You might be able to do this with the help of stepped simulations and measurement commands.
Consider this simple voltage to frequency converter:
This will convert a voltage at the FM port to a voltage with the frequency at the Q port.
To get a plot of voltage versus frequency, I use a stepped input voltage using .step param Vin 1 100 1 and of course the parameter has to be used by the voltage source controlling the FM port, so I put {Vin} there.
Then I need to measure the frequency in a way, the data is recorded in a way it can be processed by LTSpice. This is done using .meas directives:
.meas t1 FIND time WHEN V(FreqOut)=0 RISE=1
.meas t2 FIND time WHEN v(FreqOut)=0 RISE=2
.meas T param t2-t1
This measures the time from the first zero crossing to the second zero crossing. This probably needs some tweaking for your application. It can have a delay so it will start only after some time, when your circuit reached a stable state.
After that open the error log View -> SPICE Error Log, right click the error log and select Plot .step'ed .meas data:
You will get a new empty plot window. Right click and add a trace, in this example type 1/t to get the frequency:
Complete netlist for this experiment:
A1 VoltIn N001 0 0 0 0 FreqOut 0 MODULATOR mark=1 space=0
V1 N001 0 1
V2 VoltIn 0 {Vin}
.param Vin 5
.tran 1
.meas t1 FIND time WHEN V(FreqOut)=0 RISE=1
.meas t2 FIND time WHEN v(FreqOut)=0 RISE=2
.meas T param t2-t1
.step param Vin 1 100 1
.backanno
.end
