This forum is a user-to-user support forum and not the right place to address feature enhancements to the KiCad developers.
Your request has been addressed some time ago at the bug/feature tracker https://gitlab.com/kicad/code/kicad/-/issues/2566. There also has been discussed an intermediate solution:
By adding a .control section to the Eeschema circuit diagram, replacing the previous single line in a text box
.ac dec 10 1 1Meg
you may use the output commands offered by stand-alone ngspice. This is an example:
.ac dec 10 1 1Meg
.control
* wait until simulation has finished
set controlswait
* cd into a directory with writing access
cd D:\Software\Spice\kicad\sallen_key
* set ouput format for cvs
set wr_vecnames
set wr_singlescale
option numdgt=7
* data to csv file
wrdata skey.csv "/lowpass"
* data to ps file
set hcopydevtype = postscript
hardcopy skey.ps db("/lowpass")
* gnuplot output (if gnuplot has been installed)
gnuplot skey.gn db("/lowpass")
.endc