Even though most of these have been answered above, I’ll take a stab at all of them at once for ease of reference.
You cannot use encrypted models. I did want to mention, although I’ve never tried myself, I’ve heard from many sources that contacting certain manufacturers directly for unencrypted versions of models can result in them providing them if you sign an NDA. After all, if you’re going to buy a significant quantity, they want to provide an easier design path for you. For other situations such as TI only providing a TINA model, I have spent the time to develop my own behavioral models for certain parts that I use frequently (the THS video amplifier series in particular). Although, it’s time consuming, you do come out with the added benefit of you understanding the part’s functions more thoroughly than you would have before. This can result in better designs in the real world.
Yes, if you set the compatibility switch (set ngbehavior=ps) in the newer versions.
For basic semiconductor models, yes. You can either copy the entire files found in \LIB\CMP or copy/paste the “.model” statements within those files for parts you want to split off into your own .LIB file. Even VDMOS is now supported by ngspice, which used to previously only been supported by LTspice. For subcircuits, you can open up the *.LIB or *.SUB files in the \LIB\SUB directory for LTspice and see that many of these libraries are unencrypted. However, several of them use LT’s proprietary A-devices to construct these subcircuits. So, I don’t believe you’ll be able to easily port those (without significant redesigning) into another SPICE software that doesn’t implement the A-devices exactly like LTspice does. I don’t really understand how ngspice’s XSPICE plays into this, so someone please correct me if I’m wrong. For models which don’t use A-devices, you can try them out and see if you’re successful. I did get the LT1083.lib to work in KiCad by using it as a model for an LM7805 symbol, as shown below.
Not sure. I never noticed it until you mentioned it.
I’ve used it to launch LTspice using KiCad. It passes the netlist generated by KiCad and runs it within LTspice, using LTspice’s GUI. There’s obviously no backannotation, so you can’t probe anything and have to add in plots/traces manually. I think this is the best way for doing simple DC operating point analysis (.op command) since it’s not supported in KiCad directly.
With certain command-line parameters, you can also have it output the RAW data to a text file for analysis later. I’m using the Windows KiCad version, and it’s very picky on having spaces in your path and it doesn’t respect quotes either. I can only get it to work using DOS style paths.
I have never tried this, and I’m not equipped to answer this question well. My gut tells me that you have it backwards and you would be ensuring more errors. Netlist orders in LTspice symbols are completely shuffled around compared to KiCad symbols.