Which of 3 SPICE models to use with LTSpice?

[741]

Here (https://www.vishay.com/mosfets/list/product-62806/tab/designtools-ppg/) are 3 models for the SQJ407EP PMOS device.

There are 2 'PSpice' and 1 HSpice' model.
SQJ407EP_HS_REVA.TXT
SQJ407EP_PS_RC_REVA.TXT
SQJ407EP_PS_REVA.TXT

My guess is I use PSpice. The larger model seems to incorporate some temperature modelling (?)

I am using this device as an on/off switch carrying 5A. The switch is used infrequently (on or off according to user selection), and so long as it switches fully on or off, I think I do not need to use the more elaborate model.

[Ian.M]

SQJ407EP_HS_REVA.TXT uses the non-standard MOSFET CAPOP parameter which LTspice doesn't support. *AVOID* !!!

SQJ407EP_PS_REVA.TXT appears to be a 'vanilla' SPICE3 subcircuit model consisting of four active parts (two level 3 MOSFETs, a diode and a unit gain voltage controlled voltage source), two fixed sources and a sprinkling of passives.  Its likely to be your best bet for LTspice.

SQJ407EP_PS_RC_REVA.TXT  uses the obsolete voltage dependent current source

Code: [Select]

Gname node1 node2 VALUE {<expression>}syntax which is an alias of the behavioral current source

Code: [Select]

Bname node1 node2 I=<expression>LTspice *should* handle it but may misbehave if there's any sort of feedback loop in the thermal modelling subcircuit.  Its also likely to be significantly slower.