Re: MosFet "LEVELS" in LTSpice compared to other spice simulators
'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
|
Re: Just noticed ... All group messages here now come from ???
John, Andy,
- I suddenly stopped getting any messages from the list about the same time as that change. Checked to see if somehow the group got added to the yahoo spam list, nada.
- I did change to the Maxthon browser, but things worked fine for weeks afterward, so I'm at a loss. Will see if I can locate the problem.
- RC
|
Hello Sam,
> PULSE(0 10 5u .1u .1u {} 1m)
This is wrong. See the correct version below.
PULSE(0 10 5u .1u .1u {Ton} 1m)
.step param Ton 2u 10u? 2u
.meas ampx? max V(out)
Run the simulation.
View -> SPICE - Error Log
Right-mouse click in this log-file then choose plot.
Best regards,
Helmut
?
|
Re: MosFet "LEVELS" in LTSpice compared to other spice simulators
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.
|
Re: Plot Log curve as inverse to Antilog (Exp) curve?
Hello,
I don't understand your log-plot.
May be you simple asked for the step response of RC-circuits.
.param tau = 0.2
V = 5*(1-exp(-time/tau))
Best regards,
Helmut
|
Plot Log curve as inverse to Antilog (Exp) curve?
I've uploaded 2 files to the Temp folder: curve_exp.jpg curve_log.jpg
To get the exp curve in?curve_exp.jpg?I used: Value: V=5*exp(7*(time-1)) in a Behavourial Voltage source. It gives an exponential climb to 5V over 1 Second.
What equation should I use to get the inverse of that curve shown in?curve_log.jpg ?
Thanks. ?
|
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,
You could use the command from the menu
Plot Settings -> Autorange Y-axis
The shortkey is Ctrl-y
Best regards,
Helmut
|
(1) Choose any plot, drag a rectangle over it all, then all
plots get same time axis limits.
(2) Doing this with "Manual Limits" only zooms the plot selected
(not all).
So: What I'd like to be able to do is -
?? To precisely specify "Manual Time Limits" for all plots at
once - like (1) and (2) combined. --- I gather there is a way to do this, "lock horizontal axis" - but I have not found how to acess this feature yet.
|
Re: Pull-Push transformer for valve amp in LTspice
Hello analogspiceman
I'm not denying that your library works (I have used it a few times, successfully) or that a quasi-real transformer can not be built around the Chan core, but I have never used it with two primaries, which is why I lacked the experience in how to do it and the only very vague notion I had was the remembrance of a past conversation that may have been related to a push-pull, which I couldn't find in the archives. It's also true I didn't insist in searching for it too much but, it's irrelevant now, the question has been answered. Besides, I did try a quick example and I convinced myself that I was wrong (see my post above), which probably means I'm also confused about the memory. And... that's pretty much it.
|
Re: Pull-Push transformer for valve amp in LTspice
Hello Vlad, a transformer has multiple windings, but only one core (which is the only nonlinear part).? That is why LTspice does not allow coupling between saturating inductors (either Chan or behavioral).? If a Chan model is used, it must represent only the single common core, not one for each winding (as can be done for perfectly linear windings).? However, it is quite easy to construct a transformer model such that there is only a single internal core part and an arbitrary number of windings, including any number of identical parallel or push-pull primary windings.? A good and proper model matches reality, so it has no problem with any of these typical realistic hook ups.? The model I created does this very well.
|
Re: Need triangular wave with using PWL mode
Hello See Triangular_Pulse_Wave.zip on
| | | | Yahoo! Groups offers free mailing lists, photo & file sharing, group calendars and more. Discuss hot topics, share interests, join online communities. | | | | Preview by Yahoo | | | ?Regards PhB
|
Re: Need triangular wave with using PWL mode
Kevin replied:
? ? "? PULSE(-6 6 0 5m 5m 1p 10m)" That is how I'd do it too. ?Except that I probably would have used 0 rather than 1ps, because the on-time Ton is allowed to be zero. ?The waveform is indeed piecewise linear.
But if Mete insists on using an actual PWL source, you could?have?this: ? ?PWL (0ms -6v 5ms 6v 10ms -6v 15ms 6v 20ms -6v 25ms 6v 30ms -6v) but you need to keep adding points to last the full simulation. ?Or do this, using LTspice's undocumented "repeat forever" syntax:
? ?PWL REPEAT FOREVER (0ms -6v 5ms 6v 10ms -6v) ENDREPEAT Regards, Andy
|
Re: Need triangular wave with using PWL mode
PULSE(-6 6 0 5m 5m 1p 10m)
...kevin On Wednesday, May 21, 2014 4:42 PM, "mete.90@... [LTspice]" wrote:
?
Hello guys,
I tried so hard but i can't do that. Can anyone send me PWL code of -6 to 6V 100Hz trianglular wave.
Thanks a lot. Regards, Mete
|
Need triangular wave with using PWL mode
Hello guys,
I tried so hard but i can't do that. Can anyone send me PWL code of -6 to 6V 100Hz trianglular wave.
Thanks a lot. Regards, Mete
|
Hello Sven,
After you have decided which plot(s) is the best, you can plot only one or a few of them using the @ selector.
V(out)@12
V(out)@23
Best regards,
Helmut
|
Hi John,
I want to analyze just one signal point in 27 variations. Just to understand which influence have my 3 potentiometer in 3 different positions.
Helmut's way works great. Even if I only have 4 or 5 curves, LTSpice does not tell me which curve is which.
On the .tr directive it gives you the name and color.
On the .ac directive it does not.
Thanks for the help anyway.
Sven
|
Thanks Helmut,
works great.
Sven
|
In message <llj28q+1ji2evs@...>, dated Wed, 21 May 2014, "helmutsennewald@... [LTspice]" <LTspice@...> writes: 1. Attach a cursor to e.g. V(out).
2. Use the up/down arrow key of he keyboard to jump to the waveform you are interested.
3. Move the mouse cursor near the waveform-crosshair. The mouse cursor will then change to 1, if it's the first of the two possible cursors. Now right mouse click.
LTspice will then report: Cursor 1: a=... b=... c=... (Run 7/15) Not quite as difficult as I thought, but with 27 curves it must need steady hand with the mouse. -- OOO - Own Opinions Only. With best wishes. See www.jmwa.demon.co.uk Nondum ex silvis sumus John Woodgate, J M Woodgate and Associates, Rayleigh, Essex UK
|
Hello,
Copy the file LM6172.MOD into the folder of your schematic.
Place an opamp2 from [Opamps] in your schematic.
Change the text opamp2 to LM6172/NS .
Include the model file with the SPICE-directive below.
.inc LM6172.MOD
Never place your schematics in the path C:\Program .... You will not have enough rights in this system path.
Best regards,
Helmut
|
