741 LTSpice model

[danny92]

Hi everyone,

Does anyone has the LM741/uA741 LTSpice models?
I need this models to do a school work.

Best regards,
Daniel

 

[RajkoM]

Hi everyone,

Does anyone has the LM741/uA741 LTSpice models?
I need this models to do a school work.

Best regards,
Daniel

It is very easy 😀

LTspice->Examples->Educational->LM741.asc

 

[jcx]

nobody makes them that poor anymore

nearly all spice op amp models are macromodels - use idealized controlled sources to aproximate the behavior of a given op amp

so you need to know what detail is needed and determine if available models work

in the simplest case you can use "universal" op amp models where you can set a few basic op amp parameters like DC gain, GBW, Slew rate

in LTspice the UniversalOpamp2 is included in
C:\Program Files (x86)\LTC\LTspiceIV\examples\Educational folder

This demonstrates the use of the symbol UniversalOpamp2(improved version to the UniversalOpamp). You set the SpiceModel to be
higher to simulate more aspects of opamp behavior. Level1 is merely a transconductance working into an R||C and doesn't use power
from the supplies. Level2 adds slewrate, current and voltage limits. Level3a adds a second pole. Level3b adds a delay to the dominate
pole response. Noise is modeled at all levels.

 

[danny92]

Thank you very much.

 

[jazbo8]

Here is a discrete uA741 model from:
Microelectronic Circuits
Sedra & Smith
5th Edition

* Model for uA741 Op Amp (from EVAL library in PSpice)
* connections: non-inverting input
* | inverting input
* | | positive power supply
* | | | negative power supply
* | | | | output
* | | | | |
*
.subckt uA741 1 2 3 4 5
*
c1 11 12 8.661E-12
c2 6 7 30.00E-12
dc 5 53 dy
de 54 5 dy
dlp 90 91 dx
dln 92 90 dx
dp 4 3 dx
egnd 99 0 poly(2),(3,0),(4,0) 0 .5 .5
fb 7 99 poly(5) vb vc ve vlp vln 0 10.61E6 -1E3 1E3 10E6 -10E6
ga 6 0 11 12 188.5E-6
gcm 0 6 10 99 5.961E-9
iee 10 4 dc 15.16E-6
hlim 90 0 vlim 1K
q1 11 2 13 qx
q2 12 1 14 qx
r2 6 9 100.0E3
rc1 3 11 5.305E3
rc2 3 12 5.305E3
re1 13 10 1.836E3
re2 14 10 1.836E3
ree 10 99 13.19E6
ro1 8 5 50
ro2 7 99 100
rp 3 4 18.16E3
vb 9 0 dc 0
vc 3 53 dc 1
ve 54 4 dc 1
vlim 7 8 dc 0
vlp 91 0 dc 40
vln 0 92 dc 40
.model dx D(Is=800.0E-18 Rs=1)
.model dy D(Is=800.00E-18 Rs=1m Cjo=10p)
.model qx NPN(Is=800.0E-18 Bf=93.75)
.ends

 

[Mooly]

Is it just basic opamp circuits you are doing ?

I wouldn't imagine a school project needs you to set up a specific model. Can you not just use a basic opamp from the hundreds in the LTspice library. Try the LT1001

 

[VivaVee]

There is a complete 741 opamp circuit in the examples folder of LTSpice.
e.g. C:\Program Files (x86)\LTC\LTspiceIV\examples\Educational\LM741.asc

 

[danny92]

Hi everyone,
Thank you all for your help

Yes that's right in C:\Program Files (x86)\LTC\LTspiceIV\examples\Educational\LM741.asc directory, there is a circuit diagram of the internals of the LM741 (this circuit is good to better understand opamp topologies). I'm going to use jazbo's model. I'm doing a low power class C/B amplifier using the LM741 and BD139/140 pair it's a college work.

Best regards,
Daniel

 

[James26]

Hi,

I would like to use this 741 op amp as part of a circuit I am trying to simulate, how do I turn the subcircuit file in the examples folder into a symbol for use in my circuit ?

Thanks,
James