AC Simulation in Power supply simulators
The circuit shown is ready for the open-loop analysis you want: \$L_1\$ and \$C_2\$ close the loop in dc and open it in ac analysis. This is an old trick and I traced it back to the Vince Bello times when he first published his average models.

When you run the ac analysis, SPICE computes a bias point to know where all the elements operate. During this moment, inductors are shorted and capacitors are opened. The loop of your converter is thus physically closed by \$L_1\$ and the simulator calculates the correct operating point set by the resistive divider.

When the ac analysis starts, the extremely-low cutoff frequency of \$L_1C_2\$ filter isolates/opens the return path and the converter runs in ac open-loop conditions. Should you change operating conditions (input voltage, load current...), the correct operating point will be computed each time you run the .AC analysis and parameter sweeping is easy.

Now, if you want the power stage transfer function, probe the output voltage and the voltage at the COMP pin. When plotting the ratio of these two variables you'll obtain the control-to-output transfer function you want and decide what strategy to adopt with the compensation elements. Once compensation elements are calculated, probe \$V_{out}\$ only and you'll have the loop gain from which you can infer the 0-dB crossover and various margins. If you now want to test the transient response, reduce both \$L_1C_2\$ to a 1-p value and the loop is now closed in dc and ac. More information in this book.