how do I specify a different operating temperature for a specific component instead of it applying it to all?
.TEMP -32 for example is for all the components, but I would like to specify that a DIODE is at like -100 C for example, while every one else is at 38c et..
Jamie
In PSpice, it's specified in the model card, and can be parameterized.
I would expect LTspice to be similar. ...Jim Thompson
-- | James E.Thompson | mens | | Analog Innovations | et |
Something like this: Ctrl-right click on the diode symbol to get the full edit box, where you can enter the {T} parameter.
You can set T to whatever you want, or step it. It will override the global temperature for that component only.
I'm not sure how good the provided models are. There aren't any with Tikf, Trs1, and Trs2 set, and the LTspice default for all those is zero.
Version 4 SHEET 1 880 680 WIRE 240 32 48 32 WIRE 240 48 240 32 WIRE 48 96 48 32 WIRE 240 176 240 128 WIRE 48 272 48 176 WIRE 144 272 48 272 WIRE 240 272 240 240 WIRE 240 272 144 272 WIRE 144 288 144 272 FLAG 144 288 0 SYMBOL schottky 224 176 R0 WINDOW 123 24 76 Left 2 SYMATTR InstName D1 SYMATTR Value 1N5819 SYMATTR Description Diode SYMATTR Type diode SYMATTR Value2 temp={T} SYMBOL res 224 32 R0 SYMATTR InstName R1 SYMATTR Value 1k SYMBOL voltage 48 80 R0 WINDOW 123 0 0 Left 2 WINDOW 39 0 0 Left 2 SYMATTR InstName V1 SYMATTR Value 10 TEXT 312 96 Left 2 !.step param T -100 150 5 TEXT 312 120 Left 2 !.op
"For a successful technology, reality must take precedence over public relations, for nature cannot be fooled." (Richard Feynman)
As I've previously opined, LTspice tends to provide overly optimistic models... as Fred pointed out, many parameters are ignored or defaulted. If I were you I'd pull models down from the web rather than using the "canned" versions. ...Jim Thompson
-- | James E.Thompson | mens | | Analog Innovations | et |
Ok, the optional menu allowed me to enter TEMP -32 in a spice line, which resolved that problem..
I've been working on a noise problem that uses signal diodes and these diodes are subjected to cold temperatures. One diode gets a different temp than the other and I use these to form a bridge.
The signal is pulsed and after applying this TEMP parameter I can now see where the possible problem is.
It seems that the diode increases temperature at the junction that takes up 250 ms, according to spice, to level out. This changes the Vf during that time..
So I shorten the pulse down to 10 ms and I don't see this any more.
We'll have to apply this in real life to see if this helps. We are trying very hard not to use much for filtering so that we can maintain response time.
It's possible Ltspice is giving me some bogus numbers, i've always been partial to bench testing over sims.
Thnx Jamie
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.