How to add these components on LTspice for simulation

Question

I would like to add these spice models so i can simulate them in LTspice.

• PBSS4350X (.txt)
• PBSS5350X (.txt)
• AO4407A (.mod)

I have looked into this tutorial on how to add the models, but when I opened the library which contains all models, it looks different on the text files. The PBSS has a .SUBCKT and a .MODEL Diode on them. Do I have to add them to the diode file too?

The .mod file is even much more confusing, the files contains an NMOS where the mosfet where it came from is a PMOS.

It may be of note that doing method 1 in the turtorial where the spice text is just place on the drawing area results in an error.

Answer 1

The first thing to realize is all the manufacturer models you are using are of the .subckt form, i.e. subcircuits. A subcircuit is a collection of other primitive devices, such as resistors, capacitors, diodes, transistors, etc. More complex behaviors can be simulated using a subcircuit over a single primitive device, like a simple .model for a diode as shown in your linked video tutorial. Discrete MOSFETs actually require a subcircuit of some kind, because built-in SPICE primitives for MOSFETs are for monolithic (integrated circuit) applications only. LTspice has an exception to this with its proprietary VDMOS primitive model architecture. However, only the built-in models use this type and a 3rd party manufacturer will rarely provide you a discrete MOSFET model in this form. The AO4407A file you linked is a subcircuit, and I wouldn't worry too much about what's inside the subcircuit (like the monolithic NMOS you mentioned) unless you are the subcircuit designer or want to modify it in some way.

---

The least brain-intensive way to add subcircuit models on your system is to first put the library file into your Documents\LTspiceXVII\lib\sub folder and then use this tutorial: https://www.analog.com/en/technical-articles/ltspice-simple-steps-to-import-third-party-models.html

If you want to use standard symbols instead of the generic boxes generated by the above method, you need to Ctrl+rightclick each symbol and change the prefix to X as described in this tutorial: https://www.analog.com/en/technical-articles/ltspice-using-an-intrinsic-symbol-for-a-third-party-model.html

Answer 2

I think your problem is that you are trying to use subcircuits as models. These are very different things in SPICE. If you want to use a subcircuit then the elements instance should begin with an X rather than a Q or M.

A subcircuit is a hierarchical element that contains other primitive elements (transistors, diodes, resistors, etc.). These primitive elements may have their own model files.

A model contains only parameter values that will be used in equations built-in to the simulator.

Your AO4407A.mod file is not a model file, it is a subcircuit for something called an HP21AC. Your PBSxxxx files are also subcircuits.