THS3491: THS3491DDA spice model

Shota Mago

Expert 6580 points

Part Number: THS3491
Other Parts Discussed in Thread: OPA828, THS3001, OPA684

Hi team,

I found anomaly on spice model.

I simulated sink/source current as attached "THS3491 sink_source".
But I think current direction of I_VN should be opposite.
I simulated similar circuit with other opamp like OPA19x, OPA828 etc. and they showed result what I expected.
Is this just a problem of spice model?
I also simulated CMRR of THS3491 but it only shows 39dB as attached THS3491_CMRR whereas datasheet describes it's 75dB at typ.
I attempted to simulate CMRR with THS3001 and it showed similar value to its datasheet.
Is this also a problem of spice model?

Best regards,

Shota MagoTHS3491 sink_source.TSC

over 3 years ago

0 Shota Mago over 3 years ago

TI__Expert 6580 points

THS3491 CMRR.TSC

0 Hasan Babiker31 over 3 years ago in reply to Shota Mago

TI__Genius 15555 points

Hello Shota,

I will look into this issue further and get back to you.

Best,

Hasan Babiker

0 Shota Mago over 3 years ago in reply to Hasan Babiker31

TI__Expert 6580 points

Hi Hasan,

Noted.

I'm looking forward to hearing back from you soon.

Best regards,

Shota Mago

0 Hasan Babiker31 over 3 years ago in reply to Shota Mago

TI__Genius 15555 points

Hello Shota,

I agree with you on the matter of the quiescent current, there is an issue with the current direction. In regards to the CMRR of the THS3491, I agree that the CMRR is lower than that of the datasheet, however not to the degree to which you have simulated. One issue with measuring CMRR with the method that you have described is that Zout will interact with R1 which will give you a non-perfect difference amp configuration (you can think of Zout as a series resistor with R1).

Because of this, one way to get a more accurate CMRR measurement would be to increase your resistor values, however, these larger resistors will begin to interact with the input capacitors of the amplifier to give you an inaccurate result. So a solution you can use to fix both problems is attached below:

1425.THS3491 CMRR.TSC

Using this method I am measuring CMRR of 62dB at DC. Overall though, I would trust the measured CMRR of the datasheet rather than what is found in the spice model when it comes to design considerations.

Best,

Hasan Babiker

0 Michael Steffes over 3 years ago in reply to Hasan Babiker31

Guru 47485 points

Well Shota,

The CMRR for a CFA arises from the buffer gain across the inputs being slightly <1. THe Buffer gain in the THS3491 is very close to 1.0000 due to the very high output impedance current sources driving the buffer transistors. The previous highest CMRR CFA was the OPA684 with a closed loop input buffer stage.

In any case, your test ckt shows low CMRR because the V+ input impedance is in parallel to your shunt 1kohm.

If I isolate that with a dependent source, get a lot better results

Hasan, I am not sure you want the dependent voltage source on the inverting node - have you not broken the current feedback?

0 Shota Mago over 3 years ago in reply to Michael Steffes

TI__Expert 6580 points

Hi Hasan, Michael

Thanks for your helpful comments.

As for CMRR, I understood that modifying test circuit would make it possible to get more accurate result.

Meanwhile, Iq direction is a bug of spice model.

Do you have plan to fix it and re-publish on TI.com?

Best regards,

Shota Mago

0 Michael Steffes over 3 years ago in reply to Shota Mago

Guru 47485 points

I don't know about the model,but I did just look at the THS3491 V+ input impedance, only 50kohm which is why putting it in parallel with 1kohm gave you 980ohm termination on that path and poor apparent CMRR in sim.

0 Shota Mago over 3 years ago in reply to Hasan Babiker31

TI__Expert 6580 points

Hi Hasan,

I understood that CMRR can be simulated more accurately by changing test circuit.

But issue of current direction is inherent problem of spice mode.

Do you have plan to fix this issue?

Best regards,

Shota Mago

0 Hasan Babiker31 over 3 years ago in reply to Michael Steffes

TI__Genius 15555 points

Michael,

Thank you, the circuit I attached is definitely breaking the current feedback loop. That was an oversight on my part.

Shota,

At the moment, there is no plan to update this model. Note that the model doesn't specify accurate results in regards to Iq. Parameters that the THS3491 model is designed for include: "BW for G = 5 V/V, Slew rate, Noise, VOUT versus IOUT ,CMRR, PSRR, Enable time, Disable Time, VOS, IIB, VOH, VOL"

Best,

Hasan Babiker

0 Shota Mago over 3 years ago in reply to Hasan Babiker31

TI__Expert 6580 points

Hi Hasan,

Okay, I understood.

Thanks for your quick support!

Best regards,

Shota Mago

Amplifiers

Amplifiers forum

THS3491: THS3491DDA spice model