¿ªÔÆÌåÓý

  1. LTspice
  2. Topics

MosFet "LEVELS" in LTSpice compared to other spice simulators

 

Hello,


I am getting confusing hints from search results: ..

So a mosfet "level" is a way to model a mosfet using a set of defined parameters. (?)

There are many so called "levels" and there have been numbers assigned to them, without this meaning that one is necessarily an evolution of the previous. I see on this manual for example (http://ecee.colorado.edu/~mathys/ecen1400/pdf/scad3.pdf) that ltspice can understand at least 10 of these levels.


1)Is this numbering kept same across LTSpice, PSpice, HSpice?

2)Do all simulators use all the parameters with the same name or are they free to introduce/remove/mix parameters?

3)Will LTSpice complain if we pass to it a parameter name that it cannot understand in a model, or just ignore it without reporting?

4)Is there some solid documentation on ALL of the ltspice mosfet levels?


Any hints welcome, thanks!
 

Hello,

> 1)Is this numbering kept same across LTSpice, PSpice, HSpice?

No.

> Do all simulators use all the parameters with the same name or are they free to introduce/remove/mix parameters?

Most of the parameters are the same, but especially HSPICE has often additional parameters.

I vaguely remember that Spice programs can have different equations to calculate Weff and Leff, but I am not an IC designer and thus I may be wrong here.

>3)Will LTSpice complain if we pass to it a parameter name that it cannot understand in a model, or just ignore it without reporting?

Yes, LTspice reports ignored parameters in the Log-file.
View -> SPICE Error Log

> 4)Is there some solid documentation on ALL of the ltspice mosfet levels?

I only know of the text in the Help. See below.

Tip: Don't change any Level=... .
?LTspice recognizes the corresponding levels of PSPICE and HSPICE.


Best regards,
Helmut



level???model

------------------------------------------------------

?1???Shichman-Hodges

?2???MOS2(see A. Vladimirescu and S. Liu, The Simulation of MOS Integrated Circuits Using SPICE2, ERL Memo No. M80/7, Electronics Research Laboratory University of California, Berkeley, October 1980)

?3???MOS3, a semi-empirical model(see reference for level 2)

?4???BSIM (see B. J. Sheu, D. L. Scharfetter, and P. K. Ko, SPICE2 Implementation of BSIM. ERL Memo No. ERL M85/42, Electronics Research Laboratory University of California, Berkeley, May 1985)

?5???BSIM2 (see Min-Chie Jeng, Design and Modeling of Deep-Submicrometer MOSFETs ERL Memo Nos. ERL M90/90, Electronics Research Laboratory University of California, Berkeley, October 1990)

?6???MOS6 (see T. Sakurai and A. R. Newton, A Simple MOSFET Model for Circuit Analysis and its application to CMOS gate delay analysis and series-connected MOSFET Structure, ERL Memo No. ERL M90/19, Electronics Research Laboratory, University of California, Berkeley, March 1990)

?8???BSIM3v3.3.0 from University of California, Berkeley as of July 29, 2005

?9???BSIMSOI3.2 (Silicon on insulator) from the BSIM Research Group of the University of California, Berkeley, February 2004.

12???EKV 2.6 based on code from Ecole Polytechnique Federale de Lausanne. See and "The EPFL-EKV MOSFET Model Equations for Simulation, Version 2.6", M. Bucher, C. Lallement, F. Theodoloz, C. Enz, F. Krummenacher, EPFL-DE-LEG, June 1997.

14???BSIM4.6.1 from the University of California, Berkeley BSIM Research Group, May 18, 2007.

73???HiSIMHV version 1.2 from the Hiroshima University and STARC.
 

'selportion'?wrote:

? ?"So a mosfet "level" is a way to model a mosfet using a set of defined parameters. (?)"

There are different "levels" because there is not only a single way (one set of equations) to describe how a MOSFET works. ?Different research groups formulated different sets of equations. ?SPICE took the different descriptions (sets of equations) and assigned each of them a LEVEL. ?Each LEVEL might use a few different parameters than the other LEVELs, and might use the parameters in different ways because their equations are not the same.

? ?"1)Is this numbering kept same across LTSpice, PSpice, HSpice?"

Not exactly, but some are the same. ?I believe the first few LEVELs (1 through 3, maybe as high as 6) might be the same, because Berkeley SPICE (the original SPICE) had those levels already, and many of the higher numbered levels came later after the other SPICE programs branched off. ?Unfortunately there is no "central clearing house" for assigning LEVEL numbers.

I think HSPICE was the main offender at creating multiple new LEVELs. ?Years ago they had four or five dozen levels that were unique to HSPICE.

? ?"2)Do all simulators use all the parameters with the same name or are they free to introduce/remove/mix parameters?"

If a LEVEL is the same, then there is a good chance that the parameters for that LEVEL are the same. ?But again, because there is no clearinghouse, a SPICE program could modify how a LEVEL works but not give it a new LEVEL number (which in my opinion is how they should have done it).

Another problem with HSPICE models, is that HSPICE lets the user re-define some of the base units, for example, to use microns rather than meters in the model parameters. ?That is cause for a lot of grief.

? ?"3)Will LTSpice complain if we pass to it a parameter name that it cannot understand in a model, or just ignore it without reporting?"

It will give a warning, and then ignore the unknown parameter and proceed without it. ?You need to look in the log file to see the warning.

? ?"4)Is there some solid documentation on ALL of the ltspice mosfet levels?"

LTspice's Help pages list many, but I think LTspice itself understands more MOSFET LEVELs than the eleven levels currently listed there. ?(Note the actual Help pages in the program include one more level than the list in the file you referred to, which is an earlier 'snapshot' of the Help pages.) ?Unfortunately, LTspice's documentation always seems to be lagging to some degree.

Regards,
Andy
 

Quite a mess, as expected :)
Thank you Andy, I think I have it clear now.

1 - 4 of 4