LM311 SIMULATION MODEL

[jfitzen]

The model for LM311 used in PSpice and several other simulation programs do not function according to the Data sheet from National Operational Amplifiers
Databook. Does anyone know were I can find a working model?
JFitzen

 

[crust]

What do you mean by does not work as described? Can you post the spice model, and why you feel it does not function.

 

[crust]

I received the spice model you PM'd me. It looks ok, but uses some directives that are no longer used in spice3 (which might be why your model did not work correctly). In any case, I tried a model that I had in a hysterisis configuration, presumably for a tachometer circuit since that seems to be asked about 1/week on this board. Here is the model (sorry if the tabs do not line up).


*-----------------------------------------------------------------------------
* connections: non-inverting input
* | inverting input
* | | positive power supply
* | | | negative power supply
* | | | | open collector output
* | | | | | output ground
* | | | | | |
* | | | | | |
.subckt LM111 1 2 3 4 5 6
*
f1 9 3 v1 1
iee 3 7 dc 100.0E-6
vi1 21 1 dc .45
vi2 22 2 dc .45
q1 9 21 7 qin
q2 8 22 7 qin
q3 9 8 4 qmo
q4 8 8 4 qmi
.model qin PNP(Is=800.0E-18 Bf=833.3)
.model qmi NPN(Is=800.0E-18 Bf=1002)
.model qmo NPN(Is=800.0E-18 Bf=1000 Cjc=1E-15 Tr=118.8E-9)
e1 10 6 9 4 1
v1 10 11 dc 0
q5 5 11 6 qoc
.model qoc NPN(Is=800.0E-18 Bf=34.49E3 Cjc=1E-15 Tf=364.6E-12 Tr=79.34E-9)
dp 4 3 dx
rp 3 4 6.122E3
.model dx D(Is=800.0E-18 Rs=1)
*
.ends


Here is the plot showing my results with this model -- in this case, I have added 250mV of noise to the input to show the hysterisis working.