How to generate impulse response in pspice

Hi! I am using vpulse source in order to extract the impulse response of a circuit. I use
V1=0
V2=1Meg
TR=1n
TF=1n
PW=1u
However, the simulation pauses and the following window appears. What should i do?

What happens if you click "OK & Resume Simulation"?

The same window appears again

You didn't report the error message that appears before the runtimes settings dialog...

I am sorry, you are right FvM. I get these messages:
ERROR(ORPSIM-15138): Convergence problem in transient analysis at Time = 1.001E-06.
These supply currents failed to converge:
I(E_READOUT_E1) = -6.022mA \ -6.015mA
ERROR(ORPSIM-15660): These devices failed to converge
X_READOUT_U1.Q_Q5
X_READOUT_U1.Q_Q9
X_READOUT_U1.Q_Q14
X_READOUT_U1.Q_Q12
X_READOUT_U1.Q_Q11
ERROR(ORPSIM-15661): 5 of 5 errors shown. See output file for complete list
INFO(ORPROBE-3185): Simulation paused

Can i ask you something else? Can i use these values
V1=0
V2=1Meg
TR=1n
TF=1n
PW=1u
with a pulse source in the input of OPA 657(commercial opamp, pspice model) with a negative feedback of course?
Thanks in advance

Your problem is with convergence. Go to the Spice Analysis (Edit Simulation Command) and try selecting the "Skip Initial Operating Point" and/or the "Start External DC Supply Voltage at 0V" to see if that helps. If not try reducing the accuracy of the parameters in the "Spice" panel of the Tools\Control Panel window by a factor of ten.

A V2 value 1 million volts should not be needed for an adequate impulse response signal. Try a value of perhaps 10V to start. You can vary the value to see if affects the output response. When you find little change in the response then you know going to a higher voltage will have no significant effect on the result.

analogpr, which max. time step did you select (if any?) for the TRAN simulation?

If your circuit doesn't attenuate 1Meg volts to a level within the OP ratings, no meaningful simulation results can be expected. What are you trying to achieve?

max step size= 0.1u

- - - Updated - - -

I just want to compare the impulse response of an ideal filter with the impulse response of a filter realized by real opamp

analogpr said:

I just want to compare the impulse response of an ideal filter with the impulse response of a filter realized by real opamp

Click to expand...

And what do you expect to get at the opamp output (real model with supply limits) with such a huge input signal ? Impulse response?

You cannot get an impulse (zero width, zero risetime). It
is an idealization.

You could make your source properties "good enough" but
this can challenge the simulator's ability to keep up, as
you see.

Setting minimum timestep lower than risetime would help
solving, but make runtimes unacceptable perhaps. You
may instead perfer to:

- tighten transient voltage and current tolerances
- increase iteration limits for transient by the same
factor that you tightened tolerances (rough guess)
- select a numerical method that converges better
than the default one (Euler, TrapGear2)

Now what "good enough" is, wants some thought as
well. You probably don't need to challenge a 1MHz
op amp with sub-nS risetimes and pulse widths, and
you don't need to feed a 5V op amp a 1kV input
amplitude either. What you want is enough harmonic
content that you can see what you need to see,
within constraints of linear input amplitude range
and so on - ideal filter response being a relevant
point of comparison, only if what you're comparing
is operating linear (or maybe you want to know that
it indeed is - but that still needs you to make it so,
or try).