General Ltspice question

Thread Starter

Aleph(0)

Joined Mar 14, 2015
597
So I'm confused abt why default Ltspice components (like diodes and mosfets) most often don't work at all but commercial components selected from list of "pick another component" always work even way outside of their specifications? Ok so I know LTspice doesn't usually enforce max stress characteristics but only default components need strict adherence to specs for any chance of working:confused:! So if anyone understands this plz share:cool: Thanks:)!
 

Bordodynov

Joined May 20, 2015
2,801
default Ltspice components
.MODEL ideald D ( IS =1e-14 RS =0 CJO=0 VJ=1 TT=0 M=0.5 BV=1e+30 N=1 EG=1.11 XTI=3 KF=0 AF=1 FC=0.5 IBV =0.001 TNOM=27)
LTspice not like CJO=0. --> CJO=10f xor Alternate.
.MODEL idealnmos NMOS (
+ VTO=0 KP = 2e-05 LAMBDA= 0 PHI = 0.6 GAMMA = 0 RD = 0 RS = 0 IS = 1e-14 CGBO = 0 CGDO = 0 CGSO = 0 CBD = 0 CBS = 0 PB = 0.8 RSH = 0 CJ = 0 MJ = 0.5 CJSW = 0 MJSW = 0.5 JS = 0 TOX = 1e-07 NSUB = 0 NSS = 0 TPG = 1 LD = 0 U0 = 600 KF = 0 AF = 1 FC = 0.5 TNOM = 27
it is bad VTO=0 and LAMBDA=0 ---> VTO=0.8 and LAMBDA=1m
 

crutschow

Joined Mar 14, 2008
26,735
Default LTspice components seem to have some unusual properties in certain applications, so I always select a commercial device that's close to what I would use in the real circuit.
Otherwise you may end up with a circuit that operates differently than it ever would in the real world.
 

ci139

Joined Jul 11, 2016
1,696
. . . commercial components selected from list of "pick another component" always work even way outside of their specifications . . .
is quite intuitive to grasp - as they are models of the real devices - the least of which consist from billions of atoms and pass through real electric charge carriers - that in turn apply to laws of electro- and thermodynamics and quantum physics - the more simple processes of which do fall to close correlation with the appropriate statistical descriptions by the main observed (not all) physical parameters . . . blah, blaah . . .

. . . in other words - the current IT proccessing power won't enable a real time realistic simulation - thus the simulator handles even lesser than the (not all) physical parameters and like computer games attempts to cheat through complex situations - all this for the user to not to turn gray and drop dead before the simulation finishes

(((( though you can always add programmed resistors to circuit and dynamically monitor some component power and extra simulate thermal effects and component burn out . . .
. . . which makes you LT simulation 10-s of times slower (due non-optimized extra code) and more complex to pass through the fast voltage and current changes ((( because the cheats ((estimation of ( / simplification to ) the most likely system state after certain delta-time or/and transitions )) can't pass - because your code requires proccessing all of the cosequential time-steps ))) ))))

so you have to monitor the realistic limits yourself
? which is good ? - so you can simply replace the low power/voltage device with higher P/U 1
 

Hypatia's Protege

Joined Mar 1, 2015
3,226
So I'm confused abt why default Ltspice components (like diodes and mosfets) most often don't work at all but commercial components selected from list of "pick another component" always work even way outside of their specifications? Ok so I know LTspice doesn't usually enforce max stress characteristics but only default components need strict adherence to specs for any chance of working:confused:! So if anyone understands this plz share:cool: Thanks:)!
Default LTspice components seem to have some unusual properties in certain applications, so I always select a commercial device that's close to what I would use in the real circuit.
Otherwise you may end up with a circuit that operates differently than it ever would in the real world.
Indeed! Such has been my experience as well:confused::rolleyes:

@Aleph(0) --- Further to study/investigation of said behaviour, please draft an example then 'up' the .asc file to this thread - from which I may post screen captures of simulations for the benefit of members w/o an Ltspice installation:)

Best regards
HP:)
 

Hypatia's Protege

Joined Mar 1, 2015
3,226
default Ltspice components
.MODEL ideald D ( IS =1e-14 RS =0 CJO=0 VJ=1 TT=0 M=0.5 BV=1e+30 N=1 EG=1.11 XTI=3 KF=0 AF=1 FC=0.5 IBV =0.001 TNOM=27)
LTspice not like CJO=0. --> CJO=10f xor Alternate.
.MODEL idealnmos NMOS (
+ VTO=0 KP = 2e-05 LAMBDA= 0 PHI = 0.6 GAMMA = 0 RD = 0 RS = 0 IS = 1e-14 CGBO = 0 CGDO = 0 CGSO = 0 CBD = 0 CBS = 0 PB = 0.8 RSH = 0 CJ = 0 MJ = 0.5 CJSW = 0 MJSW = 0.5 JS = 0 TOX = 1e-07 NSUB = 0 NSS = 0 TPG = 1 LD = 0 U0 = 600 KF = 0 AF = 1 FC = 0.5 TNOM = 27
it is bad VTO=0 and LAMBDA=0 ---> VTO=0.8 and LAMBDA=1m
is quite intuitive to grasp - as they are models of the real devices - the least of which consist from billions of atoms and pass through real electric charge carriers - that in turn apply to laws of electro- and thermodynamics and quantum physics - the more simple processes of which do fall to close correlation with the appropriate statistical descriptions by the main observed (not all) physical parameters . . . blah, blaah . . .

. . . in other words - the current IT proccessing power won't enable a real time realistic simulation - thus the simulator handles even lesser than the (not all) physical parameters and like computer games attempts to cheat through complex situations - all this for the user to not to turn gray and drop dead before the simulation finishes

(((( though you can always add programmed resistors to circuit and dynamically monitor some component power and extra simulate thermal effects and component burn out . . .
. . . which makes you LT simulation 10-s of times slower (due non-optimized extra code) and more complex to pass through the fast voltage and current changes ((( because the cheats ((estimation of ( / simplification to ) the most likely system state after certain delta-time or/and transitions )) can't pass - because your code requires proccessing all of the cosequential time-steps ))) ))))

so you have to monitor the realistic limits yourself
? which is good ? - so you can simply replace the low power/voltage device with higher P/U 1
Thanks Gents! - Hopefully @Aleph(0) will upload example{s} (as suggested in the previous post) where, by dint of study of same in light of your expertise, we (i.e. Aleph and I:oops:) may arrive at an intuitive grasp of the subject:cool:

Very best regards
HP:)
 
Last edited:

Thread Starter

Aleph(0)

Joined Mar 14, 2015
597
@Aleph(0) --- Further to study/investigation of said behaviour, please draft an example then 'up' the .asc file to this thread - from which I may post screen captures of simulations for the benefit of members w/o an Ltspice installation:)
HP I can try to do both but screen capture might be low rez:oops: Anyhow now that I set my vpn for Northern European servers my connection is much better so maybe whole file can upload before transfer bombs out:cool:

Thanks Gents!
Thanks from me too:D!

Plz check back after while:)
 

MrAl

Joined Jun 17, 2014
8,063
Hello there,

Sometimes components appear to be working when really they are not. That's because it depends what we call an "error". Should the simulator stop and state that there is an "error" if a diode voltage goes beyond it's reverse rating? It depends how you look it it. A diode operated in a real circuit where its voltage goes beyond its rating may just act like a zener for a while or short out, and that would give you a set of results that reflect that action. But if replaced with a new diode, the same thing will happen again. So it may be considered to be some sort of unusual operation, but it is still electrical operation.
Do resistors have a voltage rating in the simulator? I dont think i checked this either. If a voltage on a real resistor goes too high it might arc over once or many times. It's hard to model that. So some simulators may show a warning when a component rating has been exceeded while others wont show that, you have to check yourself from the simulation results. If you have a resistor rated for max 200v and the voltage goes up to 300v, you know you have to do something about it.

The short story is that simulators are not perfect, yet.
 

Standisher

Joined Jan 16, 2015
129
Mmmm...I have just started to try modelling in LTspice (must admit I haven't read the help/instructions yet) but was surprised that I didn't get any warning when I deliberately placed a 1/4W 60 Ohm resistor in a 12v path. I thought that defining a components parameters would enable the simulator to flag up a warning when running a simulation on a circuit where a component was under rated (the resistor is shown as dissipating 2.4W :)) ... or could it be that I'm not using LTspice properly?
 
Last edited:

OBW0549

Joined Mar 2, 2015
3,566
Mmmm...I have just started to try modelling in LTspice (must admit I haven't read the help/instructions yet) but was surprised that I didn't get any warning when I deliberately placed a 1/4W 60 Ohm resistor in a 12v path. I thought that defining a components parameters would enable the simulator to flag up a warning that the component was under rated (the resitor is shown as dissipating 2.4W :)) ... or could it be that I'm not using LTspice properly?
Spice will NOT warn you that you are over-stressing a component or otherwise using it inappropriately; that is simply not what it is for, so don't expect it to do that.

Spice computes the voltages and currents in a circuit, either in the time domain (.TRAN analysis) or in the frequency domain (.AC analysis), without making any judgement about whether those voltages or currents are OK.
 

Alec_t

Joined Sep 17, 2013
11,980
If you hover the mouse over a component and press the 'Alt' key you will see a thermometer icon pop up. Left click and you get a plot of the power dissipated in that component. That will enable you to decide if it is over-stressed :).
 

Standisher

Joined Jan 16, 2015
129
Spice will NOT warn you that you are over-stressing a component or otherwise using it inappropriately; that is simply not what it is for, so don't expect it to do that.

Spice computes the voltages and currents in a circuit, either in the time domain (.TRAN analysis) or in the frequency domain (.AC analysis), without making any judgement about whether those voltages or currents are OK.
Ah, OK thanks. It certainly does what it is specified to do just fine. I just thought as the tool also quotes dissipation figure for a component, it would be logical and relatively straight forward for the software to highlight that the specified component properties were inappropriate for the dissipation calculated. Wishful scope creep on my behalf i guess :oops:
 

Standisher

Joined Jan 16, 2015
129
If you hover the mouse over a component and press the 'Alt' key you will see a thermometer icon pop up. Left click and you get a plot of the power dissipated in that component. That will enable you to decide if it is over-stressed :).
Thanks for the tip Alec, that's good.
 

crutschow

Joined Mar 14, 2008
26,735
Ah, OK thanks. It certainly does what it is specified to do just fine. I just thought as the tool also quotes dissipation figure for a component, it would be logical and relatively straight forward for the software to highlight that the specified component properties were inappropriate for the dissipation calculated. Wishful scope creep on my behalf i guess :oops:
There actually was a Spice simulator system back in the 80's called Analog Workbench that would pop up a little symbol (I think something like a thermometer with a line through it) when a part was overstressed, but I think it's no longer available.
The difficulty is that for many parts, such as power transistors, the dissipation depends upon the heat-sink, which is not specified in the transistor model.
 

Standisher

Joined Jan 16, 2015
129
There actually was a Spice simulator system back in the 80's called Analog Workbench that would pop up a little symbol (I think something like a thermometer with a line through it) when a part was overstressed, but I think it's no longer available.
The difficulty is that for many parts, such as power transistors, the dissipation depends upon the heat-sink, which is not specified in the transistor model.
I see, that makes sense to me. Thank you
 

OBW0549

Joined Mar 2, 2015
3,566
I just thought as the tool also quotes dissipation figure for a component, it would be logical and relatively straight forward for the software to highlight that the specified component properties were inappropriate for the dissipation calculated.
To do that would open up a whole 'nuther can of worms. What is the maximum allowable junction temperature for that part? Which package is the component in, and what is its thermal resistance to ambient? Lots of semiconductor parts are available in multiple packages, ranging from tiny SOT-23 to large TO-220, and they have drastically different thermal characteristics. How is the part mounted? What is the ambient temperature? What is the velocity of air flow around the part (if any)? All of these factors, and more, would have to be taken into account to arrive at any meaningful assessment of whether a design is problematic.

WAYYYY too complicated. Far better to just report the part's power dissipation, and let the designer render judgement.
 

Thread Starter

Aleph(0)

Joined Mar 14, 2015
597
@Aleph(0) --- Further to study/investigation of said behaviour, please draft an example then 'up' the .asc file to this thread - from which I may post screen captures of simulations for the benefit of members w/o an Ltspice installation:)
HP I can't get upload to work w/o flash so I emailed .asc to your home addy so plz post it for me with screen shots? Tnx:cool:!
 
HP I can't get upload to work w/o flash so I emailed .asc to your home addy so plz post it for me with screen shots? Tnx:cool:!
Received! -- I will post it (along with simulation plots of the circuit using both the default and standard semiconductors) this evening -- You're right! The behaviour of the 'default' diode is bizarre!:confused:

Best regards
HP:)
 
Hello @Aleph(0) , et al

@Aleph(0) - RE: The default diode -- As you may recall the 'proclivities' of the (LtSpice) 'Default Diode' (among other Spice topics) were addressed last autumn ON THIS THREAD -- Please re-read the linked thread, should you yet have questions I'll happily post your Default Diode study schematics for discussion here:)

RE: The Default BJT --- That's one on me too!:confused::oops:
Inasmuch as your (ahem, our) confusion in this regard stems from consideration of a circuit posted to the "EHT PS Design And Construction" thread - I'll merely link said resource in the following...

To summarize your (and, now, my:oops:) question:
The real-world circuit represented by the attached schematic and ".asc" file operate well-nigh exactly as simulated using 2n3773s and closely so with 2n3055s -- but will simulate correctly only with the 'default' NPN BJT
(Please note that although LtSpices' library does not contain the 2N3773, the rather similar 2N3055 is 'available') -- Based upon comparative simulation, it seems LtSpice grossly underestimates the gain of the 2n3055...

Hence the question: Why is the Default NPN model more 'realistic' than the model of an appropriate real device?:confused:

Many advance thanks for any info/insight!!! -- I'm not too proud to confess that my-own desire for 'Spice literacy' is equal to Aleph's:)
:cool:

Very best regards
HP

Shown below is the schematic and correct simulation results using LtSpice Default NPNs
 

Attachments

Top