Author Topic: How to Use Vishay's MOSFET models in LTSPICE  (Read 1185 times)

0 Members and 2 Guests are viewing this topic.

Offline palpurul

  • Regular Contributor
  • *
  • Posts: 87
  • Country: tr
  • Hey
How to Use Vishay's MOSFET models in LTSPICE
« on: October 15, 2021, 07:58:54 pm »
Hello,
I am trying to simulate a MOSFET(SISS10ADN) that I picked from Vishay. I'd like to incorporate them into my design , but I want to simulate them first in LTSPICE. Vishay gives me a bunch of models (I think) that can't really simulate in LTSPICE.


When I try to run it, LTSPICE gives me this:

Error on line 13 : r:u1:1 +12v«:d» u1:3 1.700e-03 3.725e-03 1.827e-05
    Unknown parameter "1.827e-05"
Error on line 17 : r:u1:tcv u1:100 n001«:s» 1e6 1.266e-04 1.174e-06
    Unknown parameter "1.174e-06"
Error on line 24 : .model u1:dbd d ( fc = 0.1 tt = 3.088e-08 tref = 25 bv = 41 rs = 1.115e-02 n = 9.388e-01 is = 1.078e-13 eg = 1.495e+00 xti = -9.765e+00 trs = 3.626e-03 cjo = 2.702e-10 vj = 8.119e+00 m = 1.000e+00 )
   * Unrecognized parameter "trs" -- ignored
Error on line 23 : .model u1:pmos pmos ( level = 3 tox = 5e-8 nsub = 3.967e+16 is = 0 tpg = -1 capop = 12 )
   * Unrecognized parameter "capop" -- ignored
Error on line 22 : .model u1:nmos nmos ( level = 3 tox = 5e-8  rs = 0 kp = 9.844e-06 nsub = 5.390e+16  kappa = 1.073e-01 nfs = 1.009e+11  ld = 0 is = 0 tpg = 1 capop = 12 )
   * Unrecognized parameter "capop" -- ignored
WARNING: Node N004 is floating.
WARNING: Node N003 is floating.

WARNING: Less than two connections to node N004.  This node is used by C1.
WARNING: Less than two connections to node N003.  This node is used by C1.
Instance "m:u1:2": Length shorter than recommended for a level 3 MOSFET.
Instance "m:u1:1": Length shorter than recommended for a level 3 MOSFET.
Direct Newton iteration for .op point succeeded.
Singular matrix:  Check node n004
   Iteration No. 1
Fatal Error: Singular matrix:  check node n004
   Iteration No. 1

This circuit has floating nodes.


I tried all of the models in the folder that I downloaded from Vishay's website, but they all give similar errors. Can they work in LTSPICE at all?

Link to MOSFET models: https://www.vishay.com/product?docid=79237&tab=designtools-ppg
 

Offline T3sl4co1l

  • Super Contributor
  • ***
  • Posts: 18471
  • Country: us
  • Expert, Analog Electronics, PCB Layout, EMC
    • Seven Transistor Labs
Re: How to Use Vishay's MOSFET models in LTSPICE
« Reply #1 on: October 15, 2021, 09:26:36 pm »
Change the resistor second parameter from comma-separated to "TC2=".

PSPICE is weird.

Similarly, you'll have to find equivalent for the extra device parameters, or maybe it works okay without them.

Or no wait, HSPICE actually?  Yeesh, a bit of an adventure to find what document I'm looking for.  It's in here:
http://www2.ece.rochester.edu/courses/ECE222/hspice/hspice_mosfet.pdf
Doesn't sound very unusual, CAPOP = 12 "Ward Dutton model" something or other, which seems to be an old method (published in the 70s), would that not be a normal model integrated with plain-vanilla SPICE then?  No idea.

And TRS is just a tempco for RS, if nothing else, the diode can set RS = 0 and then implement it separately (a resistor of R = RS and TC1 = TRS in series).

Tim
« Last Edit: October 15, 2021, 09:39:49 pm by T3sl4co1l »
Seven Transistor Labs, LLC
Electronic design, from concept to prototype.
Bringing a project to life?  Send me a message!
 
The following users thanked this post: palpurul

Offline palpurul

  • Regular Contributor
  • *
  • Posts: 87
  • Country: tr
  • Hey
Re: How to Use Vishay's MOSFET models in LTSPICE
« Reply #2 on: October 16, 2021, 05:52:44 am »
 
Change the resistor second parameter from comma-separated to "TC2=".

PSPICE is weird.

Similarly, you'll have to find equivalent for the extra device parameters, or maybe it works okay without them.

Or no wait, HSPICE actually?  Yeesh, a bit of an adventure to find what document I'm looking for.  It's in here:
http://www2.ece.rochester.edu/courses/ECE222/hspice/hspice_mosfet.pdf
Doesn't sound very unusual, CAPOP = 12 "Ward Dutton model" something or other, which seems to be an old method (published in the 70s), would that not be a normal model integrated with plain-vanilla SPICE then?  No idea.

And TRS is just a tempco for RS, if nothing else, the diode can set RS = 0 and then implement it separately (a resistor of R = RS and TC1 = TRS in series).

Tim

Thank you I just omitted that line and it worked.
Now I have to make this model work.
Model: https://www.diodes.com/part/view/DGD05473?BackID=8231#tab-details

I renamed the extenstion as .cir and when I try to run it in LTSpice it gives me this error:
Fatal Error: Undefined subcircuit: :

How to make this one work?

Thank you so much

 

Offline T3sl4co1l

  • Super Contributor
  • ***
  • Posts: 18471
  • Country: us
  • Expert, Analog Electronics, PCB Layout, EMC
    • Seven Transistor Labs
Re: How to Use Vishay's MOSFET models in LTSPICE
« Reply #3 on: October 16, 2021, 08:11:42 am »
Eeeeh yikes, all those switches... you're probably better off using an E source and/or logic gates to fake it.  SPICE doesn't like lots of abrupt characteristics like switches.

Probably the syntactic thing LT is choking on is the nested SUBCKT.  Move the gen_switch block to the bottom (below the outer .ENDS).

Dunno about those pinnames things either. And colons in the param list?

Tim
Seven Transistor Labs, LLC
Electronic design, from concept to prototype.
Bringing a project to life?  Send me a message!
 
The following users thanked this post: palpurul

Offline palpurul

  • Regular Contributor
  • *
  • Posts: 87
  • Country: tr
  • Hey
Re: How to Use Vishay's MOSFET models in LTSPICE
« Reply #4 on: October 16, 2021, 08:47:30 am »
Eeeeh yikes, all those switches... you're probably better off using an E source and/or logic gates to fake it.  SPICE doesn't like lots of abrupt characteristics like switches.

Probably the syntactic thing LT is choking on is the nested SUBCKT.  Move the gen_switch block to the bottom (below the outer .ENDS).

Dunno about those pinnames things either. And colons in the param list?

Tim

Thank you so much for your response.
I am getting into switching converter design and I decided to simulate them first. I really don't know if I have to use generic switch models or vendor supplied models. Eventually I'd like to simulate the loop and get the frequency response to monitor stability. Obviously I can't get the frequency response with those models (or can I?).
Do you have suggestion about this? Should I use average models or vendor supplied models to simulate switching converter circuits (both transient and AC response).
Thanks again you helped me a lot.
 

Offline T3sl4co1l

  • Super Contributor
  • ***
  • Posts: 18471
  • Country: us
  • Expert, Analog Electronics, PCB Layout, EMC
    • Seven Transistor Labs
Re: How to Use Vishay's MOSFET models in LTSPICE
« Reply #5 on: October 16, 2021, 11:11:13 am »
The gate driver doesn't do much for you in simulation, it's a propagation delay and that's about it; the particulars about UVLO, input threshold, output level, etc. shouldn't be too important.  It's quite possible that's about all they're simulating in that model anyway, it doesn't look too involved.

Using a plain E source has no delay, but if delay is a small fraction of your overall loop phase margin (and, I would hope it is?), it won't have much impact; and you can simply avoid testing the other aspects as part of control loop modeling.

A part of modeling is wanting to build something as comprehensive as possible, for example so you can build the circuit, do all your simulations in one place with the complete model, then build it from exactly the same place.  Well, you don't have that last luxury, as LTSpice isn't PCB design software, but to the extent you can import the schematic in something else, or at least the netlist, there would be that.

But a more refined level of modeling, or perhaps a substitute depending on particular goals of a given project -- or a necessity above a certain scale -- it can be broken up into smaller pieces.  This may not be too important for a converter, which you can easily model whole; but if you're having trouble putting together the whole thing, you might still slice it up different ways.  Namely: the inverter by itself, doesn't need to be tested in a closed loop; you can wire up a few VPULSEs for gate drive, with a dummy load, resistor or inductor or some combination like that, to get representative load current going.  That's good for testing switching loop dynamics (rise/fall, ringing, overshoot).  Conversely, the control loop doesn't care a smidge about the rise/fall/ringing, the inverter can basically be a single switch for all that matters, or even a dependent source.

There's also such a thing as an average mode model, which does away with the switching, and models the control loop very well; ripple can even be added back in; at least, potentially so.  (However, to do this automatically, as it were, you'll need support from the sim engine itself, i.e. periodic steady state (PSS) analysis -- ngspice for example includes this.)

Tim
Seven Transistor Labs, LLC
Electronic design, from concept to prototype.
Bringing a project to life?  Send me a message!
 

Offline 3roomlab

  • Frequent Contributor
  • **
  • Posts: 835
  • Country: 00
  • kT kT kT kT kT kT kT kT kT
Re: How to Use Vishay's MOSFET models in LTSPICE
« Reply #6 on: October 16, 2021, 01:55:58 pm »
seem to work fine. SiSS10ADN_PS.LIB
the law of conservation dont work on humans, you eat a kg of food but you appear to grow 2kg of fat 
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf