1. Home
  2. Electronics Design
  3. Is there something wrong with PMOS model in the LTSpice XVII?
  4. Page 2

Is there something wrong with PMOS model in the LTSpice XVII?

This is a very interesting circuit. Thanks for posting.

Please ignore Larkin's claims of lockup. He FUD's any circuit he did not make himself. There is no lockup. The circuit has only two stable states: M1 is on, or M1 is off. This is abundantly clear from the schematic.

I made some corrections:

  1. Except in rare cases, never use default components. Always select some realistic component for that location.

  1. Always name every node. If you do not, then when you add a component during development, all the node numbers change. Good luck trying to find what you were measuring before.

  2. Never connect to the stub of a component. When you do, and you try to move it, you will get slanted wire connections.

  1. Always define the Max Timestep in .TRAN analysis. You can start with Max Time / 1,000 and increase or decrease as desired.

  2. Always check to see you are in Modified Trap mode. Gear and Trap may give erroneous results. To check, follow

Control Panel -> SPICE -> Default Integration Method: modified trap

For more information, see

SPICE Differentiation, by Mike Engelhardt

formatting link

With these changes, the circuit starts immediately. You do not have to run 300ms to see the oscillations begin. This wastes time. 5ms is sufficient to see the startup and break into oscillations.

The modified circuit is at

formatting link

If your server doesn't like the url, you can try

formatting link

Reply to
Steve Wilson
Loading thread data ...

I forgot some very important suggestions:

  1. Always add realistic values to capacitors and inductors. The default series resistance for capacitors is zero ohms and zero series inductance. This never occurs in real life and can greatly affect the results.

  1. The default series resistance for inductors is 1 milliohm. This is not realistic in most cases.

Also, the default parallel capacitance is zero. This can cause problems in switching circuits where fast edges cause high speed damped oscillations.

  1. SPICE can slow down trying to follow these edges and make the analysis too slow to be useful. This can be a real problem in transformer-coupled circuits that feed fast schottky diodes. Add realistic component values, and add snubber circuits where needed to speed the analysis and give realistic results.

  1. Some schottky diode models can give very slow .TRAN results in PWM circuits. Try another diode, or use the default diode model.

Reply to
Steve Wilson

And set Solver = Alternate to ensure accurate results. ...Jim Thompson

--
| James E.Thompson                                 |    mens     | 
| Analog Innovations                               |     et      | 
| Analog/Mixed-Signal ASIC's and Discrete Systems  |    manus    | 
| STV, Queen Creek, AZ 85142    Skype: skypeanalog |             | 
| Voice:(480)460-2350  Fax: Available upon request |  Brass Rat  | 
| E-mail Icon at http://www.analog-innovations.com |    1962     | 

             I'm looking for work... see my website. 

          Thinking outside the box... elegant solutions.
Reply to
Jim Thompson

Exactly. M1 on is a stable state. Until something melts.

Actually, when I run it in LT Spice, it is stable, no oscillation. If you play with diode drops and Spice settings, you can probably get it to oscillate.

I don't trash any circuit that's not mine. But most posted and published circuits are bad.

I don't criticize Phil's stuff, because he knows what he's doing. Besides, he's bigger than me.

If you have to fiddle with Spice settings to get a circuit to oscillate, how can you be sure it will oscillate in real life?

How do you know what "erroneous results" are?

--

John Larkin         Highland Technology, Inc 

lunatic fringe electronics
Reply to
John Larkin
[snip]

The default settings in LTspice are designed to emphasize _speed_.

Go to an LTspice seminar and see what Mikey brags about.

Only an amateur at Spice doesn't understand the significance of MaxTimeStep. ...Jim Thompson

-- | James E.Thompson | mens | | Analog Innovations | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | STV, Queen Creek, AZ 85142 Skype: skypeanalog | | | Voice:(480)460-2350 Fax: Available upon request | Brass Rat | | E-mail Icon at

formatting link
| 1962 |

I'm looking for work... see my website.

Thinking outside the box... elegant solutions.

Reply to
Jim Thompson

The default time step in LT Spice can cause pretty big errors, or prevent convergence.

But fiddling with Spice settings (or diode drops) until a circuit makes you happy, may not make the production people happy.

--

John Larkin         Highland Technology, Inc 

lunatic fringe electronics
Reply to
John Larkin

If you give the circuit a small kick, you can reliably tell if it will star t oscillating from noise. The only condition is that the kick has to be a s mall perturbation on the DC quiescent bias, but larger than the SPICE toler ance settings. Since the buildup is exponential, it doesn't take long.

And the Gear integrator is helpful with stiff systems (ones with widely dif fering eigenvalues), which otherwise require very small time steps. It does have drawbacks, e.g. it can mask oscillations.

Cheers

Phil Hobbs

Reply to
pcdhobbs

I was thinking about nonlinear circuits, ones that may not start or ones that might lock up in some horrible state.

In real life, things like power supply rampup rates, or brownouts, can do nasty things. My point was that a pleasing Spice run, especially if fiddled and forced, doesn't mean you can manufacture a zillion of them.

The problem then is, how can you trust Spice? I think the answer is that you can't.

--

John Larkin         Highland Technology, Inc 

lunatic fringe electronics
Reply to
John Larkin

Agreed. For a start, very few IC models are good enough to be more than vag ue indicators of how real circuits behave. Op amp macromodels are especiall y bad. Discrete models are generally better, except that the SPICE diode is garbage, and the MESFET one is no better.

Good luck getting SPICE to predict the gate bias of a pHEMT floating negati ve, but it does.

*gasp*....maybe _design_ is required? Or even _measurements_? Horrors!

;)

Cheers

Phil Hobbs

Reply to
pcdhobbs

I don't fiddle, I set LTspice "defaults" to the same as PSpice... and PSpice _always_ matches the big expensive guys' simulations. ...Jim Thompson

--
| James E.Thompson                                 |    mens     | 
| Analog Innovations                               |     et      | 
| Analog/Mixed-Signal ASIC's and Discrete Systems  |    manus    | 
| STV, Queen Creek, AZ 85142    Skype: skypeanalog |             | 
| Voice:(480)460-2350  Fax: Available upon request |  Brass Rat  | 
| E-mail Icon at http://www.analog-innovations.com |    1962     | 

             I'm looking for work... see my website. 

          Thinking outside the box... elegant solutions.
Reply to
Jim Thompson

Thou speaketh of LTspice "hokey" models (*)... real Spice diode models are generally quite good, likewise FET's.

And the foundry models I work with are excellent.

The default "break-out" MOSFET model in LTspice doesn't even have a settable VTH parameter. ...Jim Thompson

--
| James E.Thompson                                 |    mens     | 
| Analog Innovations                               |     et      | 
| Analog/Mixed-Signal ASIC's and Discrete Systems  |    manus    | 
| STV, Queen Creek, AZ 85142    Skype: skypeanalog |             | 
| Voice:(480)460-2350  Fax: Available upon request |  Brass Rat  | 
| E-mail Icon at http://www.analog-innovations.com |    1962     | 

             I'm looking for work... see my website. 

          Thinking outside the box... elegant solutions.
Reply to
Jim Thompson

Dunno. Do your diode models accurately predict 1-2V overshoot in V_F due to diffusion delays? That's the main problem with LTspice's.

Probably so, at least in use cases they've thought about, because foundries

I'd be very impressed if SPICE were able to predict the Broadcom pHEMTs spo ntaneously biasing their own gates negative when left open-circuited.

Cheers

Phil Hobbs

Reply to
pcdhobbs

The main problem with LTspice's diode models is that they are idealized.

Yep.

To impress you all that would be required is that the pHEMT's manufacturer produce an accurate Spice model.

There's generally nothing wrong with Spice... whatever the flavor... IF the model is good. ...Jim Thompson

--
| James E.Thompson                                 |    mens     | 
| Analog Innovations                               |     et      | 
| Analog/Mixed-Signal ASIC's and Discrete Systems  |    manus    | 
| STV, Queen Creek, AZ 85142    Skype: skypeanalog |             | 
| Voice:(480)460-2350  Fax: Available upon request |  Brass Rat  | 
| E-mail Icon at http://www.analog-innovations.com |    1962     | 

             I'm looking for work... see my website. 

          Thinking outside the box... elegant solutions.
Reply to
Jim Thompson

There are two issues, I think. The first is (as you say) that the mfg needs to make good models if possible.

The second is more of a SPICE limitation: the D() facility doesn't include diffusion delays, which makes it intrinsically incapable of accounting for V_F overshoot, and the MESFET facility doesn't model real device behaviour such as the aforementioned self-biasing of pHEMTs.

The one is a modelling issue, but the second is an intrinsic limitation of the simulator.

This is not to say that it can't be patched up, just that after N years we' re still waiting. (Other more expensive tools may be better, of course.)

Cheers

Phil Hobbs

Reply to
pcdhobbs

(1) Nonsense. It's quite feasible to write such a MODEL.

(2) Nonsense. Refer to (1) above.

I have multiple papers on diffusion and recovery... the problem is they're all by PhD's... clueless about how to really model >:-} ...Jim Thompson

--
| James E.Thompson                                 |    mens     | 
| Analog Innovations                               |     et      | 
| Analog/Mixed-Signal ASIC's and Discrete Systems  |    manus    | 
| STV, Queen Creek, AZ 85142    Skype: skypeanalog |             | 
| Voice:(480)460-2350  Fax: Available upon request |  Brass Rat  | 
| E-mail Icon at http://www.analog-innovations.com |    1962     | 

             I'm looking for work... see my website. 

          Thinking outside the box... elegant solutions.
Reply to
Jim Thompson

That's rare for RF parts. You're lucky to get any DC specs. All you usually get is s-params, which don't help much if you want to use them in switching apps. The noise data is at high freqs, often just a microwave band, with no hint of low frequency behavior. Leakage currents? C-V curves? Substrate diode effects? As if!

Even the rare Spice model is sketchy.

Depletion parts typically enhance nicely, but there's usually no suggestion of that on data sheets. So we test them.

--

John Larkin         Highland Technology, Inc 

lunatic fringe electronics
Reply to
John Larkin

So? Take data and write your own model. ...Jim Thompson

--
| James E.Thompson                                 |    mens     | 
| Analog Innovations                               |     et      | 
| Analog/Mixed-Signal ASIC's and Discrete Systems  |    manus    | 
| STV, Queen Creek, AZ 85142    Skype: skypeanalog |             | 
| Voice:(480)460-2350  Fax: Available upon request |  Brass Rat  | 
| E-mail Icon at http://www.analog-innovations.com |    1962     | 

             I'm looking for work... see my website. 

          Thinking outside the box... elegant solutions.
Reply to
Jim Thompson

We usually take data and design circuits! With this picosecond stuff, breadboarding is better than simulating anyhow.

formatting link 

--

John Larkin         Highland Technology, Inc 

lunatic fringe electronics
Reply to
John Larkin

MTs.

I've asked about SPICE modelling the forward overshoot of diodes both here and in the Yahoo LTspice group, and heard in both places that the SPICE D() facility is too stupid to model it. If you can produce a model for a 1N414

8 that overshoots to 1.4 V or so on turn-on (about par for a real unit), an d exhibits the same variation with dI/dt as a real one, I'll happily conced e your point.

It won't be using just D(), though, that's for sure.

the simulator.

SPICE is a pretty capable solver for largish sparse systems of nonlinear OD

Reply to
pcdhobbs

DEs. Transient carrier diffusion is governed by a transport equation, thoug h, which exhibits intrinsically more complex and nonlocal behaviour. That h as to be put in by hand, like transmission line devices, which are also non local and don't follow any ODE.

So there are actually lots of things you can't do in SPICE without hacking the actual simulator code.

Cheers

Phil Hobbs

Reply to
pcdhobbs

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.