Keyboard Shortcuts
Likes
- LTspice
- Messages
Search
|
Re: Pull-Push transformer for valve amp in LTspice
pha0001?asked: ? ?"why did you take a quarter of the total primary inductance? Why not just half it?"
Adding to what Vlad already wrote (which should lead you to your answer), it does depend on the amount of coupling between inductors. ?You used a coupling coefficient of 1.
If the inductors had been uncoupled (K=0), then it would have been correct to use half.
Regards,
Andy |
|
Re: Pull-Push transformer for valve amp in LTspice
What's the equality between the ratios of the inductances and the number of turns? Vlad ______________________ -- holding, among others: a universal analog/digital filter, block-level models for power electronics (and not only), math blocks with a more stream-lined approach, some digital ADC, DAC, (synchronous-)counter, JKflop, etc. On Fri, May 23, 2014 at 4:15 PM, pha0001@... [LTspice] <LTspice@...> wrote:
> > ? > > Thank you so much!!! Things are starting to become much clearer now. > > > If you don't mind, may I ask, why did you take a quarter of the total primary inductance? Why not just half it? |
|
Re: Lock horizontal axis
Hi Helmut
It's really the X-axis I'm having problems with - see "X-Axis different scales" in Temp. ?? Top: Initial plot ?? Middle: Set precise manual limits on time range ?? Lower: Only one plot pane is "time-zoomed". Whilst this can be useful, I'd also like to be able to zoom all plots simultaneusly - all plots get same time range. Regards Stephen. |
|
Simulating a TI DRV103 with LTspice?
Walking Through
I was looking for an electronic "dash pot" for a solenoid and found the TI DRV10{2, 3} series of delayed-start PWM devices.? Downloaded TI's DRV103 spice file, looked, did a few sort-of educated guesses, and tried to simulate it with Cd=10 nF, R(osc) = 523K, and R(duty_cycle) = 40.2K.
Thought something was "not quite right" when LTspice kept flipping in and out of DefCon. Anyone worked with this device before?? Is there something in Linear Tech's collection that might be usable as a delayed-start PWM solenoid driver? Thanks. Mark |
|
(No subject)
Sam Jesse
I also tried .meas ampx MAX V(Out_1) I(V1) thinking I can plot the max of V(Out_1) vs. I(V1).meas ampx MIN I(V1) On Fri, May 23, 2014 at 7:35 AM, Sam Jesse <revrvr@...> wrote:
|
|
(No subject)
Sam Jesse
Helmut Is there a way to optimize on 2 or 3 variables and plot results like you did? i.e. Ton Tperiod R of the inductor for example?? On Fri, May 23, 2014 at 7:07 AM, helmutsennewald@... [LTspice] <LTspice@...> wrote:
|
|
(No subject)
Sam Jesse
Helmut Thank you. That is really good.On Fri, May 23, 2014 at 4:34 AM, helmutsennewald@... [LTspice] <LTspice@...> wrote:
|
|
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 |
|
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. |
|
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! |