Hspice to Ltspice conversion
Quoting Mike Engelhardt (who develops and maintains LTspice):


  LTspice understands some hspice syntax.  For example, it understands
  single quotes for parameter substitution as well as ".lib 'file.lib'
  FAST" syntax.  It won't usually be able to understand a '$' symbol as
  the start of a comment in-line. Usually this is enough to be able to
  run 3rd party foundry BSIM3 models without modification as long as all
  dimensions, areas, and perimeters are specified.  LTspice development
  policy is that went there is a conflict between PSpice and hspice
  syntax, LTspice will follow PSpice because it a more widely used
  standard.


and also,


  LTspice does not do the Philips MOS 9 device.  As I recall, that model
  is now open sourced but it is in FORTRAN.  Also, I should mention that
  a general rule is that LTspice does not do the hspice-specific
  semiconductor enhancements.  You can use the 2nd edition of
  Semiconductor Device Modeling with SPICE by G. Massobrio and P. Antognetti as a good reference for hspice vs PSpice device
  enhancements. The PSpice enhancements in that book can be used as an
  LTspice manual.


and then on IBIS,


  No, IBIS isn't in LTspice.  I think IBIS was an Intel invention that
  allowed them to give behavioral descriptions of their I/O pins without
  giving out implementation details.
  
  Anyway, I think IBIS amounts largely to an IV curve. The DC curve you
  can put in an IV lookup table.  To do the dynamic behavior, you're
  better off with some kind of transistor level model of the device. 
  Attached is an example of using a lookup table in a current source. I
  don't know if it's otherwise documented anywhere.

Version 4
SHEET 1 880 680
WIRE -32 320 -32 288
WIRE -32 208 -32 176
WIRE -32 176 -160 176
WIRE -160 176 -160 208
WIRE -160 288 -160 320
FLAG -160 320 0
FLAG -32 320 0
SYMBOL current -32 208 R0
SYMATTR InstName I1
SYMATTR Value tbl(-5 -1 -2 -.5 0 0 1 1 5 2)
SYMBOL voltage -160 192 R0
SYMATTR InstName V1
SYMATTR Value 0
TEXT -152 368 Left 0 !.dc V1 -5 5 1m



But from someone else on IBIS and LTspice:


  I use a free utility from IntuSoft called IBIS2SPICE.
  
  It reads in IBIS models (up to version 2.1) and generates an
  equivalent    behavioural spice model. It's originally intended to
  generate a model  compatible with Intusoft's spice, but can be
  configureed to generate  models for other spices based on a template
  file. There's a templeate  file available on the net somewhere to
  configure it for PSpice models.
  
  I can't really vouch for the accuracy of the models it generates, and 
  it's limited to IBIS version 2.1.
  
  Generally it would be a great feature to have in LTSpice, but I guess 
  it's not a priority for LT's chip designers, IBIS tends to be used 
  primarily by board designers for board level Signal Integity analysis.


The above comments are from some years ago. Perhaps that will help some.