Forums

Basic LTSpice question

Started by Aussie May 17, 2017
I'm (very slowly) learning to play with LTSpice.

For temperature simulations do the models generally have a temperature 
dependent characteristics built in?

I can do a temp simulation with a Si diode and get some sensible output.

With feeding a fixed voltage from a resistor divider into an op amp 
follower I get no change in the output with temperature.

Am I correct in thinking the LT op amp models and the resistors have no 
temperature dependent parameters included?


Are temp dependent parameters only included for diodes and transistors?






Version 4
SHEET 1 880 680
WIRE 176 16 -32 16
WIRE -192 32 -384 32
WIRE -32 32 -32 16
WIRE 336 48 112 48
WIRE -192 112 -192 32
WIRE -32 128 -32 112
WIRE 176 144 176 16
WIRE 112 160 112 48
WIRE 144 160 112 160
WIRE 336 176 336 48
WIRE 336 176 208 176
WIRE 400 176 336 176
WIRE 144 192 -64 192
WIRE -240 208 -288 208
WIRE -192 208 -192 192
WIRE -64 208 -64 192
WIRE -64 208 -192 208
WIRE -384 224 -384 32
WIRE -288 240 -288 208
WIRE -192 240 -192 208
WIRE 176 256 176 208
WIRE -384 320 -384 304
WIRE -288 352 -288 304
WIRE -192 352 -192 320
WIRE -192 352 -288 352
WIRE -192 368 -192 352
FLAG 176 256 0
FLAG -32 128 0
FLAG -384 320 0
FLAG 400 176 out
FLAG -192 368 0
SYMBOL voltage -384 208 R0
WINDOW 123 0 0 Left 2
WINDOW 39 0 0 Left 2
WINDOW 3 -37 161 Left 2
SYMATTR Value 2.5
SYMATTR InstName V1
SYMBOL voltage -32 16 R0
WINDOW 123 0 0 Left 2
WINDOW 39 0 0 Left 2
SYMATTR InstName V2
SYMATTR Value 5
SYMBOL res -208 96 R0
SYMATTR InstName R1
SYMATTR Value 2K
SYMATTR SpiceLine tol=1 pwr=0.1
SYMBOL Opamps\\LT1012 176 112 R0
SYMATTR InstName U1
SYMBOL res -208 224 R0
SYMATTR InstName R2
SYMATTR Value 4K
SYMATTR SpiceLine tol=1 pwr=0.1
SYMBOL diode -304 240 R0
SYMATTR InstName D1
SYMATTR Value 1N914
TEXT -96 440 Left 2 !.temp 0 10 20 30 40 50
TEXT -96 392 Left 2 !.tran 0 1 0 0.01

On Wed, 17 May 2017 14:17:22 +0800, Aussie <aussie@none.com.au> wrote:

>I'm (very slowly) learning to play with LTSpice. > >For temperature simulations do the models generally have a temperature >dependent characteristics built in? > >I can do a temp simulation with a Si diode and get some sensible output. > >With feeding a fixed voltage from a resistor divider into an op amp >follower I get no change in the output with temperature. > >Am I correct in thinking the LT op amp models and the resistors have no >temperature dependent parameters included? > > >Are temp dependent parameters only included for diodes and transistors? > > >
Here's some stuff on resistors: https://www.electronicspoint.com/resources/managing-temperature-in-ltspice.18/ -- John Larkin Highland Technology, Inc lunatic fringe electronics
On Wed, 17 May 2017 14:17:22 +0800, Aussie wrote:

> I'm (very slowly) learning to play with LTSpice. > > For temperature simulations do the models generally have a temperature > dependent characteristics built in? > > I can do a temp simulation with a Si diode and get some sensible output. > > With feeding a fixed voltage from a resistor divider into an op amp > follower I get no change in the output with temperature. > > Am I correct in thinking the LT op amp models and the resistors have no > temperature dependent parameters included? > > > Are temp dependent parameters only included for diodes and transistors?
Different resistors (and caps, and inductors) respond to temperature differently. It's not just the magnitude of the change -- some have positive temperature coefficients, some negative, some have responses that are not straight-line with temperature. So if it matters, you'll need to model the temperature response of the components in question yourself. Hopefully the paper John cites goes into all that. -- www.wescottdesign.com
On Wed, 17 May 2017 14:17:22 +0800, Aussie <aussie@none.com.au> wrote:

[snip]
> >Am I correct in thinking the LT op amp models and the resistors have no >temperature dependent parameters included?
Yes for the resistor, yes for most of the OpAmps. The "Spice line" for a resistor is as follows, <...> means required [...] means optional R<name> <(+) node> <(-) node> [model name] <value> + [TC = <TC1> [,<TC2>]] [snip] If you examine the .asy for resistors, you'll find it has no TC's specified, but you can add them. ...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 | Thinking outside the box... producing elegant solutions. "It is not in doing what you like, but in liking what you do that is the secret of happiness." -James Barrie
On 17-May-17 9:50 PM, John Larkin wrote:
> On Wed, 17 May 2017 14:17:22 +0800, Aussie <aussie@none.com.au> wrote: > >> I'm (very slowly) learning to play with LTSpice. >> >> For temperature simulations do the models generally have a temperature >> dependent characteristics built in? >> >> I can do a temp simulation with a Si diode and get some sensible output. >> >> With feeding a fixed voltage from a resistor divider into an op amp >> follower I get no change in the output with temperature. >> >> Am I correct in thinking the LT op amp models and the resistors have no >> temperature dependent parameters included? >> >> >> Are temp dependent parameters only included for diodes and transistors? >> >> >> > > Here's some stuff on resistors: > > https://www.electronicspoint.com/resources/managing-temperature-in-ltspice.18/ > >
Thanks John. That's very useful - book marked!
On 17-May-17 11:31 PM, Tim Wescott wrote:
> On Wed, 17 May 2017 14:17:22 +0800, Aussie wrote: > >> I'm (very slowly) learning to play with LTSpice. >> >> For temperature simulations do the models generally have a temperature >> dependent characteristics built in? >> >> I can do a temp simulation with a Si diode and get some sensible output. >> >> With feeding a fixed voltage from a resistor divider into an op amp >> follower I get no change in the output with temperature. >> >> Am I correct in thinking the LT op amp models and the resistors have no >> temperature dependent parameters included? >> >> >> Are temp dependent parameters only included for diodes and transistors? > > Different resistors (and caps, and inductors) respond to temperature > differently. It's not just the magnitude of the change -- some have > positive temperature coefficients, some negative, some have responses > that are not straight-line with temperature. So if it matters, you'll > need to model the temperature response of the components in question > yourself. > > Hopefully the paper John cites goes into all that. >
Understood. Thanks Tim. PS - I hope you enjoy your new job & still find time to do the odd YouTube video.
On 18-May-17 12:16 AM, Jim Thompson wrote:
> On Wed, 17 May 2017 14:17:22 +0800, Aussie <aussie@none.com.au> wrote: > > [snip] >> >> Am I correct in thinking the LT op amp models and the resistors have no >> temperature dependent parameters included? > > Yes for the resistor, yes for most of the OpAmps. > > The "Spice line" for a resistor is as follows, > > <...> means required > [...] means optional > > R<name> <(+) node> <(-) node> [model name] <value> > + [TC = <TC1> [,<TC2>]] > > [snip] > > If you examine the .asy for resistors, you'll find it has no TC's > specified, but you can add them. > > ...Jim Thompson >
Thanks Jim. I was playing around trying to simulate the effect of temp on an op amp circuits Vio. Is there a way to add temp dependency to a voltage source? Then I could try putting that voltage source in series with say the +ve input to the op amp and simulate it that way. Maybe that would save me from getting in over my head poking around in the model definitions.
Tim Wescott wrote...
> > On Wed, 17 May 2017, Aussie wrote: > >> I'm (very slowly) learning to play with LTSpice. >> >> For temperature simulations do the models generally have a temperature >> dependent characteristics built in? >> >> I can do a temp simulation with a Si diode and get some sensible output. >> >> With feeding a fixed voltage from a resistor divider into an op amp >> follower I get no change in the output with temperature. >> >> Am I correct in thinking the LT op amp models and the resistors have no >> temperature dependent parameters included? >> >> Are temp dependent parameters only included for diodes and transistors? > > Different resistors (and caps, and inductors) respond to temperature > differently. It's not just the magnitude of the change -- some have > positive temperature coefficients, some negative, some have responses > that are not straight-line with temperature. So if it matters, you'll > need to model the temperature response of the components in question > yourself.
Then there's the serious issue that not all components on a PCB are at the same temp. We have junctions that are rather hot, from tough jobs they're doing, and other parts cruising along at ambient temp.
> >Hopefully the paper John cites goes into all that. >
-- Thanks, - Win
On 5/17/2017 9:47 PM, Aussie wrote:
> On 18-May-17 12:16 AM, Jim Thompson wrote: >> On Wed, 17 May 2017 14:17:22 +0800, Aussie <aussie@none.com.au> wrote: >> >> [snip] >>> >>> Am I correct in thinking the LT op amp models and the resistors have no >>> temperature dependent parameters included? >> >> Yes for the resistor, yes for most of the OpAmps. >> >> The "Spice line" for a resistor is as follows, >> >> <...> means required >> [...] means optional >> >> R<name> <(+) node> <(-) node> [model name] <value> >> + [TC = <TC1> [,<TC2>]] >> >> [snip] >> >> If you examine the .asy for resistors, you'll find it has no TC's >> specified, but you can add them. >> >> ...Jim Thompson >> > > > > Thanks Jim. > > I was playing around trying to simulate the effect of temp on an op amp > circuits Vio. > > Is there a way to add temp dependency to a voltage source? > Then I could try putting that voltage source in series with say the +ve > input to the op amp and simulate it that way. > > Maybe that would save me from getting in over my head poking around in > the model definitions.
If I'm not mistaken, there is a programmable voltage source component. You can drive that with the same parameter you are using to se the temperature and adjust the output to a voltage as you see fit. I haven't done this myself, so I don't recall which component would do this. It might be the voltage controlled voltage source. Or there might be a voltage source directly controlled by a parameter. -- Rick C
On 18-May-17 10:47 AM, rickman wrote:
> On 5/17/2017 9:47 PM, Aussie wrote:
>> >> I was playing around trying to simulate the effect of temp on an op amp >> circuits Vio. >> >> Is there a way to add temp dependency to a voltage source? >> Then I could try putting that voltage source in series with say the +ve >> input to the op amp and simulate it that way. >> >> Maybe that would save me from getting in over my head poking around in >> the model definitions. > > If I'm not mistaken, there is a programmable voltage source component. > You can drive that with the same parameter you are using to se the > temperature and adjust the output to a voltage as you see fit. I > haven't done this myself, so I don't recall which component would do > this. It might be the voltage controlled voltage source. Or there > might be a voltage source directly controlled by a parameter. >
Thanks Rick. I think I've found the voltage source but I'm not sure how to set it up. It gives you the option to enter a function, but it does not like the syntax. http://imgur.com/a/Edn0o I'm trying to add a voltage source with a slope of 5uV/&deg;C There are a few other configurable voltage sources but none appeared to have a temperature parameter.