How to set/sweep individual device temperature?

[Anton]

I use the LTSpice. Setting, and sweeping, the temperature for the whole
circuit at one temp is not a problem.

I need to simulate a circuit at temperature, T1, while in this circuit
one device (diod or transistor) is set to another temp T2. Preferable I
would like to sweep the device temp T2.
Is it possible and in that case, how is this done?

Thanks in advance

Anton

 

Anton wrote:

I use the LTSpice. Setting, and sweeping, the temperature for the whole
circuit at one temp is not a problem.

I need to simulate a circuit at temperature, T1, while in this circuit
one device (diod or transistor) is set to another temp T2. Preferable I
would like to sweep the device temp T2.
Is it possible and in that case, how is this done?

Thanks in advance

Anton

You should probably also ask this question in the LT-Spice discussion
group at http://www.yahoogroups.com. But first you could go to the
group's Files area and download the file containing all of the message
titles, to see if that topic has been visited in the past. (You can
also do a full-text search of the messages themselves. But it's a bit
cumbersome, making the file with the titles useful.)

Good luck.

Regards,

Tom Gootee

 

[Mike Engelhardt]

Anton,

I use the LTSpice. Setting, and sweeping, the temperature for
the whole circuit at one temp is not a problem.

I need to simulate a circuit at temperature, T1, while in this
circuit one device (diod or transistor) is set to another temp
T2. Preferable I would like to sweep the device temp T2.
Is it possible and in that case, how is this done?

Here's the idea on the netlist level:

*
D1 a 0 D temp={t}
I1 0 a 1m
D2 b 0 D
I2 0 b 1m
..step param t -55 125 5
..op
..model D D
..end

The temperature of diode instance D1 is swept from -55 to 125 degrees
in 5 degree increments. Diode D2 is there to illustrate that the
rest of the circuit is not temp swept in this.

To do this on the schematic level, control right click on the diode
body and add "temp={t}" to one of the empty attribute fields after
the diode model name which is simply "D". Below is a schematic
that shows that.

--Mike

--- temp.asc ---
Version 4
SHEET 1 880 680
WIRE -16 192 -16 160
WIRE -16 320 -16 272
WIRE 112 160 -16 160
WIRE 112 208 112 160
WIRE 112 320 112 272
WIRE 256 192 256 160
WIRE 256 320 256 272
WIRE 384 160 256 160
WIRE 384 208 384 160
WIRE 384 320 384 272
FLAG 112 320 0
FLAG -16 320 0
FLAG 384 320 0
FLAG 256 320 0
SYMBOL diode 96 208 R0
WINDOW 123 24 100 Left 0
SYMATTR InstName D1
SYMATTR Value 1N4148
SYMATTR Value2 temp={T}
SYMBOL current -16 272 M180
WINDOW 0 24 88 Left 0
WINDOW 3 24 0 Left 0
SYMATTR InstName I1
SYMATTR Value 1m
SYMBOL diode 368 208 R0
SYMATTR InstName D2
SYMATTR Value 1N4148
SYMBOL current 256 272 M180
WINDOW 0 24 88 Left 0
WINDOW 3 24 0 Left 0
SYMATTR InstName I2
SYMATTR Value 1m
TEXT 112 392 Left 0 !.step param t -55 125 5
TEXT 112 424 Left 0 !.op