TINA/Spice/TLC2262: Some questions about TINA simulation in transient analysis and AC analysis

Haoyang Zhang42

Part Number: TLC2262
Other Parts Discussed in Thread: TINA-TI, , OPA172, LF156

Tool/software: TINA-TI or Spice Models

Hi,

I am now using TINA to simulate the behavior of an op amp TLC2262. But the result of AC analysis and transient analysis is different.

1, In the first case, it is ac analysis which operates between 1 to 500kHz and from the result below, the amplitude of the output waveform is increasing with the frequency.

2, But when it comes to transient analysis with a 1V input at 500kHz, the amplitude is about 200mV which is a conflict with the result of ac analysis who has 650mV at 500kHz.

Could anyone explain to me why the result behaves like this?

Thank you!

Best regards,

Haoyang

over 6 years ago

0 Haoyang Zhang42 over 6 years ago

Prodigy 180 points

And here is the result of the second case:

My simulation circuit is also attached here.TLC2262.TSC

0 Ron Michallick over 6 years ago in reply to Haoyang Zhang42

TI__Guru*** 145996 points

Haoyang,

Gain is measured with virtually no signal amplitude, (small signal gain). Also the top scale is not dB it is (0.5 to 0.63) V/V result.

I tried a +/-1uV transient sine wave and I saw 1.26uV/2uV = gain = 0.63 V/V

So it works just fine. (other than saying "dB")

When I ran AC gain sweep, I got -6dB to -4dB (0.5V/V to 0.63V/V)

7041.TLC2262.TSC

0 Pete%20Semig over 6 years ago in reply to Haoyang Zhang42

TI__Mastermind 25795 points

Hello Haoyang,

Sorry for the delay. Many people on vacation because of weekend and New Year holiday.

First, please understand the TLC2262 is a 16V device. You cannot apply +/-15V (30V) to device.

When I change supply voltage to +/-8V, simulation has same behavior. When I replace TLC2262 device with ideal op amp, behavior is normal (gain is 0.5V/V and rolls off with open-loop gain).

Therefore I suspect an issue with the model. Please understand that the device and model are approximately 25 years old.

You should also be aware of slew rate. Given a signal that is 1Vp (2Vpp) at 500kHz the slew rate of the device should be at least 3.14V/us. I recommend at least doubling that and looking for devices with a SR of 6V/us or greater.

Therefore I suggest that you evaluate the OPA172. It is a wide-supply device with sufficient bandwidth and SR. Since it is a newer device the model is more robust. Please see attached.

Note that I removed some of the additional features you included in your design (cap load, for example). Of course you can add these in at your convenience.

Also, for more information on op amps including slew rate and op amp stability we have an excellent series of videos at http://www.ti.com/precisionlabs

/cfs-file/__key/communityserver-discussions-components-files/234/haoyang_5F00_00.TSC

0 Haoyang Zhang42 over 6 years ago in reply to Pete%20Semig

Prodigy 180 points

Hi Pete,

Thank you for your reply and it solve my question. And may I ask you another question about the input capacitor on the datasheet? If it doesn't mention if it is a common or differential capacitor, like LF156, which one it should be?

BR,
Haoyang

0 Pete%20Semig over 6 years ago in reply to Haoyang Zhang42

TI__Mastermind 25795 points

Hello Haoyang,

Please refer to Figure 43 on page 23 (and the explanation at the top of page 24) in the data sheet. It shows the input capacitance as common-mode.

Simulation, hardware & system design tools

Simulation, hardware & system design tools forum

TINA/Spice/TLC2262: Some questions about TINA simulation in transient analysis and AC analysis