OPA171: OPA171 SPICE model internal nodes

Josef Rypar47

Part Number: OPA171
Other Parts Discussed in Thread: TINA-TI

Hello,

during simulating open-loop characteristics the OPA171 in simple inverting configuration I found different results when using TINA-TI and LTSpice. After some investigation I found potential discrepancy in the OPA171 SPICE model (Final 1.1, 2019).

It seems that the name of the internal node "en_n" is used inconsistently. In some cases the "en_n" node is replaced with "N049" node but not everywhere. Here are the suspicious lines:

C_DIFF en_p N049 3e-12
C_CMn N049 MID 3e-12
C_CMp MID en_p 3e-12

R52 MID en_p R_NOISELESS 1T
R53 N049 MID R_NOISELESS 1T

R34 en_p IN+ R_NOISELESS 1e-3
R35 N049 IN- R_NOISELESS 1e-3

Xi_np en_n MID FEMT_OPA171 //looks like here should be "en_p"
Xi_nn N049 MID FEMT_OPA171

Could you please verify the above lines and overall correctness of the OPA171 SPICE model?

over 4 years ago

0 Former Member over 4 years ago

Hello Josef,

Would you please specify what you mean by "different results." How different exactly?

Depending on the severity of the discrepancy, it could be a variety of things including simulation settings. I don't think it's a mistake in the SPICE model as it's been in use for a while. But, we can dig into this some more if need be.

Let me know your results and we can go from there.

Best regards,

Daniel

0 Josef Rypar47 over 4 years ago in reply to Former Member

Prodigy 240 points

Hello,

I've prepared a comparison simulation to demonstrate, see attached zip file.

My simulation was based on the SBOM442C.TSC test circuit. I've modified the circuit by adding 1TH inductor and 1TH capacitor as per the training video session https://training.ti.com/ti-precision-labs-op-amps-stability-spice-simulation

The simulation worked as expected.

Then I built the same circuit in LTSpice and followed their recommendation on the open loop analysis setting. This is to break the feedback loop at the inverting input and insert the small signal AC source there. In this case I got identical curves up to cca 100kHz but then the gain and phase started to roll off after 100kHz and ended at deep notch at 3MHz and then returning back.

I then tried to break the loop at the opamp output and insert the AC source there. In this configuration the simulation was nearly identical to the TINA results, the notch was gone.

The presence of the notch at the 3MHz brought me to the idea that there might be something wrong with the input capacitance definition in the OPA171 model. When adding a small capacitor (cca 10pF) between inverting input and ground the notch has moved in frequency which is the reaon why I started to investigate the SPICE model definition.

I'd like to understand where is the root cause of this discrepancy. I just wan't to double check that the OPA171 simulation model is really correct which is one half of the investigation. The second is a verification of the LTSpice operation correctness.

Hope you will be able to open and run the attached simulation.

Thank you.

Josef Rypar

OPA171_Simulation_Comparison.zip

0 Former Member over 4 years ago in reply to Josef Rypar47

Hi Josef,

Thanks for your detailed explanation and apologies for the delay in response.

It looks like you have properly broken the loop at the output in the TINA sim for a stability analysis. From this, we can draw information regarding the feedback factor, loaded AOL, and the AOL*Beta factor which is crucial in determining the stability of the amplifier. For simpler, single-feedback setups, the simplicity of this method is appealing.

Now when you open the loop at the input, you need to ensure that the circuit maintains a proper DC biasing point while the AC signal sees the open loop. Since the common mode is 0V, setting the DC voltage of the amplifier to 0 may satisfy this requirement. However, I see a couple of potential issues.

First, is the AC source injecting a signal into only the input of the amplifier? I'm not familiar with the LTSPICE environment, but you would not want to be injecting a signal into the output of the amplifier. I think you're fine here, but it is something to point out.

Second, the thing you need to take care of when breaking the loop at the input is that you disconnect the input capacitance of the amplifier from the feedback loop. This affects your AC response. You can compensate for this through the addition of discrete capacitance. However, I recommend just breaking the loop at the output, when possible, because it avoids the issue altogether and it is one less thing to remember.

There is an explanation about breaking the loop at the input in this presentation. I would recommend you use the same setup in the two simulators. As you noted, when you broke the loop at the output in LTSPICE, the notch disappeared. Ultimately, the technique behind how to break the loop is really based upon loop theory and not which simulator you are using.

Let me know if you have any further questions on this topic.

Regards,

Daniel

0 Josef Rypar47 over 4 years ago in reply to Former Member

Prodigy 240 points

Hi Daniel,

thank you for your thorough answer. I believe that the difference really can be caused by the input capacitance that was disconnected from the feedback network by inserting stimulus to the negative input of the opamp.

Then it looks like the OPA171 spice model is ok. Can you just comment on using node name N049 instead of en_n?

Thanks and regards,

Josef

0 Former Member over 4 years ago in reply to Josef Rypar47

Hi Josef,

Happy to hear we were able to get the simulation result issue resolved.

As for your question regarding the node names, I've checked with the author of the model and everything is fine. The node names may just seem a little strange, but they are in place for some internal noise modeling.

Regards,

Daniel

Amplifiers

Amplifiers forum

OPA171: OPA171 SPICE model internal nodes