LTSpice 'annoyances'???

Discussion in 'General Electronics Chat' started by Hypatia's Protege, May 20, 2015.

  1. Hypatia's Protege

    Thread Starter Distinguished Member

    Mar 1, 2015
    Owing to its popularity with students and electronics enthusiasts I am making a study of LTspice both for my own edification and to position myself to better assist participants on this and similar sites/lists...

    Approaching LTspice, as I am, from an essentially 'OrCAD EE PSpice' background, I find myself 'navigating' the proverbial 'learning curve' in certain areas... Please do not perceive the following as a litany of complaints!!! In point of fact I am (pleasantly) surprised at LTspice's power and flexibility -- in any regard -- but especially as a gratis product! Moreover the veritable ubiquity of LTspice component models greatly enhances this already highly attractive platform!:)

    The intent of this post is to verify bugs where present and learn the error of my ways where such is the case:cool::) --- Again, this is in no way a 'put down' of LTspice!!! Trust me! OrCAD has more than a few 'proclivities' of its own!:mad::D

    So, here it goes...

    RE: LTspice:

    1) Transformers (i.e. inductors related via the mutual inductance "K" directive) do not simulate properly in the absence of inter-winding ohmic 'continuity'...

    Example: The EMF plot of the 'hot' end of a grounded 'secondary' winding will be (wildly) erroneous or return a 'Singular Matrix' error, 'Floating Node' warning, etc... Unless the 'primary' is grounded (or otherwise ohmicly connected to the secondary)... As a side note, while reference to 'singular matrices' grants (welcome) insight into the modeling algorithm, it, sadly, throws little 'light' upon this aparent 'bug'...

    2) MOSFETs do not 'simulate' well from threshold up to (but non-inclusive of) saturation --- Moreover subthreshold slope simulation is hopeless...

    3) Apart from Zeners, the simulator does not support reverse breakdown characteristics...

    4) Please advise me as to the native (or 'accepted') method of defining/modling inductor 'saturation'

    Many advance thanks for any and all info, feedback and/or advice!:):):)

    Best Regards
  2. MikeML

    AAC Fanatic!

    Oct 2, 2009
    1. General rule. Every electrical node must have an Ohmic path to node zero (Gnd). Not specific to LTSpice. I first ran into this with Berkley spice. Work around: put a 1G resistor from the floating side of the transformer to Gnd.

    2. Mosfet models define those behaviors. Get better models. LTSpice is tuned for power mosfets, where sub-threshold behaviour max-nix. Pay for HSpice if you want to do sub micron IC design...

    3. No Spice engine does. You have to create more complex sub-circuit library models rather than using the parameterized in-built components.

    4. This can be done using the rich behavioral models in LTSpice, but I am no expert. I would google this question...
    Here is one example found that way
    Hypatia's Protege and cmartinez like this.
  3. Alec_t

    AAC Fanatic!

    Sep 17, 2013
    Have you read the LTS 'Help' about non-linear inductor modelling?
    Hypatia's Protege likes this.
  4. Hypatia's Protege

    Thread Starter Distinguished Member

    Mar 1, 2015
    Thank you! Pleased to learn 'tis merely 'the nature of the beast' as it were!:) --- I find it surprising that Linear Technology, having, as they seem to, 'power-conversion' as their stock-and-trade, would fail to provide direct implementation of so central an element as the magnetic transformer? I must assume similar caveats apply to (ideal) electrostatic and piezoelectric components? --- Anyway, the important point is that the 'quirk', once acknowledged, may, as you point out, be readily worked around:D

    While I can 'survive' sans faculty of sub-threshold simulation, I feel that simulation of 'tantric region' (i.e. Egs[th]<=Egs[applied]<Egs[sat]) operation (inclusive of power devices) is essential --- As an example of a practical application of said mode please see the document linked below - In Figure 1 you will observe an IRLR024 employed as an analog current control in a feed-back regulation scheme -- Please note that the IRLR024, excepting its rather low Egs[th] figure, is in no way a 'special' device... Here's the link: --- Hope that 'makes my point' I searched far and wide for that!:D --- As per your advice I will look for more accurate models, there seems to be a lot of LTspice 'stuff' out there!:D

    Thanks, It's becoming clear that desirable program performance will require attainment of model creation skills --- Even so, it seems specified characteristics (at least) should be supported (WAH!!!) :(;):D
    Actually a study of 'model programming' will be something like 'fun' especially as I have access to a large variety of characterization instruments/systems... :)

    I will check into these resources forthwith!:D

    With many sincere thanks for the replies and info!:D:D:D

    Best regards
    Last edited: May 20, 2015
  5. MikeML

    AAC Fanatic!

    Oct 2, 2009
    Hypatia's Protege likes this.
  6. Bordodynov

    Well-Known Member

    May 20, 2015
    I will return to the first question. I apologize for the delay in my response.
    I would like to respond immediately,
    but registration for the forum to take time.
    I will show that LTspice even better than you thought.


    1. Also behave practically all spice-program.
    My advice, put on the circuit following:
    .option gshunt=1f cshunt=1f .

    2. Also behave practically all spice-program.
    Use model MOS-transistor level 2.

    Model vdmos has Ksubthres,Mtriode,Theta,Lambda.
    .model BSC050NE2LS VDMOS(Rg=.65 Vto=2.25 Rd=1.95m Rs=500u Rb=2.46m Kp=157.5
    + Ksubthres=.1 Mtriode=1.5 Theta=.3 Lambda=.05 Cgdmin=13p Cgdmax=.24n A=.6 Cgs=.72n

    3. MOS-transistors vdmos have a breakdown voltage (BV,ibv,nbv).

    Bipolar transistors have a breakdown voltage (BVcbo,nBVcbo,BVbe,Ibvbe,nbvbe).
    It also has options for the area quasisaturated (Gamma,Qco,Rco).

    Diodess have a breakdown voltage:

    .MODEL PLVA650A D IS=535.74E-18 N=1.0029 RS=.29276 IKF=2.505 CJO=119.42p M=.32565
    + VJ=.62169 ISR=216.91n NR=4.995 BV=5. NBV=2. nbvl=5 ibvl=5u IBV=0.25m TT=132.15n mfg=NXP type=zener

    .model C3D10170H d is=1e-17 n=1 bv=2200 ibv=500u nbv=100 ibvL=10u nbvL={5k*(1+10m*(temp-27))}
    + Tbv1=-20u Tbv2=-5u Rs=0.1 Trs1=8.5m Trs2=14u TT=0.1n Cjo=830p Vj=2.5 m=0.5
    + Iave=14.4A Vpk=1700V mfg=Cree type=Schottky

    .model C3D10170H_simplest d Ron={0.053+Temp*1.1m} Roff=340Meg Vfwd={0.975-Temp*1.4m}
    + Vrev=1700 Rrev=1k Iave=14.4A Vpk=1700V mfg=Cree type=Schottky

    4.The model of the magnetic core by Chan has parameters Bs, Br and Hc.
    Saturation flux density is usually determined in practice.
    Take the value of a sufficiently large value Hc (for example at 800A/m or 2000A/m).
    The error in this case is small.

    For training see website
    I learned from him a lot.
    Hypatia's Protege likes this.
  7. Hypatia's Protege

    Thread Starter Distinguished Member

    Mar 1, 2015
    Many thanks for the helpful information! -- I greatly appreciate the time and effort you took on my behalf! :):):)

    Very best regards