simulating a Buck converter
I just entered your schematic into LTspice with the following circuit and results (current in \$R\$.)



(I changed the .TRAN card to provide \$200\:\mu\text{s}\$ instead of \$100\:\mu\text{s}\$ of span on the graph.)

As you can see, the results are what you expected to see. Yes, I did use your options card, as well (not shown on the schematic above.) However, I was not able to use ITL5=50000 as LTspice doesn't recognize that one.



Here's my netlist:

VS 1 0 110
Vy 1 2 0
Vg 7 3 PULSE(0 20 0 .1n .1n 27.28u 50u)
RB 7 6 250
Le 3 4 681.82µ
Ce 4 0 8.33µ
L 4 8 40.91µ
R 8 5 3
Vx 5 0 0
Dm 0 3 DMOD
.MODEL DMOD D(IS=2.2E-15 BV=1800V TT=0)
Q1 2 6 3 0 QMOD
.MODEL QMOD NPN (IS=6.734F BF=416.4 BR=.7371 CJC=3.638P CJE=4.493P TR=239.5N TF=301.2P)
.ic V(4)=60
.tran 0 1.7m 1.5m 1u uic
.options abstol = 1.00n reltol = 0.01 vntol = 0.1




I'd recommend downloading and installing LTspice to see if you can replicate the results you want with it. If so, then perhaps there's something else with respect to the spice program you are using that you need to adjust. If you don't want to use LTspice for some reason, then I'd recommend disclosing the spice program you are using to get the results you show. Perhaps someone else will be familiar with it and can guide you.