LTspice model for TL051/061/071/081 or other single OP amp with offset adjust?

[Greybeard]

I'm searching for LTspice model for TL051 (TL061/071/081) or other single OP amp with offset adjustment pins.

I only found this one without (TI):

Code: [Select]

* TL051 OPERATIONAL AMPLIFIER "MACROMODEL" SUBCIRCUIT
* CREATED USING PARTS RELEASE 4.01 ON 04/12/89 AT 09:57
* (REV N/A)      SUPPLY VOLTAGE: +/-15V
* CONNECTIONS:   NON-INVERTING INPUT
*                | INVERTING INPUT
*                | | POSITIVE POWER SUPPLY
*                | | | NEGATIVE POWER SUPPLY
*                | | | | OUTPUT
*                | | | | |
.SUBCKT TL051    1 2 3 4 5
*
  C1   11 12 3.988E-12
  C2    6  7 15.00E-12
  DC    5 53 DX
  DE   54  5 DX
  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 2.875E6 -3E6 3E6 3E6 -3E6
  GA 6  0 11 12 292.2E-6
  GCM   0  6 10 99 6.542E-9
  ISS   3 10 DC 300.0E-6
  HLIM 90  0 VLIM 1K
  J1   11  2 10 JX
  J2   12  1 10 JX
  R2 6  9 100.0E3
  RD1 4 11 3.422E3
  RD2 4 12 3.422E3
  RO1 8  5 125
  RO2 7 99 125
  RP    3  4 11.11E3
  RSS  10 99 666.7E3
  VB    9  0 DC 0
  VC    3 53 DC 3
  VE   54  4 DC 3.700
  VLIM  7  8 DC 0
  VLP  91  0 DC 28
  VLN   0 92 DC 28
.MODEL DX D(IS=800.0E-18)
.MODEL JX PJF(IS=15.00E-12 BETA=185.2E-6 VTO=-1)
.ENDS
Can anybody help?

[moffy]

I looked around and couldn't find any SPICE models with the offset adjust pins, but then SPICE doesn't do offsets well because all the same transistors are the same, no variation in temp or gain etc.

[MariuszD]

Spice models are always simplified and inaccurate for several reasons. A realistic model would significantly slow down the simulation. Creating a realistic model is work for which no client pays anyone. Companies do not want their confidential information to leak thru this channel, so they deliberately degrade the accuracy of the models. A complicated model will contain errors just like any non-trivial program. Recently, in another topic, we discussed the  simulation with OPA2992. OPA2992 has a very complex model with 500 lines of text. The header described that it simulates as many as 24 parameters, and unfortunately, it turned out to be useless because something inside is oscillating. Most models, like the one you presented, are behavioral models; there isn't a single transistor inside your TL051. What applications would an offset adjustment circuit have in such a circuit?

Describe which properties you want to test and in what configuration.
If you only want to test the offset adjustment, it can be done in another way.

[mtwieg]

Yeah it's not surprising that spice models don't include offset adjustment functions. But it is a shame, since there are valid reasons to have them (for example if they're used in some sort of auto-zeroing feedback system).

Someone on the LTspice yahoo group created a transistor-level circuit for the TL071. The files are actually attached to this diyaudio post. The model seems to roughly work, though I cannot attest to its accuracy. You could connect the offset adjust pins to the emitters of Q1 and Q2.

[Greybeard]

I looked around and couldn't find any SPICE models with the offset adjust pins, but then SPICE doesn't do offsets well because all the same transistors are the same, no variation in temp or gain etc.

I am aware that SPICE operational amplifiers do not exhibit offset, as all components are perfectly ideal.
However, I would like to see what happens in the simulation when I change certain settings—including the offset trim potentiometer—in an existing amplifier circuit.

Can the netlist from the opening post be converted into a schematic?

[moffy]

I looked around and couldn't find any SPICE models with the offset adjust pins, but then SPICE doesn't do offsets well because all the same transistors are the same, no variation in temp or gain etc.

I am aware that SPICE operational amplifiers do not exhibit offset, as all components are perfectly ideal.
However, I would like to see what happens in the simulation when I change certain settings—including the offset trim potentiometer—in an existing amplifier circuit.

Can the netlist from the opening post be converted into a schematic?

Yes, if you draw it out by hand and connect the components with the same node/net number. I am not aware of any automated software but there could be some. But doing it by hand wouldn't take long. You could manually draw it up in LTSpice, with a little effort.

[Greybeard]

I didn't mean drawing it by hand.
The original internal circuit consists of about 30 components, so I would prefer an automated tool.

Maybe this tool will do the job:
https://ltwiki.org/index.php?title=LTspice_Tools_and_Applications#How_to_convert_SPICE_Netlist_to_an_LTspice_schematic

[Greybeard]

Somehow, I managed to get SchBuilder to spit out the following:



After some manual sorting in LTspice, it looks like this:



I don't know exactly what is going on inside the various current and voltage sources of the simulation model yet, but as far as I can tell, it doesn't look too bad.

Compared to the circuit diagram in the datasheet:




Perhaps someone can tell me whether I can use nodes 11 and 12 of the model as offset adjustment pins N1 and N2.

[moffy]

A simplified schematic with some resistor values can be found here: https://www.flywing-tech.com/blog/the-ultimate-guide-to-tl072-op-amp/

[Greybeard]

I found an error in the generated .cir file from SchBuilder:

All the JFETs are drawn as P-channel types in TLspice schematic viewer, although the simulation models are P-channel ("MODEL JX PJF ...").
I will correct my TL051 schematic and will try to contact the autor of SchBuilder.

I also searched for TL072 schematic and found one with capacitor value ans some some different resistor values:


https://electronics.stackexchange.com/questions/72967/difference-between-differential-op-amp-and-comparator

What is the function zener diode? What zener voltage?
What standard P-CH-JFET and NPN/PNP BJT should I use for the subcircuit simulation?

[moffy]

The JFET connected to the zener is a constant current source, helps make the opamp voltage insensitive. The zener drives an npn transistor with emitter resistor which acts as a constant current source and drives 3 pnps, 1 for bias and 2 act as bias current sources. The voltage of the zener will be low as it and a few other components would set the minimum supply voltage that the opamp would work at.

[Greybeard]

TL051 model transformed to schematic (after N-channel to P-channel correction):