Which file to use for LTSpice?

[Wilson__]

This chip has many files. 

Which file to use for LTSpice version (x86) 24.0.12 (downloaded recently)?  For voltage and current analysis of low speed high side power switch.  P-MOSFET as high side switch of 4.2V power source.  N-MOSFET to interface with MCU at 3V.

Many thanks

[Ian.M]

I assume you are referring to the Spice models from https://www.vishay.com/en/product/62968/tab/designtools-ppg/

The .txt and .lib files with the same root filename are (in this case) identical and contain the actual SPICE models.  The .olb files are PSPICE symbols for the models and are useless to a LTspice user.   This reduces it to three possibles:

• SiUD402ED_HS_Rev_A
• SiUD402ED_PS_RC_Rev_A
• SiUD402ED_PS_Rev_A

Unfortunately the accompanying PDF doesn't give any usage details for the three models, and the headers in the model files are also notably uninformative.  It is likely that the HS and PS in the model filenames refer to HSPICE and PSPICE, two well known SPICE modelling programs, not tied to any semiconductor manufacturer.   They both accept standard SPICE3 netlist syntax but PSPICE extends this with its own proprietary syntax for certain devices which LTspice doesn't accept.  HSPICE has the same issue, most notably with extra unnamed parameters for resistors which LTspice also doesn't accept.

Comparing SiUD402ED_PS_RC_Rev_A and SiUD402ED_PS_Rev_A, they both contain *exactly* the same subcircuit model for the SiUD402ED MOSFET, but the _RC_ one also contains a cascaded RC thermal model for the device, to enable PSPICE to determine if it is operating within the SOA boundaries.  LTspice has similar capabilities but I expect you'd have to reverse engineer the PSPICE thermal model to wrangle it into a LTspice SOAtherm compatible format.

Comparing SiUD402ED_HS_Rev_A and SiUD402ED_PS_Rev_A, the _HS_ file is similarly structured to the _PS_ file, but very different on a line by line basis.  They appears to contain the same components (and values) and the same nodes, but the _HS_file has the problematic extra resistor unnamed parameters.

I believe SiUD402ED_PS_Rev_A (either .txt or .lib) is your best bet.  LTspice will give warnings in its error log for PSPICE specific named parameters it doesn't support, but they shouldn't stop the model running or gossly affect its accuracy.