Electronic – Hspice to Ltspice conversion

hspiceibisltspice

Has anyone had any luck converting Hspice or IBIS model files to formats LtSpice can use? Any help much appreciated, thank you!

Best Answer

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.

Related Topic