If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

# OPA593: Unexpected pulse during steep load change

Part Number: OPA593

Dear Technical Support Team,

I'm evaluating steep load change with simulation(both PSpice model and TINA), then unexpected over 10V pulse occurred on output.

Does this behavior also occur with ic? Is this model problem?

See attached files.

■Condition

tr/tf 1us from 20mA to 180mA

noninverting configuration(1 V/V)

5Vdc input ⇒ 5Vdc output

■Tina TI

OPA593.tsc

Pspice for TI

Best Regards,

ttd

• Hi ttd-san,

The test is equivalent to apply 5Vdc at the input, pulse load in current at the output, Vout =5Vdc. This is equivalent to say what is output impedance of the OPA593 under the test condition.

If you perform the simulation above, you will see that OPA593's output impedance changes between -87.12dB (1Hz) to 51.76dB (peaked approx. 10MHz). At DC, the output impedance is approx. 44uΩ, and the output impedance is approx. 387Ω at 10MHz.

To generate 10V output voltage spike, the output impedance will be approx. 10V/0.180A = 55.5Ω (approx. 35dB @3MHz). The output voltage spike is expected dynamically during the rising and falling edges of the current pulses. This dynamic behaviors will show up in any feedback op amp or control system.

Best,

Raymond

• Hi TTD,

the simulation suffers a bit from abrupt changes of waveform of your piecewise linear input signal. Abrupt changes result in points of discontinuity of the first time derivative. A simulator does not like that. Also, the source impedance of your current source is assumed to be infinite, which means that the current shall flow entirely unhinderedly. But this is impossible because the output voltage is partially breaking down and the current just cannot flow then as simulated by the ideal current source.

So, if you really want to know what's going on, then you should also simulate the current source in detail and not rely on an ideal current source.

Having said this, I think it is nevertheless very very propable that you will see voltage spikes at the output of OPA593. Eventually not of the simulated amplitudes, but you will definitely see considerable voltage spikes.

Can you give details on the current source? What is making the load current to flow?

Kai

• Hi Raymond,

I'd like to minimize this spike, do you have any idea? 10us tr/tf helps the spike smaller than 1us.

However 1us tr/tv is required.

Datasheet is still preview and output impedance is TBD.

When OPA593 will be released(Active), these are changed from current things to new ?

I have OPA593EVM and will evaluate it.

Best Regards,

ttd

• Hi ttd-san,

The Vout voltage spike is resulted from sudden current load change at the output. Your current pulse load is a way to simulate the INA593's Vout spike conditions. Do I understand this transient event correctly?

If that is the case, please place TVS or zener at the output of INA593, if you are able to.

When the INA593's output transient event is occurred, DAC input at 2.5Vdc and Vout is already stabilized at 5Vdc.

Or you may place the schottk diodes at the output to steer the current to the supply rail. Assumed that you only need to have single supply rail for the application.

If the scope shot is the actual Vout voltage spike (voltage spikes may go higher up to 20Vpk), the following configuration may help. I am not 100% certain what the Vout transient conditions are from - my speculation is that you are concerned about the voltage spikes when INA593's Vout is experienced with current pulse transient events as simulated.

OPA593 Vout Current Steering 11142022.TSC

Best,

Raymond

• Hi TTD,

please elaborate what the current source "IG1" actually is. As I explained above you see in the simulation the behaviour of an ideal current source which can be highly different from what you have in the real circuit. Because of that it is highly impropable that the step response will make the output voltage of OPA593 exceed the supply voltages. This is absurd. An overvoltage can only develop in the case of an inductive kickback. But this would impy the existence of an inductance, which I do not see in your simulation.

So please tell what "IG1" is.

Kai

• Hi Raymond and Kai

I tried to evaluate it with OPA593EVM.

Unfortunately my electric load(KIKUSUI PLZ205W) settings up to 0mA > 200mA(2.7us) and 200mA > 0mA(1.7us).

Then spike didn't occur. Do you have OPA593EVM and more faster electric load?

P.S

Output of OPA593EVM has your diode you suggested.

Current source "IG1" means electric load

Best Regard,

ttd

Yellow: Output voltage

Pink: Current probe

• Hi TTD,

I think this simulation gives a more realistic result:

ttd_opa593.TSC

Kai

• Hi ttd-san,

Thanks Kai for the simulation!

If you want to test OPA593's output transient behavior, Kai is schematic is more realistic.

R2 or 2.5kΩ represent a nominal load. Then you parallel a low resisitive load, like R1 (5V/0.18A ≈ 28Ω) + fast electronic or contact switch in series with R1 load. The electronic switch will be turned on and off momentarily and you can monitor the rising and/or falling edge of pulse responses and behaviors from a power amplifier or control system.

Or you can remove R1 and switch, and replace with a programmable current source to perform similar current pulse load tests. Or keep R1 and place a programmable voltage source in series with the load (as simulated).

Generally, I only use resistive load or mimic the application's actual load conditions for the transient tests. Electronic load is a complex load, it may have some unwanted inductive and capacitive load behaviors that are difficult to manage. Sometimes, electronic load can oscillate as well under certain load conditions.